Printer Friendly

Comparison of Various Drag Reduction Devices and Their Aerodynamic Effects on the DrivAer Model.

Introduction

There has been growing interest in improving vehicular fuel efficiency due to global regulations on C[O.sub.2] emissions. The ever-tightening environmental regulations have proven to be obstacles to automobile manufacturers; therefore, research and development of high-fuel-efficiency vehicles should be promoted. Overall driving resistance, which affects the fuel efficiency, consists of aerodynamic drag, rolling resistance, acceleration resistance, and climbing resistance. The aerodynamic drag increases in proportion to the square of the driving speed, while the rolling resistance increases a little with speed. Therefore, the aerodynamic drag becomes greater than the rolling resistance beyond a particular driving velocity. Using the technical data of the Mercedes-Benz B-class as an example, aerodynamic drag exceeds rolling resistance at approximately 60 km/h [1]. Vehicles' maximum speeds have increased with better engine performance and road conditions, which is why aerodynamic drag has become more important than ever before. To reduce the driving resistance of a vehicle, it should have a light body and/or an aerodynamically designed shape.

In the Worldwide Harmonised Light Vehicle Test Procedure (WLTP) driving cycle, fuel efficiency has been shown to improve by approximately 3.3% when the vehicle mass is reduced by 10%, and it has been shown to improve by approximately 2.6% when the aerodynamic drag of a vehicle with an aerodynamic drag coefficient ([C.sub.D]) of 0.3 is reduced by 10% [2]. Changing materials or downsizing the engine are required to reduce the vehicle weight; however, this would lead to an increase in the vehicle price. Improving the exterior of the vehicle to an aerodynamic shape can be achieved with minimal costs, rendering it highly cost-effective for improving the fuel efficiency. The front of an automobile has a streamlined form, but its back has an angled bluff shape that is different from an aircraft wing. This causes highly complicated rear flow patterns such as vortices, eddies, downwash, upwash and mixed wake flows [1]. Controlling the rear flow of an automobile is a core technology for improving its aerodynamic performance.

There are two fundamental types of flow separation from the rear of a vehicle. If separation occurs at the edges that are perpendicular to the main flow, vortices develop with axes parallel to the separation lines. The shear layers behind the body interact to form a recirculation zone consisting of two vertically distributed contra-rotating vortices. This typical form of a "dead water" region common to two- dimensional bluff bodies also extends to the three-dimensional rear geometry of the vehicle. Conversely, if separation occurs at the intersection of the body quarter panel edge at a significant angle, with respect to the main flow, an induced vortex develops in a form of a counter-rotating vortex pair. Their axes are aligned in the longitudinal direction of the vehicle. These vortices are mainly observed in the passage to the rear window, which is called the c-pillar. They are superimposed on the mentioned cross vortices and change the pressure drag. The formation of a vortex implies energy loss in the flow and acts as a cause of induced drag, negatively affecting the vehicle aerodynamic characteristics. Notably, the vortex from the c-pillar merges with the downwash of the upper flow to form a pronounced longitudinal vortex pair in the wake region.

Many researchers have exerted considerable efforts to reduce automotive aerodynamic drag using flow control of the rear wake. Drag reduction methods of applying additional devices such as the spoiler and the wing are as follows. Bearman analyzed the effect of rear pressure rise by installing a flap behind a fastback model [3]. Additionally, a vertical strake was attached to the rear surface to induce a pressure rise, which has the effect of preventing the formation of longitudinal vortices. A spoiler is designed to improve stability under high-speed driving conditions by increasing the downforce, and may increase the aerodynamic drag [4]. However, it is also possible to find the optimal point at which [C.sub.D] is minimized by adjusting the length and height of a rear spoiler [1]. Schutz applied a roof spoiler and a side spoiler to reduce the [C.sub.D] of a commercial vehicle by 5-7 counts [5]. In the case of passive devices, only a description of the method and the effect of reducing the aerodynamic drag are being summarized as the shape of the vehicle becomes complicated. Additionally, analyzing the aerodynamic drag reduction mechanism does not provide a design guide for a general aerodynamic drag reduction device.

Since most of the current studies were performed on relatively simple models such as the Ahmed body or the SAE model, it is necessary to confirm whether the same effect can be obtained when applied to an actual vehicle. Additionally, it is difficult to systematically compare the aerodynamic improvement effects of individual devices due to the difference in the baseline models and flow conditions used in the study of flow control methods. Therefore, there is a need for research to compare the performance of various devices under equivalent conditions.

Approach

In this study, (1) different aerodynamic drag reduction devices are applied to the DrivAer model, which has similar geometrical characteristics to commercially available light-duty vehicles. The effects on the flow around the vehicle are analyzed numerically. (2) To reduce the c-pillar vortex and upper flow downwash, which are the main factors of the longitudinal vortex pair, the effects of various aerodynamic drag reduction devices are compared as shown in Figure 1 (vertical and horizontal plates). (3) The effect of each aerodynamic drag reduction device on the flow around the vehicle is analyzed, and the mechanism of the drag reduction effect is examined.

First, a baseline model analysis dealing with the flow field and surface pressure distribution is performed to select the types of aerodynamic drag reduction devices to be applied. The effect of each selected device on reducing the aerodynamic drag is analyzed through CFD analysis. By comparing the performance based on the design parameters of the aerodynamic drag reducing devices, the main design parameters for each aerodynamic drag reducing device which shows a positive effect are examined. The mechanism by which the aerodynamic drag of the automobile is reduced is considered using flow field analysis. Since the longitudinal vortex pair is clearly formed in the sedan configuration, the result of this study can be applied to the development of the actual vehicle.

Numerical Methods

Vehicle Model and Simulation Settings

The car model used in this study is the DrivAer model. The DrivAer model is a generic vehicle body developed at the Technical University of Munich for acquiring research results applicable to vehicle development. Its shape is based on two typical medium-class vehicles, the Audi A4 and BMW 3 Series [6]. The previously widely used Ahmed and SAE reference bodies are highly simplified geometries whose proportions diverge widely from those of production cars, making them difficult to utilize in road vehicle research. However, since the development of the DrivAer model reduces the difference in shape between the model car and the commercial vehicle, it is easy to apply the research results to vehicle development.

The DrivAer model has a fixed front body, and the greenhouse can be chosen from three forms: fastback, notchback, and estate back (Figure 2). The cross-flow velocities in the wake regions show the formation of vortices on each of the three models (fastback, notchback, and estate back), but it is less pronounced in the estate back than in the other two models. Additionally, in the estate back, the lower flow rises at the wake region, and the upper flow does not approach the ground but flows upward. In the case of the fastback, the tendency of the bottom flow to rise at the wake region is more pronounced than for the notchback, so the downwash of the top flow in the notchback can be observed strongly [7]. Therefore, various aerodynamic drag reduction devices are applied to the notch-back, which shows a flow pattern combining the downwash of the upper flow and the wake vortex. The basic shapes used in this study were the detailed underbody, mirrors, and wheels including spokes similar to those on commercial vehicles. The under hood flow including engine bay flow was not considered in this study. The influence of engine bay flow to drag reduction device is considered to be insignificant because the location of applied aerodynamic drag reduction devices is on the rear upper side of the vehicle. When the engine bay flow is considered, the quantitative analysis result, [C.sub.D], could be changed.

Open FOAM is used as a CFD analysis tool, which shows good agreement with experimental data in predicting the aerodynamic drag of automobiles [8]. Due to the bluff vehicle shape, the flow around the vehicle is unsteady, so a steady simulation cannot analyze the unsteady flow characteristics that occur in the actual driving situation. Many calculations are performed in this study to compare and analyze the effects of various aerodynamic drag reduction devices. The simulation results with respect to the grid levels and the analysis conditions are compared to determine the analysis condition that not only catches the wake pattern accurately but is also efficient. The steady simulation is performed using the SIMPLE algorithm implemented in Open FOAM simple Foam solver. The SIMPLE (Semi-Implicit Method for Pressure-Linked Equations) algorithm allows to couple the Navier-Stokes equations with an iterative procedure, velocity and pressure are treated in a sequential manner. The discretized momentum equation was solved to compute the intermediate velocity field and the pressure field computed by the pressure correction equation that exploits the discrete momentum equation to replace the velocity field in the continuity equation with a pressure term. Then the velocities were corrected on the basis of the new pressure field. For the unsteady simulation pisoFoam solver is used which using PISO (Pressure Implicit with Splitting of Operators) algorithm to solve the Naiver-Stokes equation in incompressible unsteady problem. The main differences from the SIMPLE algorithm are no under-relaxation applied, and the momentum corrector step is performed more than once. The solution of the steady simulation is applied as an initial condition of the unsteady simulation. The SST k-[omega] model, which is well known to predict flow separation in adverse pressure gradient conditions, is used as the turbulence model [9]. Other calculation conditions are summarized in Table 1.

Computational Domain and Boundary Conditions

The surface and volume grids for evaluation of the external vehicle flow are created using an unstructured grid. The dimensions of the computational domain are chosen such that the aerodynamic force is unaffected by the domain size. The cross section of the computational domain, shown in Figure 3, is 6L upstream, 13L downstream, and 9.5W on both sides of the vehicle. The height of the domain is 15H (L, W, H stand for the length, width, and height of the vehicle, respectively). Hence, the blockage ratio calculates to less than 0.3%, whereas it is 8% in the experiment [6]. A previous study of Peddiraju s simulation based on wind tunnel geometry showed that the drag force tends to be calculated to be about 3% larger when analyzed in the open domain [10]. The difference of 3% of the previous study was considered when comparing the numerical method. The study of comparing the aerodynamic drag reduction device was conducted according to the actual driving conditions of open domain. The entire domain comprises approximately 40 million volume meshes for fine grid and 25 million volume meshes for coarse grid. Grid independence tests have been performed using both grid types to find an appropriate grid level.

Because the focus of this study is the influence of drag reduction devices on the flow field, the meshes were refined near the vehicle, and in particular, at the rear to capture the clear structure of the rear wake including the c-pillar vortex and longitudinal vortex pair. In the refinement zone, the cell size is limited to 15 mm for the fine grid and 25 mm for the coarse grid to ensure the efficient and accurate capturing of all details of the flow phenomenon. The total height of the turbulence boundary layer is 6.78 mm based on the length of the vehicle and a driving speed of 140 km/h, assuming an infinitely wide flat plate. To capture the boundary layer, prism meshes are built up from the vehicle surface. Since high-Reynolds flows would require a highly resolved near-wall mesh, wall functions are applied in order to reduce the computational cost [8, 11, 12]. The thickness of the first boundary prism mesh is set equal to a y+ of 30, with the consideration of using the wall function. The total thickness of the prism meshes, composed of eight layers, is equal to 9.14 mm.

To simulate a vehicle driving on an actual road, the inlet boundary is set to 38.89 m/s of inflow toward the vehicle. The velocity corresponds to a Reynolds number of 1.26 x [10.sup.7] based on the vehicle length. Both sides and the upper boundary are set to a slip boundary condition. At the outlet boundary, zero pressure is imposed. The wheels have been modelled with Multiple Reference Frame (MRF). The MRF-zone is created like pieces of cake that encapsulate the area between the spokes of the rim [13]. It is important to ensure that MRF-zone is not expanded to the flow field dominated by high-velocity flow that is passing the side of the vehicle. This is because if the translational flow is perpendicular to the axis of rotation, it is not considered uniform in the reference frame. The angular velocity of the rotating wheel was set to 122.23 rad/s. This equated to the velocity of the ground which was set to the free stream velocity of 38.89 m/s. The rest of the vehicle is set to have stationary walls with a non-slip condition. The overall boundary conditions for the CFD analysis are shown in Figure 3. The conditions of the aerodynamic simulation are fully turbulent, with rotating wheels and moving ground, which implies that the turbulence intensity is high. The turbulence intensity at the inlet boundary is set to 0.1%, and the turbulence length scale to 10 mm with consideration of the free stream condition based on other numerical studies of ground vehicles [14].

The [C.sub.D] for a vehicle with various combinations of drag reduction devices is evaluated through a steady-state analysis. The reference area for calculating [C.sub.D] is the frontal projection area of the reference model for all cases. [C.sub.D] and the residual histories of the steady and unsteady simulation indicate that the aerodynamic drag fluctuates periodically even after the drag is within a stable range. The flow around the vehicle exhibits highly three-dimensional and nonlinear flow phenomena owing to its blunt shape. Kwak and Heft averaged the [C.sub.D] values after reaching a stable range to obtain the exact aerodynamic coefficient [6, 15]. 5,000 iterations are carried out in the steady simulation to ensure convergence. The aerodynamic coefficient and entire flow field for each analysis are averaged over the final 2,500 iterations. The time step size for unsteady simulation is set to 0.1 ms. Five seconds of physical time are simulated, and the aerodynamic coefficient and the entire flow field for each analysis are averaged over the final 4.5 seconds.

Grid Independence Test and Baseline Flow Pattern Analysis

Most automotive aerodynamic drag is due to the pressure drag caused by the low-pressure zone in the rear wake, and the induced drag resulting from the rear vortex [16]. To predict the effect of an aerodynamic drag reduction device, it is important to capture the changes in the flow pattern accurately when applying the aerodynamic drag reduction device. Therefore, a grid independence test was performed to select the appropriate grid level. Based on the baseline flow pattern analysis, the aerodynamic drag reduction devices to be applied were selected.

Observing the baseline flow pattern, the a-pillar and c-pillar vortices merge with the downwash from the upper flow of the car, forming a longitudinal vortex pair in the rear wake (Figure 4). This phenomenon causes the induced drag on the vehicle, and the vortex pair itself indicates energy loss in the flow. Therefore, it is important to prevent the vortex pair from developing or to dissipate it quickly to reduce the induced drag. Based on understanding the flow characteristics, aerodynamic drag reduction devices are designed to weaken the downwash from the upper flow, and prevent the formation or weaken the strength of the vortex pair.

The experimental results for the DrivAer model are compared with simulation results to verify the CFD code [6, 8]. The Reynolds number of a full-size vehicle driving at 140 km/h is 1.26 x [10.sup.7], which is different from the Reynolds number of 4.87 x [10.sup.6] for the wind tunnel test condition of Heft et al. However, as Heft et al. noted, even if the Reynolds number increases, it is known that there is little change in the [C.sub.D] value. In the verification process, the grid independence test is performed using the baseline model to determine the appropriate grid level and the simulation setting. Steady and unsteady analyses are performed using both fine and coarse grids, and the aerodynamic coefficients are compared with the wind tunnel test results as shown in Table 2. For comparison of the efficiency, the simulation times for each analysis are normalized by the steady calculation time when using the coarse grid.

Comparing the accuracy by grid level, the steady and unsteady analyses show additional errors of 1.7 and 3.4%, respectively, for the coarse grid relative to the fine grid. To visualize the wake region, the area in which the total pressure coefficient ([C.sub.P, total]) was less than 0.9 was regarded as the wake region. The wake regions at 3 m behind the vehicle are compared in Figure 4 where the rear wake is fully developed. The wake region of the coarse grid is wider than that of the fine grid in both the steady and the unsteady analysis. The wider wake region means that the energy loss is calculated to be larger than that of the fine grid due to the numerical dissipation in the coarse grid. It is obvious that the coarse grid is insufficient to calculate the aerodynamic drag as well as to identify the rear flow characteristics. The analysis using Spalart-Allmaras improved delayed detached eddy simulation (IDDES) on the coarse grid accurately calculated the aerodynamic drag coefficient than the unsteady analysis using the SST k-[omega] turbulence model using the same level of grid. However, the turbulence characteristics are completely different from those of other turbulence models, which is consistent with the results of Ashton [17]. The application of the IDDES turbulence model takes 9.2 times the computation time than the steady analysis using the SST k-[omega] turbulence model and does not fit the purpose of this study to analyze and compare various cases. The numerical analysis using various turbulence model of the DrivAer fastback model have been compared with the experiment [17]. The difference of the drag coefficient in the SST k-[omega] model is 2.3%, and the IDDES model shows a difference of 5.5%. In addition, Wang [18], which compared the results of high speed train slipstream analysis with various turbulence models, simulations show qualitatively consistent results with wind tunnel measurements for slipstream assessment and predicting [C.sub.D]. Therefore, the SST k-[omega] turbulence model was used in this study to quantitatively compare the aerodynamic drag coefficient. Additionally, for the detailed analysis of the aerodynamic drag reduction mechanism, which is the purpose of this study, the fine grid should be used because the wake patterns must be accurately analyzed and compared.

Comparing the results based on the analysis condition in the fine grid, the steady (black line) and unsteady (red line) analysis results show a similar rear flow structure. The [C.sub.D] difference is just one count, and both simulations have similar accuracy when considering the error due to numerical approximation. The computation time required for the unsteady analysis is approximately 7 times longer than for the steady analysis. Therefore, it is sufficient to analyze the performance of the aerodynamic drag reduction devices using a steady analysis if there is no significant difference in the flow field of current baseline simulation result and this will be discussed more as follows [19].

The surface pressure distributions of the upper center-line and side of the vehicle are examined for more accurate comparison. The pressure coefficient ([C.sub.P]) distributions of the steady and unsteady analyses using the fine grid are compared with wind tunnel test results in Figure 5. The surface pressure distributions of both the steady and unsteady analyses agree well with the experimental values. The slight [C.sub.P] disagreement at the roof of the vehicle is believed to be caused by the presence of measurement equipment in the wind tunnel experiment. Since most of the aerodynamic drag is caused by the pressure drag, the error in the roof does not affect the aerodynamic drag. In order to analyze the drag reduction mechanism of the aerodynamic drag reduction device, the entire flow field is averaged after the simulation reached a stable oscillatory condition. This was done to obtain a representative snapshot of the transient flow characteristics of the bluff shape of the vehicle. In order to obtain a more accurate snapshot, we performed averaging of fluid properties at every position in each iteration after a certain convergence of the solution. This is similar to analyzing typical flow characteristics by averaging the flow field at every time step at every location in the transient simulation [6, 15].

Figure 6 compares the results of the numerical analysis and the wind tunnel test results, which were obtained by measuring the pressure distribution on the rear windshield of the vehicle using 11 measurement points. Regardless of the analysis conditions, the surface pressure distribution and the trend agree well with the experimental data. In detail, however, there is some difference in the pressure in the center of the rear windshield. In the wind tunnel test, the equipment installed in the loop would have affected the measurement of the central pressure. In addition, since there are insufficient measurement points, the results are compared by interpolating the data between the measurement points. It is concluded that both the steady and unsteady simulation results of the surface pressure are in good agreement with the wind tunnel test results.

To determine accurate and efficient analysis conditions, the baseline analysis results for each grid level and analysis condition were compared with the experimental data. The result of the steady analysis using the fine grid is in good agreement with the wind tunnel test result and has the same accuracy as the unsteady analysis when the aerodynamic drag prediction accuracy and the surface pressure distribution are compared. For the efficiency of the study, all case studies were carried out under this simulation condition.

Results and Discussion

Various Types of Aerodynamic Drag Reduction Devices

Compared to the flow behind the previously widely used Ahmed body, that of the DrivAer model is highly complicated since the model was developed based on commercial vehicles. There are two typical characteristics of the flow around the DrivAer baseline model: the pressure drag due to the flow separation at the rear window and trunk end, and the induced drag due to the longitudinal vortex pair, which is created by the c-pillar vortex and downwash from flow over the model.

(1) A vertical plate is applied to the trunk lid and c-pillar to prevent the development of the vortex. It is a device to initially block the generation of the c-pillar vortex, to weaken the strength of the vortex pair at the rear of the vehicle, or to control the vortex that develops as it enters the wake. To suppress the downwash from the upper flow, (2) a horizontal plate is applied to the trunk end. It is designed to rapidly dissipate the wake vortex by suppressing downwash. The performance of three types of aerodynamic drag reduction devices were analyzed by adjusting design variables such as position, shape and length for each device. Comparing the performance of 15 cases, the aerodynamic drag reduction mechanism was analyzed and important design parameters were confirmed in designing the device.

In the case of automobiles, not only aerodynamic performance but also aesthetic design is a very important issue in vehicle exterior design. Considering this, it is essential that the aesthetics are not ruined when an aerodynamic drag reduction device is installed. All aerodynamic drag reduction devices are designed to be deployed only at high-speed driving conditions where the aerodynamic drag becomes greater than the rolling resistance, approximately over 100 km/h, while being hidden under low-speed driving conditions. This design takes into account the fact that the aerodynamic drag is proportional to the square of the vehicle speed, so aerodynamic drag is important only at high-speed driving conditions where the ratio of the aerodynamic drag to the total vehicle drag is large. Figure 7 shows the position and shape of the aerodynamic drag reduction devices applied in this study.

After modeling of the aerodynamic reduction device, the grid was densely created around the device. This is because the location of the aerodynamic drag reduction device will be installed where a complex flow phenomenon is expected to occur as the separation at the trunk end, or a region where the side flow and the upper flow combine to generate a vortex. Also, it is essential to use very fine grid elements because the shape of the aerodynamic drag reduction device is a rough plate shape without fillet. Horizontal plate and the vertical plate case was limited to the surface mesh size of the device with a maximum of 2.5 mm. Since the thickness of the device was modeled as 5 mm, at least two mesh elements were utilized on the device edges. After generating the surface meshes of the device, the boundary prism layer was added and the volume meshes were generated in the same manner as the reference model. Cases with aerodynamic drag reduction device were analyzed using more grid elements than the 40 million cells used in the reference model analysis.

The performance of each aerodynamic drag reduction device is analyzed using CFD at 140 km/h, which is a general high-speed driving condition. The aerodynamic drag reduction effects of each case with respect to type, parameter, and position are compared to the baseline in Table 3. The aerodynamic drag and lift improvements of all cases are summarized in Figure 7. In 15 cases using the horizontal and vertical plates, aerodynamic drag reductions were generally obtained, except in 4 cases. HP06, with a 150 mm plate behind the trunk, and VP04, with a 50 mm wedge on both sides of trunk lid, show aerodynamic drag reductions of 5.1% and 3.3%, respectively. The rate of aerodynamic drag reduction was less than 5%, which is low, because the DrivAer model is already aerodynamically well-designed. In the following two sections, each aerodynamic drag reduction device is analyzed in detail. The drag reduction effect is analyzed taking into account the mechanism expected from the design of the device. Additionally, wake patterns and characteristics are analyzed to identify the effective aerodynamic drag reduction mechanism.

Horizontal Plate

The horizontal plate was designed to weaken the downwash of the upper flow and to inhibit the formation of the longitudinal vortex pair in the rear of the car. The device extends a planar plate behind the top of the trunk for four lengths of 50, 100, 150, and 200 mm under high-speed conditions. To analyze the effect of the aerodynamic drag reduction device shape, triangle, tooth and saw tooth plates were compared with the plane shape for 50 mm and the length showing the biggest rate of drag reduction. The aim was to investigate the form that interacts with a longitudinal vortex pair made by downwash and thereby relieves its effect.

The Effect of Horizontal Plate Length To investigate the effect of length, the simple plane shape was analyzed by changing its parameters. Since the length of the trunk lid is approximately 300 mm, the maximum length of the horizontal plate is limited to 200 mm and the performance was studied by changing the length in 50 mm increments. The drag reduction is related to length, with an optimum value close to 150 mm (HP06) which shows 5.1% drag reduction. The reduction decreased to 1.0% when the length was elongated to 200 mm (HP10).

In the Figure 8, the rear surface pressure of the baseline shows that there are two areas of high pressure, which means that the wake consists of two rotating wakes. After the installation of the horizontal plate, the two high-pressure regions are merged, and as the length of the horizontal plate increases, the position of the high-pressure region moves upward. Since the vehicle is bluff-shaped, flow separation occurs and the separated flow merges at the dead wake end. The point where the upper and lower flow merge is called the free stagnation point. As the horizontal plate lengthened, the height of the free stagnation point increased compared to the baseline (Figure 8). This confirms that the horizontal plate weakens the downwash. As the downwash of the upper flow reduces, the lower flow past the rear bumper enters the wake region at an increasingly large angle to fill the dead wake. The pressure of the lower flow is lower than the upper flow, creating a low-pressure area in the rear of the vehicle and setting back aerodynamic drag reduction. Until the 150 mm plate was applied, HP06, the reduction of the vortex pair due to the downwash suppression was sufficient to overcome the adverse effect of the lower flow filling the wake area with low pressure. Therefore, the rate of aerodynamic drag reduction increased. However, the aerodynamic drag reduction effect of HP10 due to the downwash weakening is less than that of HP06 because the vortex pair was already relaxed with the application of the 150 mm plate. Additionally, due to the downwash of the upper flow, the total pressure of the wake deviates downward in the baseline case, but it is symmetrical in HP06 case. However, in HP10 case where a 200 mm plate was used, the downwash was excessively suppressed and the bottom flow was excessively up washed, thereby increasing the asymmetry of the rear wake. The bottom flow can be considered to occupy an excessively large portion of the wake region and an adverse effect is shown on the aerodynamic drag reduction.

Cogotti used Equation 1, which predicts the micro drag with wake flow field data [20].

[mathematical expression not reproducible] Eq. (1)

Here u, v, and w represent each component of the velocity, and [u.sub.[infinity]] is the free stream velocity. Micro drag analysis of wake region is capable of ensuring that drag is mainly generated at which location. Through the surface integral of micro drag, the total aerodynamic drag can be calculated. The micro drag at 3 m behind the car are compared in Figure 9, indicating that the weakening of the downwash leads to the relaxation of the longitudinal vortex pair formation. In the baseline case, the core of the vortex pair is evident near the height of the rear bumper. It is formed by the combination of the vehicle side flow and the upper flow downwash. In contrast to the baseline case, when the horizontal plate with a length of 50 mm is installed (HP01), the symmetry of the vortex pair is not apparent and the wake pattern has been changed. When the length of the horizontal plate is increased to 150 mm (HP06), the micro drag at the longitudinal vortex pair is weak enough to make it difficult to locate the core. However, it can be seen that an additional drag occurs due to the increase of the wake area at the position where the horizontal plate is installed. This phenomenon appears to be strong when the horizontal plate length is increased to 200 mm (HP10), and it can be confirmed that an additional vortex is generated due to the excessive suppression of the upper flow downwash. Therefore, when the length is increased to 200 mm, the aerodynamic drag reduction is reduced. There is a appropriate length for the ratio for the down-wash of the upper flow and the up-wash of the lower flow.

The difference in the total pressure between HP06 and the baseline case is shown in Figure 10. The iso-surfaces where the values of [DELTA][C.sub.P,total] are [+ or -]0.6, [+ or -]0.4, and [+ or -]0.2 are represented to clearly identify the region where the energy of the flow is improved by the aerodynamic drag reduction device. The red region rear the device implies the suppression of downwash. The blue region shows that the total pressure at the side and bottom were increased and the flow characteristic were enhanced by suppressing the downwash of the upper flow. The improved flow also affects the wake, which decreases the wake area 4 m behind the car, where the wake is fully developed. The rate of aerodynamic drag reduction is 5.1% due to the combination of inhibition of the longitudinal vortex pair by downwash weakening, restoration of rear pressure by the increase in the total pressure of the lower flow, and decrease of the wake area.

The Effect of Horizontal Plate Shape In the previous paragraph, it was confirmed that the horizontal plate weakened the downwash and inhibited the formation of the longitudinal vortex pair in the wake region. In this section, other complicated shapes of horizontal plate that alleviate drag by interacting with the longitudinal vortex pair are applied. The performance has been analyzed and compared for the 150 mm length where the plane-shaped plate, HP06, showed 5.1% drag reduction and for the shortest length of 50 mm. When the lengths of the plates were 50 mm and 150 mm, the changes in aerodynamic drag compared to the baseline case were -2.0%, 0.1%, -0.6% and -2.9%, 0.9%, -0.5%, respectively; for the triangle, tooth, and saw tooth shapes. Contrary to expectation, the complex shapes showed rather negative effects compared with the plane-shaped plate, which showed drag reductions of 2.2% and 5.1%, respectively, at the same lengths.

Since there is no significant trend with respect to length when using complex-shaped plates, the vorticity and vortical velocity at 3 m behind the vehicle with the 150 mm horizontal plate are compared in Figure 11. In the baseline case, a vortex pair is clearly observed. For HP06, with the 150 mm plane-shaped horizontal plate, on the other hand, the position of the vortex core can hardly be specified, and the vortex strength weakens. However, in the case of the tooth-shaped horizontal plate (HP08), the aerodynamic drag reduction effect is poor, and the vortex pair is hardly dissipated. Additionally, the vortex area is wider at the periphery and the lower part of the trunk. That is, a complex shape forms a new eddy rather than suppressing the vortex pair formation, leaving an unscattered vortex in the wake. The vortex caused by the aerodynamic drag reduction device was observed in all shapes except the plane shape. To understand the difference, HP06 and HP08, which have the largest difference in effect, are compared below.

The complicated shape of the aerodynamic drag reduction device is a cause of additional aerodynamic drag compared to the plane-shaped plate. The locations where the micro drag value is over 0.4 behind the aerodynamic drag reduction device are shown in Figure 10. The micro drag region of HP06 is the area between the two blue lines and that of HP08 is the area between the two red lines. Compared to the baseline case, the region of HP06 case is reduced but that of HP08 case is increased. Similarly, an additional micro drag region has been identified when using sawtooth (HP09) and triangle (HP07) shape devices. New eddies created by the complex shape of the device seem to increase the drag. The vortices formed interact with the downwash of the upper flow, side and bottom flow of the vehicle and their influence continues into the wake. As a result, the more complicated the shape, the less aerodynamic drag reduction is obtained. Additionally, the region where micro drag is over 0.4 is widespread at the bottom for the baseline and HP08 case. However, as downwash is suppressed by the application of the planar horizontal plate, HP06, the lower flow is induced to rise, and the area in which micro drag is over 0.4 is reduced.

Vertical Plate

A vertical plate is installed at the c-pillar and trunk lid to dissipate the c-pillar vortex. It controls the flow from the side to the center of the vehicle along the c-pillar. The combination of the vortex from the c-pillar and the downwash of the upper flow forms a longitudinal vortex pair, which is an important characteristic of the vehicle wake flow. Therefore, if the c-pillar vortex is initially weakened, a notable change in the wake flow can be obtained.

Vertical Plate at Trunk Lid A square shape and a wedge shape, each with a height of 50 mm, were installed on the trunk lid to confirm the aerodynamic drag reduction effect. VP03 (with a square shape) increased aerodynamic drag by 2.0% and VP04 (with a wedge shape) reduced aerodynamic drag by 3.3%. The aerodynamic drag reduction devices applied in both cases are the same in height and position but different in shape. However, the effect on the aerodynamic drag in the two cases is opposite, confirming the importance of the configuration on performance.

The surface pressure distribution on the vehicle and the total pressure distribution of the flow field around the trunk with the aerodynamic drag reduction device are compared in Figure 12. In the baseline case, the side flow is centered along the body of the vehicle and merges with the c-pillar vortex. This creates a strong vortex that lowers the surface pressure along the trunk lid. When the vertical plate is installed, it prevents the side flow from entering the center, and changes the flow direction of the c-pillar vortex. In the case of VP03, the aerodynamic drag reduction device blocks the side flow and weakens the c-pillar vortex. However, at the starting point of the device, the vortex generated by the configuration combines with the c-pillar vortex, which increases the vortex intensity. A high-pressure region is formed at the front of the aerodynamic drag reduction device and the aerodynamic drag is increased.

For VP04, like VP03, the overall flow structure weakens the c-pillar vortex and blocks the side flow. However, because of the low height at the front of the device, there is no tip vortex due to the configuration itself and no high-pressure area is observed at the beginning. The c-pillar vortex and the streamline of the side flow are shown in Figure 12(d) to compare the flow around the aerodynamic drag reduction devices. In the baseline case, side flow proceeds along the c-pillar to the rear of the trunk, merges with the c-pillar vortex, and proceeds backward with a high vortex intensity. In the VP04 case, however, the side flow and the c-pillar vortex are separated by the aerodynamic drag reduction device and are changed into weak vortices.

To examine how the flow is changed by the aerodynamic drag reduction device, the difference in the total pressure distribution between the baseline and VP04 flow fields is shown in Figure 13. The iso-surfaces where the values of [DELTA][C.sub.P,total] are [+ or -]0.20, [+ or -]0.12, and [+ or -]0.06 are represented to clearly identify the region where the energy of the flow is improved by the aerodynamic drag reduction device. If [DELTA][C.sub.P,total] is a positive value, it indicates an area where the loss of total pressure is reduced. Likewise, if it is a negative value, the loss of total pressure is increased. When the wedge-shaped aerodynamic drag reduction device is applied, the flow structure around the device changes, which leads to improvement in the side flow of the vehicle. It can be concluded that the side flow is improved because the vortex strength of the c-pillar vortex is initially weakened, so the longitudinal vortex pair of the wake is reduced as well. Comparing the total pressure at 4 m behind the vehicle where the wake is fully developed, the energy loss of the side flow is clearly improved. In the case of the lower flow, there is both an improved region and a worse region, but at 4 m, the two effects cancel out. This is because of the change in the flow structure in which the vertical plate moves the upwash position to the right, but it does not mean that the total pressure loss is reduced.

Vertical Plate at c-Pillar and Trunk Lid In blocking the formation of the c-pillar vortex, the VP01 and VP02 cases with vertical plates mounted on the c-pillars have no effect on aerodynamic drag regardless of shape. The VP01 case with a square-shaped vertical plate increased aerodynamic drag by 2.7%. This is because a vortex is generated in the aerodynamic drag reduction device itself, and the method does not block the side flow to the center. The VP02 case with a wedge-shaped vertical plate has a 0.2% reduction in aerodynamic drag, which is not effective. To maximize the effect of the VP02 case, a vertical plate extending from the c-pillar to the trunk lid was applied to the VP05 case in combination with a square-shaped vertical plate on the trunk lid, as in the VP03 case. The c-pillar vortex and the side flow streamline are compared in Figure 14 to examine the flow around the aerodynamic drag reduction device. In the baseline case, side flow goes along the c-pillar to the rear of the trunk, merges with the c-pillar vortex, and proceeds backward with a high vortex intensity. The side flow is blocked by the vertical plate at the c-pillar and divided into two. Additionally, the intensity of each is weakened compared to the baseline, and the position is shifted toward the center.

To observe how the aerodynamic drag reduction device changes the flow structure and affects the wake, the difference in total pressure between VP05 and the baseline is shown in Figure 15. The application of the vertical fence to the c-pillar changes the flow pattern around the vehicle and improves the side and upper flow. The side and upper flows are improved because the strength of the longitudinal vortex pair is weakened by initially suppressing the side flow and c-pillar vortex. In the case of the lower flow, the total pressure loss is also changed. Comparison of the loss of total pressure at 4 m behind the vehicle, where the wake is fully developed shows that the energy loss of the flow is improved over the entire rear region of the vehicle by the improvement of the upper flow.

The VP04 case (with a vertical fence on the trunk lid only) and the VP05 case (with the device from c-pillar to trunk lid) show 3.3% and 3.6% aerodynamic drag reductions, respectively. The aerodynamic drag reductions are similar, but the VP05 case shows slightly better performance. The two aerodynamic drag reduction devices have the same mechanism of separating the vortices of the c-pillar and the side flow to weaken them, but there is a difference in the degree to which the side inflow is blocked. The VP05 case blocks the side flow into the c-pillar and weakens the vortex strength. It also leads to improved upper flow as well as side flow by changing the flow structure. Therefore, it would be possible to reduce the aerodynamic drag by designing an aerodynamic drag reduction device for an actual vehicle to not only weaken the c-pillar vortex but also to block the side inflow.

Summary of Results

The primary purpose of applying horizontal and vertical planes was to reduce the aerodynamic drag by making a meaningful change in the flow around the automobile. The characteristic flow around the vehicle includes flow separation due to the bluff-shaped body and a long-lasting wake region. In particular, the vortex generated at the c-pillar not only contributes to energy loss itself, but it also merges with the down wash of the upper flow and side flow at the rear of the vehicle to form a pronounced longitudinal vortex pair in the wake. Therefore, two items have been considered to reduce aerodynamic drag: a horizontal plate to inhibit the formation of longitudinal vortex pairs by weakening the downwash, and a vertical plate to prevent the development of the c-pillar vortex. A total of 15 cases were compared and analyzed. In the case of the horizontal plate and the vertical plate, a substantial change in the flow occurred, and the aerodynamic drag was reduced. The aerodynamic drag reduction methods using the horizontal plate or the vertical plate were designed to suppress the downwash of the upper flow and the development of the c-pillar vortex. The downwash and the c-pillar vortex are commonly observed flow patterns in sedan-type vehicles. Therefore, the fundamental mechanism of the devices can be applied to many commercial sedan vehicles as well as the DrivAer notchback

Conclusions

In this article, the performance of various aerodynamic drag reduction devices was compared and evaluated using the DrivAer notchback model with a detailed underbody. The changes in the wake caused by each aerodynamic drag reduction device were analyzed and the mechanism that generated the reduction effect was confirmed. The aerodynamic drag reduction mechanism that has been computationally illustrated and the wake and pressure effects of the devices and contributed to a greater understanding of the fluid mechanisms behind these devices. Since the study was carried out with the DrivAer model based on an actual vehicle shape, the result of the analysis can be utilized in real device development.

Both unsteady and steady CFD analysis were performed with a coarse grid and a fine one to determine the appropriate condition for analysis. Through the analysis of the averaged flow field, it was confirmed that the wake pattern results of the unsteady and steady analysis are in good agreement with each other when using the fine grid. The aerodynamic drag coefficients and surface pressure distributions of both analyses also match the experimental results. This implies that the steady analysis is an adequate approach for predicting the aerodynamic drag of a vehicle. Including the baseline model, 15 cases were analyzed in total, using horizontal plates, and vertical plates in the rear of the car to reduce aerodynamic drag.

1. The suppression of the upper flow downwash by the horizontal plate was confirmed. The drag reduction effect of the vertical plate-by preventing vortex formation, blocking development and inducing dissipation-was confirmed as well.

2. The horizontal plate installed at the trunk end suppressed the downwash of the upper flow, and it was confirmed that the formation of the longitudinal vortex pair was mitigated and the aerodynamic drag was reduced. The drag reduction effect of the plane-shaped horizontal plate was excellent compared to that of other complex shapes, and the drag reduction effect improved as the length increased up to 150 mm. The aerodynamic drag was reduced by 5.1% when the 150 mm plate was applied, and the improvement of the bottom and side flow by suppressing the downwash of the upper flow was confirmed. Vertical wedge and square plates were installed on the c-pillar and trunk lid, respectively, to reduce aerodynamic drag by 3.6%. The side flow was blocked from going toward the center above the c-pillar, weakening the vortex. Additionally, the improvement of the top flow, as well as the side flow, was effected by the change of the flow structure around the vehicle.

3. The development of the c-pillar vortex and the vortex pair in the wake due to the downwash of the upper flow are the main characteristics of the flow around sedan-type vehicles. The flow characteristics at the rear of the vehicle can be improved through the aerodynamic drag reduction mechanism revealed by the horizontal plate and vertical plate, leading to the overall enhancement of the aerodynamic characteristics of the vehicle.

Recommendations and Future Work

This study analyzed the performance of aerodynamic drag reduction devices using steady numerical simulation. Numerical analysis of the performance of aerodynamic drag reduction devices needs to be verified by unsteady simulation and wind tunnel experiment. In order to derive a more general conclusion because the analysis was conducted only for the DrivAer notchback model, it is necessary to check whether the performance of the aerodynamic drag reduction device is the same in the fastback model. In order to apply the devices analyzed in this study, it is necessary to optimize the aerodynamic drag reduction performance for the position and shape parameters of the horizontal plate and the vertical plate.

Contact Information

Jun-Ho Cho (Ph.D. Candidate)

Seoul National University

jochun86@snu.ac.kr

Kwanjung Yee (Professor)

Institute of Advanced Aerospace Technology

Seoul National University

kjyee@snu.ac.kr

Acknowledgements

This research was supported by the project of Development of Active Aerodynamic Technology Concept funded by Hyundai Motor Company contracted through the Institute of Advanced Aerospace Technology at Seoul National University. This work was supported by the National Research Foundation of Korea (NRF) Grant funded by the Ministry of Science and ICT (NRF-2017R1A5A1015311).

References

[1.] Schutz, T., Aerodynamics of Road Vehicles Fifth Edition (Warrendale: SAE International, 2015). ISBN:978-0-7680-7977-7.

[2.] Mock, P., Kuhlwein, J., Tietge, U., Franco, V. et al., "The WLTP: How a New Test Procedure for Cars Will Affect Fuel Consumption Values in the EU," ICCT White Paper, 2014.

[3.] Bearman, P.W., "Bluff Body Flows Applicable to Vehicle Aerodynamics," Aerodynamics of Transportation, ASMECSME-Conference, Niagara Falls, June 18-20, 1979.

[4.] Katz, J., Race Car Aerodynamics (Cambridge: Bentley, 1996).

[5.] Schultz, S., "Aerodynamics of Modern Sport Utility Vehicles," 8th MIRA International Vehicle Aerodynamics Conference, 2010.

[6.] Heft, A.I., Indinger, T., and Adams, N.A., "Introduction of a New Realistic Generic Car Model for Aerodynamic Investigations," SAE Technical Paper 2012-01-0168, 2012, doi:10.4271/2012-01-0168.

[7.] Ahmed, S.R., "An Experimental Study of the Wake Structures of Typical Automobile Shapes," Journal of Wind Engineering and Industrial Aerodynamics 9(1):49-62, 1981.

[8.] Heft, A.I., Indinger, T., and Adams, N.A., "Experimental and Numerical Investigation of the DrivAer Model," ASME Fluids Engineering Division Summer Meeting, 2012, Volume 1, 41-51.

[9.] Huang, P.G., Bardina, J., and Coakley, T., "Turbulence Modeling Validation, Testing, and Development," NASA Technical Memorandum, 110446, 1997.

[10.] Fotiadis, G., Skaperdas, V., and Iordanidis, A., "The Influence of Mesh Characteristics on External Airflow CFD Simulations of the DrivAer Model," AMS Seminar Series, NASA Ames Research Center, Sept. 17, 2015.

[11.] Wojciak, J.D., "Quantitative Analysis of Vehicle Aerodynamics during Crosswind Gusts," Doctoral thesis, Munich, 2012.

[12.] Collin, C., Mack, S., Indinger, T., and Mueller, J., "A Numerical and Experimental Evaluation of Open Jet Wind Tunnel Interferences using the DrivAer Reference Model," SAE Int. J. Passeng Cars - Mech. Syst. 9(2):657-679, 2016, doi:10.4271/2016-01-1597

[13.] Mlinaric, P., "Investigations of the Influence of Tyre Deformation and Tyre Contact Patch on CFD Predictions of Aerodynamic Forces on a Passenger Car," Department of Applied Mechanics, Chalmers University of Technology, 2007.

[14.] Levin, J. and Rigdal, R., "Aerodynamic Analysis of Drag Reduction Devices on the Underbody for SAAB 9-3 by Using CFD," 2011.

[15.] Kwak, M., Yun, S., Lee, Y., Kwon, H. et al., "Optimum Nose Shape of a Front-Rear Symmetric Train for the Reduction of the Total Aerodynamic Drag," Journal of Mechanical Science and Technology 27(12):3733-3743, 2013.

[16.] Kee, J.D., Kim, M.S., and Lee, B.C., "The COANDA Flow Control and Newtonian Concept Approach to Achieve Drag Reduction of Passenger Vehicle," SAE Technical Paper 2001-01-1267, 2001, doi:10.4271/2001-01-1267

[17.] Ashton, N. and Revell, A., "Comparison of RANS and DES Methods for the DrivAer Automotive Body," SAE Technical Paper 2015-01-1538, 2015, doi: 10.4271/2015-01-1538.

[18.] Wang, S., Bell, J.R., Burton, D., Herbst, AH. et al., "The Performance of Different Turbulence Models (URANS, SAS and DES) for Predicting High-Speed Train Slipstream," Journal of Wind Engineering and Industrial Aerodynamics 165:46-57, 2017.

[19.] Makowski, FT. and Kim, S.E., "Advances in External-Aero Simulation of Ground Vehicles Using the Steady RANS Equations," SAE Technical Paper 2000-01-0484, 2000, doi: 10.4271/2000-01-0484.

[20.] Cogotti, A., "Flow-Field Surveys Behind Three Squareback Car Models Using a New "Fourteen-Hole" Probe," SAE Technical Paper 870243, 1987, doi: 10.4271/870243.

Junho Cho, Joonmin Park, and Kwanjung Yee, Seoul National University

Hak-Lim Kim, Hyundai Motor Company

History

Received: 04 Feb 2018

Revised: 03 Jun 2018

Accepted: 18 Jun 2018

e-Available: 05 Jul 2018

Keywords

Automotive aerodynamics, Aerodynamic drag, Aerodynamic drag reduction device, Computational Fluid Dynamics (CFD)

Citation

Cho, J., Park, J., Yee, K., and Kim, H.-L., "Comparison of Various Drag Reduction Devices and Their Aerodynamic Effects on the DrivAer Model," SAE Int. J. Passeng. Cars - Mech. Syst. 11(3):225-237, 2018, doi:10.4271/06-11-03-0019.

doi:10.4271/06-11-03-0019
TABLE 1 Calculation schemes.

Description                Steady Unsteady
Gradient scheme            Gauss linear
Divergence scheme          Gauss upwind
Laplacian scheme           Linear corrected
Interpolation scheme       Linear
Pressure solver            GAMG
Velocity solver            smooth Solver
Non-orthogonal correctors  4

TABLE 2 Numerical simulation results and comparison with experiment.

Wind tunnel [C.sub.D]                 0.277
                       Steady         Unsteady
Description            SST k-[omega]  SST k-[omega]  IDDES

Fine grid              0.284 (+2.6%)  0.285 (+2.8%)  -
(40 million cells)
Coarse grid            0.289 (+4.3%)  0.294 (+6.2%)  0.287 (+3.6%)
(25 million cells)

TABLE 3 Various aerodynamic drag reduction devices and parameters.

Item              Case  Type            Parameter  Position

Baseline          DN00
                  HP01  Plane             50 mm
                  HP02  Triangle          50 mm
                  HP03  Tooth             50 mm
                  HP04  Saw tooth         50 mm
Horizontal Plate  HP05  Plane            100 mm    Trunk End
                  HP06  Plane            150 mm
                  HP07  Triangle         150 mm
                  HP08  Tooth            150 mm
                  HP09  Saw tooth        150 mm
                  HP10  Plane            200 mm
                  VP01  Square            30 mm
                  VP02  Wedge             50 mm    c-pillar
Vertical Plate    VP03  Square            50 mm
                  VP04  Wedge             50 mm    Trunk Lid
                  VP05  Wedge & Square    50 mm    c-pillar & Trunk

Item              [C.sub.D]

Baseline          0.284      -
                  0.278      -2.2%
                  0.278      -2.0%
                  0.284       0.1%
                  0.283      -0.6%
Horizontal Plate  0.274      -3.7%
                  0.270      -5.1%
                  0.276      -2.9%
                  0.287       0.9%
                  0.283      -0.5%
                  0.281      -1.0%
                  0.292       2.7%
                  0.284      -0.2%
Vertical Plate    0.290       2.0%
                  0.275      -3.3%
                  0.274      -3.6%
COPYRIGHT 2018 SAE International
No portion of this article can be reproduced without the express written permission from the copyright holder.
Copyright 2018 Gale, Cengage Learning. All rights reserved.

Article Details
Printer friendly Cite/link Email Feedback
Author:Cho, Junho; Park, Joonmin; Yee, Kwanjung; Kim, Hak-Lim
Publication:SAE International Journal of Passenger Cars - Mechanical Systems
Article Type:Technical report
Date:Jul 1, 2018
Words:9177
Previous Article:Parametric Study of Asymmetric Side Tapering in Constant Cross Wind Conditions.
Next Article:Vehicle Stability Control through Optimized Coordination of Active Rear Steering and Differential Driving/Braking.
Topics:

Terms of use | Privacy policy | Copyright © 2020 Farlex, Inc. | Feedback | For webmasters