Nomenclature

A_CS=surface area of the cooling system

A_VS=frontal area of the vehicle

C_D=drag coefficient

C_p=pressure coefficient

F_CS=net force acting on the cooling system

F_VS=net force acting on the vehicle surface

k_L=dimensionless loss factor

q=dynamic pressure

r_n=polynomial coefficient

v=normal velocity component

y⁺=viscous sublayer length scale

Δp=pressure drop

Δp_CS=pressure drop of the cooling system

ρ=density of the fluid

In automotive industry,the drag coefficient is a significant design parameter. A large amount of power is spent to overcome the aerodynamic drag for a road car cruising in highway with a speed of about 120 km/h,hence the fuel consumption is an important issue. Consequently,even a little improvement in C_D value may result in significant fuel economy,in a cumulative manner. Numerical prediction tools are now a viable supplement to the very costly experimental measurements [1]. However,the modeling should be handled with care to include all sources of drag both internal and external to the vehicle. The total drag of the vehicle can be increased by about 5%-10% due to its cooling system [2]. The aim is to catch low drag values by maintaining high cooling air flow. In the present study,the effect of the engine cooling on the total drag is evaluated using CFD methods for a light commercial road vehicle. Four different vehicle configurations,described in section 1,were considered for analyses. The detailed numerical mesh includes both exterior and interior (engine compartment,under hood components) parts of the vehicle. The effects of radiator and fan on the total drag were calculated,separately. The initial and boundary conditions were determined by in house experiments (radiators pressure drop) and manufacturer data (mass-flow rate information of radiator fan) that are used as inputs for the RANS based CFD analyses. The effect of the wheels motion and cruise speed on the cooling drag and total drag is also investigated. Predicted cooling drag corresponds to 6.9% of the total drag which is consistent with the test results and measurements by the manufacturer. Furthermore,increasing the cruising speed of the vehicle from 120 km/h to 140 km/h had a negligible effect on the value of cooling drag coefficient. Likewise,the cooling drag coefficient is not influenced by the road and wheel motion. However,modeling the road and wheel motion result in lower calculated total drag coefficient,consistent with the real vehicle situation.

As shown in Table 1,a total of four separate analyzes were executed to determine the difference resulting from the cooling drag (Case#1 vs. Case#2),the effect of cruising speed on cooling drag (Case#2 vs. Case#3) and the effect of moving road and wheel simulation on the total drag coefficient (Case#3 vs. Case#4).

The CFD analyses are carried out using a commercially available solver [3]. The flow is modeled by assuming three-dimensional,steady,incompressible,viscous flow. The second-order upwind scheme is used for the spatial discretization. The Realizable k-ε turbulence model is employed to model the turbulent nature of the flow. The enhanced wall treatment is applied for the near-wall region to resolve the boundary layer and turbulence quantities more accurately.

The computational domain boundaries are 5 vehicle lengths to the upstream and 10 vehicle lengths to the downstream direction. As shown in Figs. 1 and 2,the surface elements on the vehicle are colored according to their sizes. The grid is created in millimeters.

Fig. 1 Surface element lengths on the vehicle (mm).

图选项

Fig. 2 Surface element lengths at underbody components (mm).

图选项

Smaller element sizes were used on the surface of the vehicle at possible flow separation areas,stagnation regions and areas where a proper representation of geometry is needed. The mesh refinement is not performed only at the boundary layer development regions,but also in the wake regions. This grid structure is especially focused on the critical zones where sudden and significant changes occur in the flow properties. This ensures reliable results with lower computational time since the mesh refinement is only carried out at necessary locations. The local resolution of the surface and volume mesh elements can be increased by using the “size-box” property of ANSA grid generation software.ANSA size-boxes help to refine certain areas of surface and volume meshes without creating geometrical constructions for closed inner volumes [4].

The domain consists of approximately 51.7 million volume elements where almost one third of it comes from boundary layer region. Viscous sublayer length scale at the wall-adjacent cell should be on the order of y⁺=1 when the enhanced wall treatment is employed with the intention of resolving the laminar sublayer [3]. The generated boundary layer and volume mesh specifications are given in Table 2 and shown in Fig. 3.

Fig. 3 Boundary layer and volume mesh details.

图选项

In CFD analyses,the radiator is generally treated as a porous medium or a heat exchanger that generates pressure drop. The pressure drop and heat transfer coefficient can be defined as a function of the perpendicular velocity component of the flow that passes through the radiator. It is assumed that the radiator element has a thickness which is infinitely thin and the pressure loss across the radiator is proportional to the dynamic pressure of the fluid. Experimentally determined dimensionless loss factors (k_L) can be specified as constants or defined by polynomials and used as inputs for CFD analyses. The relation between dimensionless loss factor and pressure drop can be written as,

点击浏览公式

In Equations (1) and (2),ρ is the density of the fluid (air),r_n is the coefficients of the polynomial and v is the perpendicular velocity component of the flow passing through the radiator. In the present study,the heat exchanger model was assumed to have a pressure drop caused by radiator. The temperature change in cooling fluid was not taken into account. In experiments,the tunnel speeds ranging from 1.5 to 7.5 m/s were used deriving by the manufacturer data (e.g. mass-flow rate information of radiator fan). These speeds are also consistent with the reference studies found in literature [5, 6]. The curve fitting is made to the measurements and given in Fig. 4.

Fig. 4 Fitted curves to loss measurements for the cooling system elements.

图选项

Numerical analyses is carried out to determine the cooling drag by implementing radiator definitions at relevant regions,Fig. 5. Radiator definitions depend on polynomial expressions which were extracted from experiments.

Fig. 5 Surfaces defined as radiators.

图选项

The velocity distributions on the cooling components which are defined as radiator are presented in Figs. 6-8. The flow structures on the sections can be understood by examining the velocity component distributions. The CFD analyses show that the flow through the grills cannot form a homogeneous velocity distribution on the cooling sections. Moreover,remarkable change in velocity is observed especially in the directions which are tangent and perpendicular to the freestream direction.

Fig. 6 Flow patterns and velocity field of the cooling components.

图选项

Fig. 7 Local velocity distributions of the cooling components (Case#2).

图选项

Fig. 8 Local velocity distributions of the cooling components (Case#3).

图选项

In order to determine the cooling drag,additional cross-sections were constructed at the front and rear sides of the cooling components. As shown in Fig. 9,the locations of these sections are at a distance of about 1 cm to the relevant surfaces.

Fig. 9 Cooling components (black) and the auxiliary surfaces (grey).

图选项

The static pressure distributions at these surfaces are given in Figs. 10-13. The area-weighted average of the static pressure values on the auxiliary sections were calculated to obtain the pressure drops.

Fig. 10 Static pressure distributions at auxiliary surfaces of CAC (Pa).

图选项

Fig. 11 Static pressure distributions at auxiliary surfaces of condenser (Pa).

图选项

Fig. 12 Static pressure distributions at auxiliary surfaces of radiator (Pa).

图选项

Fig. 13 Static pressure distributions at auxiliary surfaces of fan (Pa).

图选项

The predicted pressure drop values are in a good agreement with experiments. The drag force due to the cooling system is calculated by multiplying the predicted pressure drops with the corresponding surface area. The total drag force is then obtained by summing the drag forces acting on the vehicle surface and the cooling components. The calculation is done by the following formulation:

点击浏览公式

In above equations,F_VS is the net force acting on the vehicle surface and A_VS is the frontal area of the vehicle. F_CS is the net force acting on the cooling components obtained by the pressure drop values. Here,i is the index used for presenting each component of the cooling system. Therefore,A_CS,i is the surface area of the relevant cooling component,q is the dynamic pressure and equals to 1/2ρU² for incompressible flows; ρ is the mass density of the fluid (air) and U is the freestream velocity.

Case#1 and Case#2 were used to determine the drag caused by the cooling system. Results show that,the drag coefficient is increased by the implementation of cooling systems in the numerical model.

The effect of cruise speed on the prediction of drag coefficient was investigated via comparison of Case#2 and Case#3. The drag coefficient,C_D,can often be treated as a constant for high Reynolds number flow regimes such as cars at highway speed or aircrafts at cruising speed. As shown in Fig. 10 to Fig. 13,the predicted pressure distributions on the cooling components were qualitatively similar (almost identical) for the two cases but a quantitative examinaation shows that there exist differences in terms of pressure drops. In fact,it is observed that the drag force acting on the vehicle and cooling components become larger with the increased cruising speed,but the drag coefficient remained unchanged since the force is being made dimensionless with the square of the speed.

The effect of moving road and rotating wheels is also examined via comparison of Case#3 and Case#4. The resulting velocity contours for the flow field is presented in Fig. 14.

Fig. 14 Effect of wheel motions on the velocity field predictions.

图选项

The flow velocity behind the wheels that are modeled as rotating walls is faster compared to the non-rotating ones. The rotating wheel model has also smaller wake compared to stationary one which yielded a lower C_D prediction. The predicted total drag coefficients of the aforementioned cases were tabulated with detailed descriptions in Table 3.

The convergence histories of the different cases based on drag coefficient are given in Figs. 15-17. The pressure coefficient distributions and the flow characteristics around the vehicle are shown in Fig. 18 and Fig. 19,respectively.

Fig. 15 Effect of cooling drag on total CD.

图选项

Fig. 16 Effect of cruising speed on total CD.

图选项

Fig. 17 Effect of moving road and wheel simulation on total CD.

图选项

Fig. 18 Cp distributions on the vehicle (Case#2).

图选项

Fig. 19 Flow characteristics for the cooling drag analyses (Case#2).

图选项

The geometric specifications of the vehicle and the drag coefficient values are not explicitly given due to commercial confidentiality.

All calculations are carried out on a 12 core parallel machine with 2×2.30 GHz Intel Xeon E5-2630 pro-cessors. The platform uses a 64-bit Win-7 operating system and a total of 64 GB of RAM. The mesh partitioning is done using the “Metis” method of the FLUENT software. The wall clock computation time was approximately 114.5 h for a solution of 6000 iterations. It is observed that the radiator/fan modeling and the moving wall approach do not have a noticeable effect on the computation time.

CFD analyses have been performed to obtain total drag coefficient including cooling drag part for the light commercial vehicle. The pressure drop characteristics of the cooling system components are determined by wind tunnel tests utilizing the facilities of ITU Trisonic Laboratory and manufacturer's data provided by FORD. ITU wind tunnel tests have been carried out by additional studies to validate the manufacturer’s data and examine the various working-conditions (free and force-fed) of fan.

CFD analysis results are consistent with the clay model test results. A satisfactory result gathered from CFD analysis (Case#2) with a 0.1% approxi-mation to the clay model test results.

The CFD analysis for the closed grill condition represented by Case#1 have been made to isolate the effect of cooling drag on the total drag. Predicted cooling drag corresponds to 6.9% of the total drag which is consistent with the test results and measurements by the manufacturer . Furthermore,additional analysis for different cruising speeds such as 120 km/h and 140 km/h demonstrated that the cruise speed,particularly for these flow regimes,do not have a remarkable effect on the prediction of cooling drag coefficient. Likewise,the prediction of cooling drag coefficient does not change whether the CFD model includes the road and wheel motion. However,modeling the road and wheel motion reduces the total drag coefficient.

The cooling drag characteristics of different vehicles can be determined by using the modeling methodology developed in the present work. The cooling flow may be obtained with lower pressure loss by the optimization studies to be performed on the vehicle.