1 Computational Setup

In this section, the computational setup is described which was used for simulations.

1.1 Model Geometry and Virtual Wind Tunnel

A simplified semi-trailer truck model was used for simulations and is shown in Fig. 5.1 with its outer dimensions in mm.

Fig. 5.1
figure 1

Used truck model with the outer dimensions in mm

Full size image

Major simplifications were made for the wheel rims. Also, detailed components (e.g. the antenna, cabin suspension, foot board) were not considered because the influence of this components on the investigated aerodynamic parameters is negligible.

A virtual wind tunnel was created for the CFD investigations and is shown in Fig. 5.2. The box around the trucks consists of the boundaries inlet, outlet, floor and symmetric walls. The different boundary conditions for these boundaries will be explained below in Sect. 5.1.2. The outer dimensions were chosen in such a way that the influence of the truck geometry on the boundary condition is insignificantly small. The trucks are arranged in the middle of the wind tunnel and the front edge of the first truck is 50 m away from the inlet boundary. In Fig. 5.2, the flow direction and the outer dimensions of the wind tunnel are shown.

Fig. 5.2
figure 2

Virtual wind tunnel with its outer dimensions and the used boundaries

Full size image

1.2 Boundary Conditions

The boundary conditions for the simulations, as illustrated in Fig. 5.2, are:

  • Inlet: At the inlet boundary condition, a constant velocity \(u_\infty \) is specified, based on the considered truck speed.

  • Outlet: In order to guarantee a defined pressure level, the pressure at the outlet boundary is kept constant.

  • Symmetric walls: In order to guarantee a gradient-free velocity field at the boundary surfaces, a symmetrical boundary condition is prescribed at these surfaces.

  • Wheels: The wheels are modelled with rotating wall boundary conditions.

  • Floor: The floor boundary condition is modelled with a moving wall boundary condition with a constant velocity \(u_\infty \).

  • Truck surfaces: All truck surfaces except the wheels are assigned a no-slip boundary condition.

1.3 Heat Exchanger Model

The engine compartment flow is considered in the simulation. In the engine compartment, three heat exchangers are modelled, namely the water cooler, condenser and charge air cooler. In Fig. 5.3, the position of the heat exchangers is shown, condenser (green), charge air cooler (blue), water cooler (red). All three heat exchangers are modelled as porous media using the Darcy–Forchheimer law [6]. The Darcy–Forchheimer law describes the relationship between pressure loss and flow velocity based on the Darcy coefficient D and Forchheimer coefficient F.

Fig. 5.3
figure 3

Position of the heat exchangers in the engine compartment and their dimensions, specified in mm

Full size image

The coefficients can be experimentally identified by measuring the pressure loss of the individual heat exchangers at different volume flows. Using the method of least squares, the coefficients D and F can be determined from measurements. Table 5.1 shows the values used in the simulation based on experimental data:

Table 5.1 Experimentally identified coefficients of the Darcy–Forchheimer model
Full size table

1.4 Mesh Generation for Simulation

The mesh generation for simulation was done in OpenFOAM with the mesher “snappyHexMesh”. The mesher “snappyHexMesh” creates, based on the assigned model, a hexahedral dominated mesh. The base cell size was defined as 2 m, with the refinement boxes placed in close proximity to the truck. Figure 5.4 illustrates the arrangement of these refinement boxes. The different refinement levels define the mesh resolution in the refinement boxes based on the base level with the relation

$$\begin{aligned} \mathrm {cell~size} =\frac{\mathrm {base~size}}{2^{\mathrm {refinement~level}}} \,. \end{aligned}$$
(5.1)
Fig. 5.4
figure 4

Arrangement of the refinement boxes for meshing

Full size image

The truck geometry had a maximal refinement level of 8 on the walls. Inside the engine compartment, the refinement of critical geometry areas went up to level 11. The resulting mesh is shown in Fig. 5.5 as a longitudinal section (cut through \(y=0\) m), for a single truck case. It can be seen that with higher levels, the cell sizes are reduced. For the solo truck case, the mesh consisted of around 22 million cells, and for the platooning cases with 3 trucks, the simulation mesh consisted of around 66 million cells.

Fig. 5.5
figure 5

Simulation mesh for the longitudinal section

Full size image

1.5 Flow Field Computation

The CFD simulations were performed with the GNU GPL licensed software package OpenFOAM. For the investigated aerodynamic problem, the assumption of a incompressible, steady-state flow with constant material properties were made and using an Reynolds-averaged Navier–Stokes equations (or RANS equations) approach [5]. The underlying RANS conservation equations were solved with the OpenFoam “SimpleFoam” solver. SimpleFoam solver is a steady-state solver for incompressible, turbulent flow, using the Semi-Implicit Method for Pressure Linked Equations (SEMI) algorithm [4]. As turbulence model, the k-\(\omega \)-SST model was chosen, which has already proven its accuracy and efficiency in automotive aerodynamics [3]. The k-\(\omega \)-SST model is a two-equation eddy-viscosity model for the turbulence kinetic energy, k, and turbulence specific dissipation rate, \(\omega \). The used material property values for the density \(\rho _{\textrm{air}}\), the kinematic viscosity \(\nu _{\textrm{air}}\) and the reference pressure \(p_{\textrm{ref}}\) and temperature \(T_{\textrm{ref}}\) are shown in Table 5.2.

Table 5.2 Material parameters for the simulation model
Full size table

2 Simulation Results and Discussion

The simulations were done for a platoon with three trucks for different constant velocities at different inter-vehicle distances between each truck. The inter-vehicle distances within the platoon were kept constant for each simulation. The investigated velocities were 60, 80 and 90 km/h. For all velocities, the distances 6.66, 11.11, 22.22, 33.33, 56.56 m were simulated, and for the 80 km/h, the additional spacing of 15 m was simulated.

2.1 Drag Coefficients

The main key parameter to quantify the drag or the resistance of an object is the drag coefficient \(c_\textrm{d}\). For all simulations, the drag coefficient was evaluated and compared. The drag coefficient is defined as

$$\begin{aligned} c_\textrm{d} = \frac{2F_\textrm{d}}{\rho u^2\,{{A}}} \end{aligned}$$
(5.2)

where

  • \(F_\textrm{d}\) is the drag force, which is by definition the force component in the direction of the flow velocity,

  • \(\rho \) is the mass density of the fluid,

  • u is the flow speed of the object relative to the fluid,

  • A is the reference area [7].

For automobiles and many other objects, the reference area is the projected frontal area of the vehicle [1]. The drag coefficients for the different investigated velocities were nearby the same. The relative deviation for the drag coefficients for the velocities 60 and \({90}\,{\textrm{km}/\textrm{h}}\) compared to drag coefficients for the velocity \({80}\,{\textrm{km}/\textrm{h}}\) was less than \(2\%\). Thus, the drag coefficient can be assumed to be independent of the driving speed for the investigated velocities, and just, the results for the velocity \({80}\,{\textrm{km}/\textrm{h}}\) are shown.

Fig. 5.6
figure 6

Normalised drag coefficients for the velocity 80 km/h

Full size image

In Fig. 5.6, the normalised drag coefficients are shown for the velocity 80 km/h. The drag coefficient was normalised by the drag coefficient for the solo truck simulation. The greatest savings potentials are at the smallest inter-vehicle distance. Even truck 1, which only shows a change in the trailing area behind the truck, shows a reduction of about \(25\%\) of the resistance value of the solo truck case. For the smallest distances 6.66 and 11.11 m, truck 2 has a smaller drag coefficient than truck 3. It can be seen that for larger distances (15, 22.22, 33.33 and 56.56 m) truck 3 has the smallest drag coefficient followed by truck 2 and truck 1 through the slipstream effect. Truck 1 and truck 2 except for the 15 m case have a rising trend of the normalised drag coefficients. For truck 3, there is a decreasing trend for smaller distances, and from 22.22 m, there is an increasing trend. A decreasing of the averaged drag coefficient of the platoon could be observed for all simulations for a decreasing inter-vehicle distance except for 15 m. On average, up to \(30\%\) reduction of the drag coefficient is possible by using a platoon.

In terms of flow analysis, two major factors are responsible for the drag reduction on the vehicles in the platoon. These are lower incoming flow velocity which reduces the pressure on the front and higher pressure on the back.

Fig. 5.7
figure 7

Kinematic pressure distributions for the longitudinal section for all cases

Full size image

Figure 5.7 shows the kinematic pressure distribution of all cases for the longitudinal section. The kinematic pressure here is defined as followed using the static pressure \(p_{\textrm{stat}}\), the reference pressure \(p_{\textrm{ref}}\) and the density \(\rho _{\textrm{air}}\):

$$\begin{aligned} p_{\textrm{kin}} = \frac{p_{\textrm{stat}} - p_{\textrm{ref}}}{\rho _{\textrm{air}}}. \end{aligned}$$
(5.3)

The effect of a higher pressure on the back is clearly seen for smaller distances. The higher pressure on the back is the reason why for the smallest distances truck 2 has a smaller drag coefficient than truck 3 and why there is a significant drag reduction for the leading truck 1. The effect of a higher pressure on the back is also observed at large distances (33.33 and 56.56 m) for truck 1 resulting in slightly reduced drag coefficients compared to the solo case. Figure 5.8 shows the velocity distribution for the longitudinal section for all cases. The lower incoming flow velocity for the following trucks 2 and 3 can be seen, which results in reduced pressure in the front. This can also be seen in Fig. 6.11 of Chap. 6, where the pressure drag coefficients \(c_\textrm{p}\) are shown for front and back for truck 2 for selected cases.

Fig. 5.8
figure 8

Velocity distributions for the longitudinal section for all cases

Full size image
Fig. 5.9
figure 9

Cumulative normalised pressure drag coefficient for the inter-vehicle distances 6, 11, 15, 22 m for the second truck

Full size image

In Fig. 5.9, the cumulative normalised pressure drag coefficients for the cases 6, 11, 15 and 22 m for the second truck are shown to get a hint how the drag coefficients occur. The cumulative pressure drag coefficients are plotted using 20 subdivision with a spacing of around 84 cm. It can be seen that for the 15 m case the initial cumulative normalised pressure drag coefficient is higher than for the other shown cases, which leads to an overall higher drag coefficient. Higher maximal stagnation pressures in the middle of the front of truck 2 for case 22 m can be observed compared to case 15 m but for case 15 m higher pressures at the side of the front areas, roof of the cabin and the cab-roof fairing are obtained. For the other cases, the expected increasing trend of the cumulative normalised pressure drag coefficient can be seen. Also, the effect of a higher pressure on the back can be observed resulting in a lower total pressure drag coefficient, especially for case 6 m.

2.2 Fuel Savings

In order to be able to conclude from the reduction of the drag coefficient to a reduction of fuel consumption, the total share of drag losses in the total mechanical energy must be determined. It can be assumed that the relative percentage of engine losses in relation to the total energy from the fuel remains the same. The internal engine losses do not change due to the changed air resistance. Therefore, in order to evaluate the savings potential through the reduction of air resistance, the relative proportion of air resistance to the required mechanical energy must be considered [1]. Thus, the reduction of the drag coefficient with a form factor M, using

Fig. 5.10
figure 10

Fuel reduction in % relative to single truck

Full size image
$$\begin{aligned} {\Delta } c_\textrm{d} = M \cdot {\Delta } T,\end{aligned}$$
(5.4)

can be converted to the fuel saving \({\Delta } T\) (in \(\textrm{litre}/{100}\,\textrm{km}\)) [2]. A typical value of \(M=3.5\) is chosen for these studies, given in [2]. The potential fuel savings are shown in Fig. 5.10 using the simulation results for the reduction of the drag coefficient from Fig. 5.6. On average, a fuel reduction up to \(10\%\) is realised for the smallest investigated spacing.

2.3 Mass Flow Through Heat Exchangers

As seen in the previous results, the platooning effect can lead to significant reduction of the pressure in the front and the air mass flow through the heat exchangers is reduced, which leads to a reduced cooling performance. For all three heat exchangers, the volumetric mass flow was evaluated to be able to identify potential risks concerning thermal management issues. The volumetric mass flows were taken and normalised with the volumetric mass flow of the solo truck case. In Fig. 5.11, the normalised mass flows over the radiator are shown. It can be seen that there is a significant mass flow reduction over the heat exchangers for truck 2 and truck 3, especially for the smaller distances. The mass flow for the charge air cooler and condenser is not shown because they have similar results like the shown radiator case. For the case with an inter-vehicle distance of 6 m, the air mass flow drops under \(50\%\) for truck 2 and truck 3. This low air mass flows imply a risk for the thermal management system. These implications on the thermal management system are targeted in Chap. 15. This is important because the additional needed fan power for small distances increases the fuel consumption and the gains from platooning drag reduction can be diminished.

Fig. 5.11
figure 11

Normalised volumetric mass flow over radiator for a varied inter-vehicle distance

Full size image

3 Conclusion

Computational fluid dynamics (CFD) simulations are conducted for platoons of three vehicles. Several inter-vehicle distances and velocities were investigated. Further, it is apparent that there is a significant potential in fuel savings for smaller distances. It can be seen that there are also critical inter-vehicle distances like 15 m where the drag reduction is not following a decreasing trend to smaller distances for truck 2. Further investigations are needed to be able to better delimit the critical distance range. The results concerning the mass flow over the heat exchangers show a potential risk for the thermal management for the smallest distances. This issue is addressed in Chap. 15. Further simulative investigations with different model geometries and with different arrangements would be beneficial to assess their influence on the total drag reduction.