The aero development begins in the concept design, which its output is used as trigger to both Computation Fluid Dynamics (CFD) and Wind Tunnel (WT) processes. Each of it has about three phases. WT process took advantage of the concept and design data to build the wind tunnel model (WTM). This is based in production, pre-fitting and testing processes. The CFD process is composed by pre-processing, solving and post-processing. An important point about these two paths in the aero development is that CFD governs this process, which means that any model innovation or shape modification will be previously tested in CFD and WT environments. This one has the potential to analyze many configurations of the model shape. For instance, the analysis of the first concept of a wing. In just one WT run, it is possible to test many wing positions. However, WT process requires tooling, thus very skilled technician. On the other hand, CFD can go from the pre-processing to the post-processing very fast. This difference is what makes the CFD process to test many model variations, thus it leads the entire aero development. The macro and major architecture choices are defined at the CFD process. The most interesting one goes to WT to evaluate all wing and ride height configurations.

After that, the data from both paths are merged and used as inputs for the full scale validation and correlation. Depending on the project and its current situation, this process can follow two paths. Either one, it follows a controlled environment, which is the wind tunnel, but with a full scaled model. Usually, the firsts WTM are 40 to 60 % scale models. Or a track environment, where the aero evaluation is performed in a real environment. The main difference between these stages is that the last one uses a real car. Finally, the data measured in the full scale correlation and validation is used to feed the very first step, concept and design, but being a second phase of the aero development which is the performance optimization. Therefore, the CFD process is the most important part, because it is the fastest in delivering results, but it also requires a lot of simulation layouts to support the project. This is dependent on the synergy between CFD, WT and track testing personnel.

CFD tools

The aero development deals with several areas of vehicle design. In terms of race cars, the main one is the aero performance and CFD aero map. These define the drag, downforce, aero balance, design style impact, active aerodynamics and ride height sensitivity. The output of these areas is the unsteady or transient simulations, map points and overtaking analysis. In other words, it creates a package of data that characterizes the vehicle behavior under the flow. The analysis of the cooling and engine systems are important to understand the temperature field, but more importantly, the energy transferred to the flow. In addition to these, the comfort analysis, Multiphysics and 3D flow measurements. The first is more related to the road vehicles, since there is a higher concern with wind noises. Multiphysics deals with particle interactions inside the flow and 3D flow measures the position of these particles along the flow by particle image velocimetry (PIV).

The map points is the main method of analysis, it is capable to deliver a holistic view of the vehicle behavior. This is done by varying the wind tunnel model ride height in order to emulate the main vehicle movements, which are braking, acceleration, high speed corners, low speed corners and straight line moving. This results in a big map of performance, thus contours of the sensitivity and handling of the vehicle during a lap. These are all based in ride heights RH and aerodynamic coefficients. It is interesting to notice that the map points are built not only for CFD, but also for WT analysis. In this one, electromechanical active suspensions are required to change the wind tunnel model RH. However, in CFD software it is required an automatic tool that changes the CFD model RH. This tool is called morphing, which is the freezing of some parts or systems of the car, while other parts of the body are free to move. It is a quite common CFD technique that allows to perform relative movements between parts, systems and entire body automatically. This is done just setting the nodes positions according to the demand or the kind of evaluation. For the map points management, the car body is stand still while the domain and wheels are moving. This emulates the different vehicle maneuvers, just with wheel position variation and consequently the vehicle ride height variation. For example, the design RH is an information that comes with the CAD model. In CFD there is no CAD model, instead, there is a volume mesh. If the suspension volume mesh is morphed, it is possible to variate its position relative to the vehicle body. In this way, it is possible to build a map of points for all vehicle conditions.

Unsteady simulations

The transient or unsteady simulations is a key point to evaluate the external aerodynamic performance due to its high accuracy of the aerodynamic coefficients, specially for the evaluation of drag. An interesting fact on aerodynamic analysis, is the reasonable values obtained for aero balance and downforce and the strange values obtained for drag. The reason is that RANS equations underestimate the drag coefficients. For instance, the results observed on an open wheel race car CFD analysis (Figure 3) is rather smooth, when using RANS equations based simulations.

As a result, it is possible to visualize the flow behavior, it provides reasonable results for stability. Since RANS smooths all results, this kind of simulation is not suitable to visualize drag and its coefficients.

As an alternative for drag and wake analysis, it is adopted as transient or unsteady simulations. Hence, RANS simulations for drag analysis exhibit results about 2-10% more biased from the ones obtained by transient analysis, which are near to the real conditions. Apart from the wake, there are a lot of spots of high and low total pressure in the transient simulations. These are higher than the same simulation done with RANS equations.

Wake analysis

The wake analysis (Figure 5) is the main one used for one-make racing series, because the wake produced disturbs a lot the air flow for the car which is right behind. This reduces the vehicle downforce, thus its capability to follow the car in front [1,2]. Series like Indy Racing League, Formula 2 and Super Formula have the overtaking capability as the main target for the aero development. In these cases, the easier it is to overtake the car in front, the nicer the championship will be. There are several parameters defined as overtaking indexes. The main ones are the delta aero balance and the drag reduction. However, this is not totally true, because the impact of the wake on the vehicle on the tail inevitably creates huge difficulties to overtake the leading car, even though these have low drag.

This occurs, because wake is a natural consequence of the vehicle run and it concentrates at the center part of the vehicle. A typical CFD simulation is done with two CFD models in a specific environment (Figure 6). As can be seen, the wake is concentrated at the center of the car, when this is at a determined distance. As a result, this can be used to develop the front wing in order to produce more downforce by the extremities of the wing, since the middle of the car track is basically immersed in the wake. This helps to reduce the front wing sensitivity to the wake, thus it helps a car to follow the leading one. It is interesting to observe that the front wing efficiency variates according to the distance from the leading car. For instance, at some distance from it, the front wing can work with a good efficiency. However, if it approximates more, this efficiency decreases, because the car is fully immersed in the wake. However, wake is just an example of the effect that a race car suffers when running behind the other one. There are also the out-wash and the in-wash that helps to develop along the underfloor area which also helps to keep the downforce at a good level, thus reducing even more the wake sensitivity. Therefore, the development of the overtaking capabilities in one-make series should account for the other design requirements, specially the effects of the optimized front wing in the rear part of the car. In addition, in Figure 6 it is also possible to evaluate the cornering capability. This is a peculiar analysis, because the car is under a curved flow in a big radius corner. It is possible to evaluate the traffic condition inside a corner in order to understand how the front wing behaves. The design requirement changes in competitive series. In these cases, the design of the wing profile adopts shapes that create the biggest wake possible in order to reduce the aerodynamic efficiency of the car right behind.

In a closed wheels race car, the aerodynamic behaves differently, the main aerodynamic effect is the unsteady phenomena, which leads to a separation at the back of the car and this guides the wake produced. The problem is that the overtake analysis for this case does not have the same impact as in one-make series. The reason is that how these cars behave when very near each other. The effect of leading or following car is not so connected to the wing effect on the air flow. Actually, closed wheels (CW) race cars create a huge pressure that influences not only the car which is following, but also the car which is leading. At this point it is possible to understand how open and closed wheels race cars must be driven during an overtake. For instance, CW race cars usually become very near each other during overtakes. The reason is an overpressure that also changes the performance of the leading car. It is quite interesting, since the CFD simulation of GT car alone and being chased by another one is quite similar. However, when the car on the tail becomes very close, the aero balance, drag and downforce of the leading car changes drastically due to the overpressure.

Cooling and fan modeling

The cooling performance is also evaluated in CFD, this is done by fan modeling. The fan is a typical application of CW race cars, it is used for conditions that the air flow is insufficient to cool down the engine. Hence, fans are introduced to create a forced air flow that balance the heat contained into the coolant fluid. Usually fans have a fixed rotational velocity, but there are applications with different velocity stages. Once the car is at high speed, the fan is de-activated, because the air flow is sufficient, or more than that to cool the engine. This occurs because at higher speed, the air flow has a higher energy, which balances with the amount of heat contained into the coolant. In this situation, the fan enters in the so called passive fan condition. There are two different conditions of the fan operation and these require a proper configuration for the simulation. The forced fan can be done in two ways, by the calibration curve and the model reference frame (MRF) methods that can be applied into the model.

Calibration curve

A particularity of fans is that these are third party components. Hence, some suppliers are too reserved in terms of sharing their CAD model. This makes it difficult to work with CAD, because the geometry of the blades are very important to characterize the fan into the CFD environment. Hence the calibration curves are more adopted at this part of the CFD process, because it is a kind of information that suppliers prefer to share. The calibration curve contains the maximum RPM and the pressure jump. In this case, it is configured the following equation:

ΔP = Σ_n=1^N ƒ_n v^n-1

On an introduced surface it is imposed the pressure jump related to the air flow already defined, thus RPM is fixed and three pressures introduced to the plane are fixed.

CAD model and moving reference frame (MRF)

However, when the true geometry is available and it is configured that it is rotating, the fan actually is not only delivering a pressure increase, but also a swirling effect. This is an effect of the rotation of the flow, that gives components that are not uniform into the radiator. For this reason, the adoption of the MRF method is closer to the real condition in terms of performance of the radiators. This is a trade-off that should be accepted. In addition, using the fan geometry (when available) also accounts for the boundary conditions. In this case, a rotating boundary condition is also rotating the reference frame. Hence, the moving reference frame MRF is a condition of the volume that defines that the cells into that volume are moving within a certain law. This is important, because just setting a condition of rotation is not enough to reproduce correctly the pressure increase. Hence, if it is performed just a simulation of the fan to verify if this geometry represents the pressure increasing that the calibration curve indicates, it will be possible to observe that the boundary conditions are not referred to. It is necessary to have a MRF to deliver the correct pressure increase.

There are a lot of adjustments considering the fan calibration, because it requires a MRF. This is recommended when there is a rigid body rotating. For instance, fans, brake discs and vanes are examples. Another important detail about the fan geometry is that the CAD file given by the supplier has its own coordinates, which means that it rotates in a certain direction. In addition, in many high performance and race cars applications, fans are used on both sides. Hence, understanding that cars are, in the best way, symmetrical and in the CFD environment the watertight model is split in half, the result for one side must be replicated to the other. The problem is that the fan rotation does not introduce a symmetric condition into the model. This effect also occurs in situations as seen in Figure 8. In this case, the swirling effect is guiding out of the flow. For instance, considering the inlet at the front bumper and outlet towards the windscreen, the result is that the flow took a curvy path and just to one side. This effect occurs, because there is just one of the radiators that is completely hot. For this reason, both fans and radiators positioned at the same place, but at opposite sides, exhibit different results, thus they are not symmetrical. This is the case of the forced fan.

Free-wheeling fan

It is important to mention that pressure jump is a different effect from pressure drop. Actually, this is the case of the free-wheeling fan. This is the same fan, but in different operating conditions. When the fan is not activated, it is free to rotate by free stream acting on the blades. Even though deactivated, the fan still exert some impact on the flow after the radiator. The supplier also shares the pressure drop curve. The fan has some inertia and the air has to overcome the fan inertia to pass through the radiator. Hence, when the car is at high speed, the fan is stealing some energy from the flow. A car at high speeds, the fan at free-wheeling conditions is disturbing the air flow. Therefore, with the pressure drop curve, it is possible to characterize the surface and set up the software in order to set the free stream which goes through the surface, a pressure drop according to the curve is defined by the supplier.

Another possible situation during aero development, is when there is no pressure drop curve, neither CAD model. In this case, the typical solution is just to neglect the inertia that would exist on the 3D surface that represents the fan. It is far from the best case, but it is not possible to make assumptions, since try and errors can led to an unpredicted scenario. Actually, the key point is the fan inertia, because with this data it is possible to calculate the pressure drop. The pressure difference is accounted over the static pressure. The blades of the fan have a small angle, that makes possible to create suction and compression while the fan rotates. Figure 8 illustrates a CFD simulation results, it is possible to notice the pressure coefficient variation over the blade surface. The main problem of cooling CFD simulations is that fan suppliers neither always send completely the data about its product.

Thermal management

The thermal management is important to investigate the effects of the temperature field, to understand the temperatures around the car. However, the main areas are the radiator, the exhausts and the effects of the exhaust gases on the air flow, the flow inside the engine bay and the brake cooling. Each of these examples are analyzed by different methods. For instance, flows that go through radiators get out from them in a hot condition and attach on different surfaces. These cases are usually analyzed using incompressible Navier-Stokes Equations (NSE). The radiators increase the airflow temperature, but in a value which is not enough to be necessary to consider the coupling effect between the velocity and temperature. In other words, the velocity is just creating convection of the temperature in some areas. At this kind of simulation, it is possible to solve the cold flow field and then switch off the flow variable and switch on just the temperature. By doing this, it is being activated the model where the temperature is conducting and overwhelming by the flow velocity. However, this one is not affected. It is necessary to go in a more complete set of NSE when the temperature is influencing the flow velocity.

Brake cooling

The braking cooling is a complex process in the point of view of the CFD analysis. However, the literature behind brake cooling is very wide and it offers a good base for preliminary study in terms of brake cooling. The huge improvement on this analysis was the Reynolds analogy. It states that the wall shear stress is linked to the heat transfer coefficient. Hence, it is possible to analyze the wall-shear stress and where it is higher, then the brake disc cooling will be more efficient. Conversely, where the wall shear stress is lower, the brake cooling efficiency will be lower, thus this region will exhibit higher temperatures. The Reynolds analogy can be performed in all simulations and exhibits thirty indications of how two different brake ducts are performing in terms of brake disc, which also requires detailed geometries and boundary conditions. In this case there is also a post convection. The heat generation of the brake depends on the situation. Usually, it is started with experimental data given by the supplier, which is the temperatures on the inboard and the outboard. Without this information an assumption is made, which is the heat generation based on the vehicle energy.

Under-hood thermal analysis

The under-hood is an environment where the engine, the gearbox, the intercooler, the catalyst converter and the muffler are, these are all heat sources that are going inside the engine bay. A detailed temperature map is necessary to characterize all these sources inside the model. This simulation is complex, because it is not just a matter of putting these sources inside the model. Actually, it is important to have a detailed geometry in the respective area of the model and the correct material. For instance, in the analysis of the rear wing, it is required an analysis of how hot is the rear frame and how much the body work is suffering with exhausts. This is possible when the correct material is characterized on the model. For instance, a carbon fiber body work requires that the model has the material correctly characterized. In case of titanium exhausts, all the models for thermal analysis are totally different from the external aerodynamics, which are watertight models. In this kind of simulations it is used solids with very well defined material characterization and then it is introduced their conductivity and radiation. Hence, the temperature surface make an important role, because of the radiation mechanism. In addition, there is also the convection, which can be natural or forced.

Heat soak analysis

Another important thermal simulation is the heat soak condition, which is the simulation of the car at a sudden stop after an intensive use. This is a quite common situation in cars, race or road going versions. The main heat sources are at their highest temperature, but it is stopped without a gradual release. It is a difficult process since there is a boundary condition that is changing in time, from the maximum value to the simulation temperature decreasing. Heat soak is also characterized by the vehicle’s steady condition, because in a pressure based finite volume, it is not advisable to assume velocity equal to zero. Usually, it is set at a very small velocity, about 0.2 m/s. In addition, a decreasing boundary condition is solved in time, which means a transient simulation. In this kind of simulation, applying NSE it is possible to preview that the natural convection is the dominant phenomena together with the radiation. This is a very complex simulation target in the thermal analysis to check and interpret the structure. It is not just a matter of aero performance, but also an analysis of how the structure behaves under a critical condition. Hence, it is also possible to evaluate the temperature distribution that can be used as loads, characterize them into the model and study how the structure performs.

Max speed analysis

The max speed simulation is a run which the model is characterized according to the boundaries at max speed, the sources are at the maximum output, but with the considerations regarding the external flow. This is flushing everywhere and it helps with the forced convection, radiation and conduction to cool all the area. Although this simulation also deals with the structural integrity, it is useful to evaluate how naca and other openings are effective in cooling down specific areas. Hence, in this simulation, the performance is also evaluated, which is the efficiency of the ducts. Being forced convection, this kind of simulation can be also applied to skins, which are typically performed with RANS equations. In this case all the components should be modeled as solids and with conjugated heat transfer. The huge difference is that it is a static simulation and there is no boundary condition variation.

Figure 11 illustrates an example of this simulation, a mid-rear engine car which its modeling accounts for the rear part of the monocoque. As can be seen, there are a lot of solid components on the engine bay region. However, the rest of the monocoque is partially solid, since only the body work is near to the engine. The reason is to analyze the structural integrity of the region.

References

1. Newbon, J., Dominy, R., and Sims-Williams, D., “CFD investigation of the effect of the salient flow features in the wake of a generic open-wheel race car,” SAE Int. J. Passeng. Cars – Mech. Syst. 8(1):2015, doi:10.4271/2015-01-1539;
2. Watts, M. and Watkins, S., “Aerodynamic Structure and Development of Formula 1 Racing Car Wakes,” SAE Int. J. Passeng. Cars – Mech. Syst. 7(3):2014, doi:10.4271/2014-01-0600.
3. This article was based on the lecture notes written by the author the Industrial Aerodynamics course attend at Dallara Academy.