Design and Implementation of Fog Light Ducts to Optimize Hot Air Recirculation and Heat Transfer in the Toyota Hilux

This research adopted a computational approach supported by studies that have validated the combined use of CFD simulations and simplified thermal analysis techniques to understand hot air recirculation and its impact on the underhood cooling system under urban traffic conditions [5, 14].

To analyze the thermal behavior of the engine compartment over different operating periods, a transient study was developed using ANSYS CFX, based on a realistic three-dimensional geometry of a 2022 Toyota Hilux. The initial and boundary temperature conditions were configured according to the values reported in the manufacturer’s technical manual and reliable data from the automotive sector [15].

Figure 1 illustrates two simulated scenarios: (a) after 10 minutes of engine operation, and (b) after 1 hour of continuous operation. These simulations revealed the surface temperature distribution in critical engine components such as the cylinder head, engine sides, exhaust area, and radiator.

00001.png

Figure 1. Thermal evolution of Hilux: a) 10 Minutes, b) 1 Hour

Table 1. Typical temperature ranges of engine components and their sources

The model considered heat transfer by convection and conduction, in addition to the effect of fan-induced flow [16]. This approach has been used in previous studies, confirming the effectiveness of CFD tools to visualize heat accumulation, evaluate critical temperature conditions, and propose strategies for more efficient thermal evacuation [10, 17].

To facilitate the understanding of the thermal analysis, Table 1 was prepared based on technical information from manuals and official Toyota documentation [18]. These data served as the basis for the simulations conducted in ANSYS CFX, aiming to evaluate temperature behavior under steady-state conditions and analyze the heating of areas adjacent to the engine. A maximum temperature of 378 K was considered, corresponding to the normal operating conditions of a pickup truck under regular use. Although in the exceptional cases in which the surface temperature can reach up to 403 K due to cooling system failures or other overheating causes, the technical literature and manufacturer recommendations indicate a stable operating range between 373 K and 378 K.

2.1 Design, sizing, and preparation of ducts

Two three-dimensional designs (Designs A and Design B) were developed in SolidWorks, adapted to the available space behind the fog lights of a 2022 Toyota Hilux [18].

Real dimensions and structural constraints of the front compartment were respected to ensure physical compatibility and to avoid interference with other components. The region where the airflow impacts the engine surface is shown below, as defined in Figure 2.

0002.png

Figure 2. Flow impact area at the duct outlet

Two inverted “Z”-shaped designs (660 mm) were created with smooth transitions to reduce pressure losses and optimize unused space inside the vehicle (Figure 3).

However, in the area adjacent to the suspension, a critical decision had to be made regarding whether the routing would follow an internal or external path relative to it, ensuring sufficient clearance between the chassis and the tire without restricting its movement.

In the case of Design A, which features minimal directional changes, a square profile was selected to maximize airflow and efficiently utilize the available area.

The duct design was based on carefully defined geometric parameters. The total height of the inlet profile was 126 mm, measured from the bottom to the top edge in the side view, which defines the visible front contour. The inlet width progressively narrowed from 100 mm (top) to 74 mm (bottom), promoting flow acceleration. The front section, including its initial narrowing, is 90 mm long, ensuring efficient frontal air capture as it directs airflow toward the fender liner area.

The first ascending diagonal measured 260 mm in height, designed to avoid interference with the front tire by positioning the duct above the clearance space between the tire and the chassis. In the top view, the inlet depth from the front plane to the first bend of the duct measured 330 mm. The second diagonal (descending) measured 250 mm in height, allowing the duct to be routed above the structural level of the chassis support. The inlet-to-outlet section is 280 mm long, allowing the airflow to stabilize before the final curvature. In the case of Design B, this outlet featured a curvature radius of 30 mm, strategically oriented toward the underside of the vehicle to aid in the evacuation of hot air from the thermal compartment.

Design B, which incorporated multiple 90° bends, required the adoption of a circular profile due to its smooth transition between curvature changes. This also minimized welded joints or couplings during manufacturing, regardless of the selected material.

00031.png

00032.png

Both models were exported as closed solids for aerodynamic analysis via CFD simulation. To determine the performance of both duct designs, CFD simulations were conducted under identical conditions, considering vehicle speeds of 2.78 m/s and 33.33 m/s.

To ensure proper resolution of flow characteristics within ducts A and B, a structured mesh was implemented for both designs. Given the range of inlet velocities (2.78 m/s to 33.33 m/s), a refined tetrahedral mesh was used in wall-adjacent zones of Design A, while for Design B, which features a circular geometry, a shell-type mesh was employed, as it was easier to generate in such regions (Figure 4). Element size was adjusted to strike a balance between computational cost and the fidelity required to capture phenomena such as recirculation zones, pressure losses, and vortex formations. This approach is consistent with recommended practices in the technical literature, which emphasize the importance of mesh refinement in areas with high gradients and the use of adaptive techniques to maintain accuracy without significantly increasing computational cost [19].

00041.png

00042.png

In Table 2, the mesh refinement analysis conducted for Models A and B enabled the identification of the stabilization threshold for the variable of interest (maximum flow velocity), ensuring the numerical reliability of the CFD simulations. For Model A, the relative variation between consecutive simulations progressively decreased, reaching a difference below 0.1% from approximately 2 million elements (Simulation A5). Similarly, Model B showed clear stabilization starting at 1.7 million elements (Simulation B6).

Table 2. Properties of the boundary conditions of the refrigeration system

These results indicate that both models achieve mesh-independent convergence at these discretization levels; thus, using a mesh with over 2 million elements represents a suitable compromise between numerical accuracy and computational cost. This step is essential to ensure that the differences observed between duct configurations are due to geometric conditions rather than errors caused by insufficient mesh resolution.

It should be noted that the effects of active grille shutters and PWM-controlled fans were not included in the present model, as the focus was restricted to passive duct geometries. Future studies should incorporate these elements to better capture their influence on flow distribution and hot air recirculation.

The CFD simulations were carried out in ANSYS CFX using the SST k-ω turbulence model, which is well-suited for capturing velocity gradients and dissipation near walls in confined flows. Operating conditions at 2.78 m/s (representing low-speed urban traffic) and 33.33 m/s (representing highway driving) were evaluated, defining uniform flow inlets, no-slip conditions on walls, and ambient pressure outlets [10, 17]. Although idle corresponds to 0 m/s with fan-dominated flow, the present study focused on low-speed free-stream conditions (2.78 m/s) to ensure airflow interaction with the ducts.

Table 3 summarizes the boundary conditions assigned at the nozzle inlet for both simulation cases, corresponding to low and high speeds. Relevant parameters such as flow regime, inlet velocity, turbulence model, and fluid properties are detailed, which were essential to ensure consistency in the comparison of results between both scenarios.

Table 3. Inlet boundary conditions at the nozzle

Specifically, the inlet was configured as subsonic flow with two representative velocity scenarios: one at 2.78 m/s (low-speed urban traffic) and another at 33.33 m/s (highway driving), corresponding to urban and highway conditions, respectively. For the simulation, the k–ε turbulence model was employed, widely used in automotive analyses for its balance between accuracy and computational efficiency. This model has shown good performance in CFD underhood studies, where it is necessary to reliably capture turbulence effects in complex geometries without incurring high computational cost [20]. Key parameters such as turbulent kinetic energy (k = 0.05 m²/s²), turbulent dissipation (ε = 0.1 m²/s³), and the static flow temperature (298 K) were defined as boundary conditions at the inlet [21].

Continuity:

$\frac{\partial\left(\rho u_j\right)}{\partial x_i}=0$             (1)

and the momentum equations are expressed by:

$\frac{\partial\left(\rho u_i u_j\right)}{\partial x_i}=-\frac{\partial p}{\partial x_i}+\frac{\partial}{\partial x_i}\left[\left(\mu+\mu_t\right)\left(\frac{\partial u_i}{\partial x_j}+\frac{\partial u_j}{\partial x_i}\right)\right]+\rho g_i$                   (2)

Energy (enthalpy form):

$\rho c_p u_j \frac{\partial T}{\partial x_i}=\frac{\partial}{\partial x_i}\left[\left(\lambda+\lambda_t\right) \frac{\partial T}{\partial x_i}\right]+S_T$                (3)

k-equation:

$\frac{\partial\left(\rho k u_j\right)}{\partial x_i}=\frac{\partial}{\partial x_i}\left[\left(\mu+\frac{\mu_t}{\sigma_k}\right) \frac{\partial k}{\partial x_i}\right]+P_k-\rho \varepsilon$                  (4)

$\varepsilon$-equation:

$\frac{\partial\left(\rho \varepsilon u_j\right)}{\partial x_i}=\frac{\partial}{\partial x_i}\left[\left(\mu+\frac{\mu_t}{\sigma_{\varepsilon}}\right) \frac{\partial \varepsilon}{\partial x_i}\right]+C_{\varepsilon 1} \frac{\varepsilon}{k} P_k-C_{\varepsilon 2} \rho \frac{\varepsilon^2}{k}$                (5)

Turbulent viscocity:

$\mu_t=\rho C_\mu \frac{k^2}{\varepsilon}$               (6)

Turbulent thermal conductivity:

$\lambda_t=\frac{\mu_t c_p}{P r_t}$              (7)

To ensure a comprehensive analysis, the engine and radiator were also modeled in ANSYS to enable subsequent evaluations both through applied calculations in MATLAB, using the aforementioned heat transfer and fluid dynamics equations, and through CFD simulations in ANSYS CFX [22]. The goal is to establish a reliable comparison between analytical and numerical results. Initially, the objective is to achieve stable outcomes by leveraging the meshing strategies previously discussed. Although the mesh refinement was specifically applied to the ducts, it serves a critical role in identifying which design better fulfills the purpose outlined in the introduction: enhancing the recirculation of hot gases.

To assess this, the outlet velocity of both ducts must be quantified, along with the pressure they exert on the duct walls, which translates into mechanical loads on the vehicle's mounting structures. This evaluation also contributes to identifying which design imposes lower structural loads on the vehicle chassis. Once the optimal duct configuration is selected based on these criteria, a coupled thermal-fluid analysis will be performed including the engine and radiator.

This will determine the heat transfer behavior at vehicle speeds of 2.78, 8.33, 13.89, 22.22, and 33.33 m/s (equivalent to 10, 30, 50, 80, and 120 km/h), enabling the quantification of the thermal differential (ΔT) introduced by the duct system under realistic operating conditions.

However, it should be emphasized that the structural evaluation was restricted to aerodynamic loading and did not include long-term material degradation phenomena. In particular, PP+GF composites commonly used in bumper and duct systems have a continuous-use temperature limit of approximately 90℃, which is lower than the 105℃ zones identified in the present simulations. Therefore, future studies should include creep and fatigue assessments under combined thermal and pressure loads to fully validate the durability of the solution.

2.2 Meshing and preparation of the engine and radiator

The engine, like the Toyota Hilux pickup truck, was not modeled as a traditional solid but was developed from STL files obtained through 3D scanning. This format poses significant challenges for meshing in CFD-dedicated software due to the high number of generated surfaces. To enable its analysis, the geometries were cleaned and smoothed using SolidWorks and later ANSYS Discovery. The truck model alone exceeded 5 million surfaces, while the engine surpassed 2.3 million, without accounting for the additional complexity introduced by the internal hood compartment, which significantly increased the surface count.

Once the surfaces were optimized in Discovery, the engine model was exported in STEP format, allowing for better integration into ANSYS meshing module. There, a mesh consisting of 7,239,603 elements was generated (Figure 5), pushing the limits of the computing system used (Intel Core i9 processor with 32 GB of RAM). Figure 6 presents representative details of the final engine mesh.

0005.png

00061.png

00062.png

To evaluate the thermal performance of the selected duct, the analysis of convective heat exchange generated by the impact of the airflow on the thermal modules was considered [23]. This phenomenon can be described using the classical equations for forced convection heat transfer, which make it possible to quantify the heat flux transferred from the air to the impacted component [24]. Their application enables a quantitative assessment of the effectiveness of the proposed solution with the redesigned ducts [21, 23].

The air properties are required for the calculation of the dimensionless parameters and the convective coefficient. These properties are evaluated at a mean temperature close to that of the air jet [25, 26]. The expressions are:

Air density $(\rho)$:

$\rho=\frac{P}{(R . T)}$                  (8)

Dynamic viscosity of air $(\mu)$:

$\mu=\mu_0 \cdot\left(\frac{T}{T_0}\right)^{\frac{3}{2}} \cdot \frac{\left(T_0+C\right)}{(T+C)}$                 (9)

The Prandtl number was used as a parameter relating momentum diffusion to heat diffusion. It is defined as:

$\operatorname{Pr}=\frac{c_p \cdot \mu}{k}$               (10)

Thermal conductivity of air (k):

$k=k_0+k_1 T+k_2 T^2$             (11)

where, $c_p$ is the specific heat of air at constant pressure $\frac{{J}}{{kg} \cdot . {K}}$, $\mu$ the dynamic viscosity of air Pa.s and $k$ the thermal conductivity of air $\frac{W}{m \cdot K}[27,28]$.

$R e=\frac{\rho \cdot U \cdot D}{\mu}$             (12)

where, $\rho$ represents the air density $\frac{{kg}}{{m}^3}, U$ the mean flow velocity $\frac{m}{s}, D$ the hydraulic diameter of the duct $m$, and $\mu$ the dynamic viscosity of air [29, 30].

The Nusselt number was used as the dimensionless parameter relating convective heat transfer to conductive heat transfer within the fluid [28, 31], defined as:

$N u=\frac{h_{ {convection}} \cdot D}{k}$                  (13)

where, $h_{\text {convection }}$ is the convective heat transfer coefficient $\frac{W}{m^2 \cdot K}, D$ the hydraulic diameter of the duct $m$, and $k$ the thermal conductivity of air $\frac{W}{m . K}$.

This number allows the evaluation of the efficiency with which heat is transferred from the duct walls to the air flow or vice versa [21]. Its value depends on the flow regime (laminar or turbulent), the thermophysical properties of the air, and the duct geometry. For internal flows with well-defined conditions, widely accepted empirical correlations exist to estimate the Nusselt number as a function of the Reynolds and Prandtl numbers.

The convective heat transfer coefficient h represents the ability of the air flow to transfer heat from the engine surface to the environment or vice versa. It is calculated from the Nusselt number by the expression:

$h=\frac{N u . k}{D}$               (14)

where, $N u$ is the Nusselt number, $k$ the thermal conductivity of air $\frac{W}{m v}$ and $D$ the hydraulic diameter of the duct or nozzle.

This coefficient has units of $\frac{W}{m^2 \cdot K}$, and its value depends on air velocity, channel geometry, and the thermal properties of the fluid. A higher $h$ value indicates more efficient heat transfer between the flow and the surface.

The heat transfer rate from the hot surface to the airflow is calculated using forced convection [32]. However, under real conditions, losses due to natural convection and thermal radiation to the surroundings also occur, and these must be considered to obtain the net useful heat flow.

The net heat flow by convection is defined as the amount of thermal energy transferred exclusively by forced convection to a surface impacted by an air jet, discounting the contributions from other heat transfer mechanisms such as natural convection and thermal radiation. This estimation makes it possible to isolate the actual effect of the jet on the cooling of the analyzed surface [23].

Mathematically, it is expressed as:

$q_{ {convection }}^{\prime \prime}=q^{\prime \prime}-\left(q_{ {nat }}^{\prime \prime}+q_{{rad,front }}^{\prime \prime}+q_{ {rad,back }}^{\prime \prime}\right)$               (15)

$q_{n a t}^{\prime \prime}=h_{n a t} \cdot\left(T_\omega-T_{a m b}\right)$               (16)

$q_{r a d}^{\prime \prime}=\sigma \cdot \varepsilon_{f / b} \cdot\left(T_\omega^4-T_{a m b}^4\right)$                  (17)

The supplied heat is equal to the steady-state heat loss in the absence of jet impact; therefore, Eq. (15) represents the heat flux balance.

$q^{\prime \prime}=q_{ {nat }}^{\prime \prime}+q_{{rad,front }}^{\prime \prime}+q_{ {rad,back }}^{\prime \prime}$                 (18)

Once the net heat flux is determined, the amount of thermal energy extracted from the component over a specified time interval can be estimated. From this, the corresponding temperature drop and the final temperature reached can then be obtained [32].

Extracted energy:

$Q=q_{ {net}} \cdot t$           (19)

Thermal reduction of the component:

$\Delta T=\frac{Q}{m \cdot c_p}$               (20)

Final temperature:

$T_{\text {final }}=T_{\text {surface }}-\Delta T$                   (21)

This set of equations was implemented in MATLAB and validated through numerical simulations under varying conditions of vehicle speed, ambient temperature, and initial engine temperature. The results provided a quantitative assessment of the influence of these parameters on cooling effectiveness.

Application of these equations requires prior knowledge of variables such as flow velocity, air temperature at different points within the system, and static pressure. These parameters were obtained from computational fluid dynamics (CFD) simulations of the developed geometric models. The simulation outputs further enabled the calculation of the Reynolds and Prandtl numbers, and subsequently, the Nusselt number, using well-established empirical correlations for air jets impinging on heated surfaces.

The study demonstrated that the redesigned rectangular duct (Design A) provides a more reliable and energy-efficient airflow delivery to the engine compartment. Beyond aerodynamic improvements, its implementation enhanced heat transfer by forced convection, achieving measurable reductions in surface temperature that complement the vehicle’s primary cooling system. Structural evaluations through modal analysis confirmed that the duct maintains adequate stiffness, and that the addition of an intermediate support further increases natural frequencies and reduces effective modal masses, minimizing the likelihood of resonance under operational excitations.

The methodological integration of analytical modeling in MATLAB with numerical simulations in ANSYS CFX ensured robust validation of the results, reinforcing confidence in the predictive capability of the proposed workflow. From a practical standpoint, the findings suggest that the solution can be extended to other vehicles facing similar challenges of thermal recirculation, with minimal structural modifications and without significant increases in computational or manufacturing cost.

Future work should include experimental validation under real operating conditions, evaluation of material durability under thermal–vibrational loads, and the integration of active cooling strategies to further enhance system performance. These aspects will provide a more comprehensive framework for the adoption of the proposed design in automotive applications.