ENGINEERING AND CFD

Introduction

With constantly growing fuel prices and toughening of environmental legislation, the vehicle industry is struggling to reduce fuel consumption and decrease emission levels for the new and existing vehicles. One of the ways to achieve this goal is to improve aerodynamic performance by decreasing aerodynamic resistance.

Rotating wheels together with the wheelhouses can produce up to 25% of the total aerodynamic drag. Furthermore, there are power losses associated with the resistance moments acting on the wheels; originating from the relative movement of the wheels in the air.

The improvement of vehicle aerodynamics requires the tools of aerodynamics development to perform at ever-increasing levels of accuracy. Computational Fluid Dynamic (CFD) is very important due to the complexity of problems and accuracy required. Requirements of CFD are high process integration to keep pace with vehicle development cycle and the accuracy of results must be reliable, especially where no experiments are available.

The Open-Source CFD is chosen in this project, because the commercial environment for CFD codes are truly viable for productive use with limited insight or the black-box approach.

The simulations of full car in a computational domain have been studied with rotating wheels and different parameters. And the forces and moments were calculated. The simulations were carried on on the HPC system SuperMUC of the Leibniz Supercomputing Centre in Garching near Munich.

Preliminary Results and Methods

For the project, the researchers selected the DrivAer model, which is developed at TU München in cooperation with the automotive industry companies BMW and Audi. The experiments reported in this project were executed in the Wind Tunnel A of the Institute of Aerodynamics and Fluid Mechanics at Technical University Munich, a 1:2.5 model wind tunnel with a blockage ratio 8%. The test section is 4.8m long, the cross section of nozzle exit is 4.32m². Vortex generators are installed at the nozzle exit to reduce the pressure fluctuations induced by the developing shear layers. The maximum wind speed is 65m/s. Four different setup experiments were studied which would be used to validate the simulation results.

For the numerical investigation the open source code OpenFOAM was chosen. The customizability of open-source software, along with the absence of licensing restrictions, is increasing its presence in the engineering and research environments [1]; the user has the choice of technology provider. Full transparency of technology permits complete analysis and solves problems which is very flexible for calculating the ventilation moment of the rotating wheels.

The pressure-velocity coupling in the present work is realized using the SIMPLE algorithm implemented in simpleFoam. For the Reynolds Averaged Navier Stokes Equations (RANS) simulations, the k-ω-SST (Shear-Stress-Transport) model following Menter [2] was chosen. The ω-equations has significant advantages near adverse pressure gradient flows leading to improved wall shear stress. The SST model combines the k-ω model near the wall and the k-ε model away from the wall as a unified two-equation turbulence model. It was developed for external aerodynamic flow simulation and has shown to be superior to other two-equation models in view of separation, lift and drag prediction.

The simulations were conducted at the velocity u = 41.2 m/s with rotating wheels, the turbulent intensity is 0.4% and the turbulent length scale is 1.5mm, which are in line with the inlet conditions during the wind tunnel experiment. To prevent backflow into the domain, the velocity boundary condition at the outlet was set to an inletOutlet condition. A no-slip boundary condition was enforced at the walls and a symmetry boundary condition was chosen for the wind
tunnel buffer.

First, the results of the body-shell alone without wheels and mirrors were compared to the simulation. It can significantly reduce the turn-around time for optimizing the numerical schemes and boundary conditions with the basic body, with less and easier cells regardless of the wheels. The model was positioned x=2000 mm downstream of the nozzle exit and the tests were conducted at a Reynolds number of Re=5.2 Mio, which corresponds to a freestream velocity of about 45 m/s. All the tests are conducted under moving ground. Table 01 shows the comparisons of the drag and lift coefficients with the experiments under the moving ground condition.

The simulations were computed in an idealized box. On the whole, good accuracy is obtained for the prediction of drag coefficient over different range of vehicles. The simulation has the best agreement with the experiment for sedan car, the station wagon.

The rotation of the wheels is approximated by imposing a rotatingWallVelocity boundary condition. The chosen wall function for the viscosity term imposes a continuous vt profile near the wall based on the velocity, as proposed by Launder and Spalding [3]. To solve the transport equations, a basic second-order scheme linearUpwind discretization was implemented for the divergence terms.

To compute the velocity components from the divergence term the Gauss bounded linearUpwindV scheme has been chosen. The Gauss linear scheme, a basic second-order gradient scheme using the Gauss theorem and face interpolation, was chosen as the base gradient scheme for the simulations. Gauss limited was chosen as the snGradSchemes based on the mesh information, normally when orthogonality bigger than 60, and cellimited Gauss linear scheme was used for gradSchemes, in order to avoid unphysically oscillation. In this project it addresses the accuracy of different methods to simulate the wheel rotating, like the multiple reference frame (MRF) and two ways using sliding mesh, seen in Fig. 2, and also the differences between Reynolds-averaged Navier-Stokes equations (RANS) and Delayed Detached Eddy Simulation (DDES), all compared with particle image velocimetry (PIV) data and drag forces for an isolated rotating wheel. The sliding mesh case wheel on ground gives a similar flow field like the MRF-DDES case. The flow filed around spokes in sliding mesh case is more rotating-symmetry than the MRF case.

In the next step, the full car simulations with DDES and sliding mesh is studied, in order to study the influence of wheel parameters, based on the DoE plan, there are 25 configurations covering 15 parameters of a automotive wheel, as seen in Fig. 3.