During the 2000 Fluent Germany UGM, Dipl. Ing. Andreas Kleber from Adam Opel AG's International Technical Development Center presented a paper on his team's CFD design process for vehicle external aerodynamics. By way of illustration, he outlined the simulation approach for modeling the popular European coupe, the Opel Astra. Opel CFD engineers optimize the interaction between the software products they use to perform external aerodynamic simulations: UNIGRAPHICS, ANSA, GAMBIT, TGrid, and FLUENT. In doing so, they aim to produce high-accuracy CFD predictions in the shortest turn- around times without being limited by grid size, since they often perform several grid adaptions during the solution process. Typically eight processors of an SGI Origin 2000 computer are used for one run.

External aerodynamics simulation process at Opel AG

Opel employs a common CAE database that contains all of their car components in CAD format. The CFD Group can extract a base chassis from this database, and then add various components ranging from external mirrors to rear wing airfoils. The simulation process has been honed to the point where optimal unstructured hybrid meshes are being generated for each simulation. Meshes of more than 3 million cells are commonly used so that the complicated real-world geometries of production cars and the resultant flow-field physics and boundary-layer effects can be resolved.

The pre-processing software ANSA is used by Opel CFD engineers to produce a uniform triangular surface mesh. For volume grid generation, a hybrid mesh strategy using prismatic and tetrahedral elements is applied to realize highly automatic meshing. Prism layers are grown from the ground plane in front of the car and on the styling surfaces of the car body to provide a good resolution of the viscous boundary layer flow. Using a combination of TGrid, the Cooper quad meshing tool in GAMBIT, and non-conformal interfaces, complex geometry like external mirrors, underbody, or side window steps can be meshed effectively using tetrahedra or separate prism blocks. The height of each prism layer on the ground plane and on the car body is allowed to grow according to a geometric ratio that yields good initial y+ cell distributions and smooth transitions to the tetrahedral mesh in the external fluid region. Opel engineers seek to have a maximum cell skewness magnitude no greater than 0.8 in their CFD meshes.

Once the optimal 3D vehicle mesh is generated, the realizable k-e turbulence model, non-equilibrium wall functions, and second order upwind schemes are used in the FLUENT solver. During the solution process, the engineers typically use a total of 5 combined grid adaptions (hanging-node) to both y+ and static pressure gradient criteria. For each adaption, 1-2% of the total cell count is marked. Final convergence of the simulation is determined when f luctuations in lift and drag coefficients vary within ± 0.001.

The visualization of the computed flow-field data helps the development engineer evaluate the quality of a given aerodynamic concept. Although the absolute computed values of drag and lift coefficients can still be improved, these values can be used to compare different design studies at the very beginning of the vehicle development process when no hardware models are available. Another important product from the CFD simulation is the computation of forces acting on body parts (e.g., the front door frame) to support the FEM structural analysis.

In the future, the model complexity and the accuracy of the aerodynamic simulation will increase further. New CFD activities at Opel will also include the development of capabilities for aeroacoustics and water management.

Hybrid volume mesh
Insert: Non-conformal interfaces near the side mirror

FluentNEWS