Gianluca Iaccarino Center for Turbulence Research, Stanford University, Stanford, CA 94305-3030 Predictions of a Turbulent Separated Flow Using Commercial CFD Codes Numerical simulations of the turbulent flow in an asymmetric two-dimensional diffuser are carried out using three commercial CFD codes: CFX, Fluent, and Star-CD. A low- Reynolds number k- model with damping functions and the four-equation v ' 2 - f model are used; the first one is available as a standard feature in all the codes, the v ' 2 - f model was implemented using the User Defined Routines. The flow features a large recirculating zone due to the adverse pressure gradient in the diffuser; the v ' 2 - f predictions agree very well with the experiments both for the mean velocity and the turbulent kinetic energy. The length of the separation bubble is also computed within 6 percent of the measured value. The k- calculations do not show any recirculation and the agreement with the measurements is very poor. The three codes employed show very similar characteristics in terms of convergence and accuracy; in particular, the results obtained using the v ' 2 - f are consistent in all the codes, while appreciable differences are obtained when the k- is employed. DOI: 10.1115/1.1400749 1 Introduction Computational Fluid Dynamics tools are becoming standard in many fields of engineering involving flow of gases and liquids; numerical simulations are used both in the design phase to select between different concepts and in the production phase to analyze performance. Industrial CFD applications require high flexibility in the grid–generation procedure for complex configurations, short turn around time, and easy–to–use environments. At present, several commercial packages are available for the CFD industrial community; these packages are usually integrated sys- tems which include a mesh generator, a flow solver, and a visual- ization tool. Often the numerical techniques adopted in these CFD codes are well accepted algorithms published in the open litera- ture; the selection of one technique with respect to others is usu- ally based on robustness and reliability. There have been few attempts in the literature to compare the performance of these codes; laminar and turbulent test cases have been proposed to several CFD code vendors by the Coordinating Group for Computational Fluid Dynamics, of the Fluids Engineer- ing Division of ASME1. A series of five benchmark problems were calculated, with all the mesh generation and simulations per- formed by the vendors themselves; only two of the problems re- quired turbulent simulations. The first problem is the flow around a square cylinder; the flow is unsteady and all the codes predicted reasonably well the measured Strouhal number. However, poor accuracy resulted in the prediction of the details of the wake flow field. It was also noted that, depending on the code used and assuming grid-converged results the same k - model predicted very different results. The reasons for this difference can be dif- ferent grids, no demonstration of grid convergence, different implementations of the models, and different boundary conditions. It must also be pointed out that the prediction for this problem is strongly affected by the treatment of the stagnation point region. As shown by Durbin 2, the k - models predict a spurious high level of turbulent kinetic energy in this region. The other turbulent problem reported by Freitas 1 was the three-dimensional developing flow in a 180 degrees bend. In this case all the solutions reported were unsuccessful in predicting the measured data in the bend region and the resolved structure of the flow field was significantly affected by the choice of the turbu- lence model. The uncertainties associated with i  different computational grids, ii  boundary conditions definition, iii  convergence, and i v  numerical schemes do not allow drawing specific conclusions about the codes used, other than the usual conclusion that further research into more advanced turbulence models for use in com- mercial CFD codes is required 1. In order to carry out a fair comparison between different CFD codes and to establish definitive conclusions on the state–of–the– art of commercial CFD codes, all the differences i - i v  must be fully addressed and, if possible, eliminated. In the present work, an effort has been made to control all these parameters. The codes available for comparison are CFX, Fluent, and Star-CD. The ob- jective is to compare their predictive capabilities for the simula- tion of a turbulent separated flow. Several turbulence closures and near-wall treatments are available in these codes ranging from k --type models to full Reynolds stress models. The main focus of the work is on two models: the k - low-Reynolds model by Launder and Sharma 3 and the v ' 2 - f by Durbin 4. In addition, results obtained using different closures are reported. The k - model is well described in the literature and has been widely used. Its implementation poses some challenges and it re- quires the solution of two transport equations with numerically stiff source terms. This model is available in all the codes consid- ered and, although it is not expected to be extremely accurate 5, it provides common ground for comparisons between different codes. The v ' 2 - f model implemented in a NASA research code has been already successfully used for simulating separated flows 4, three dimensional configurations 6 and flows with heat transfer 7. It is rather complex involving the solution of four differential equations three transport equations plus an Helmotz-type equa- tions. The test case analyzed in this study is a two-dimensional tur- bulent flow in a diffuser. Due to the adverse pressure gradient the flow is separated and a large recirculation bubble is generated. This problem has been selected because a very reliable experi- mental database is available. Moreover, a detailed Large Eddy Contributed by the Fluids Engineering Division for publication in the JOURNAL OF FLUIDS ENGINEERING. Manuscript received by the Fluids Engineering Division October 16, 2000; revised manuscript received May 21, 2001. Associate Editor: I. Celik. Copyright © 2001 by ASME Journal of Fluids Engineering DECEMBER 2001, Vol. 123 Õ 819