Converging-diverging transonic diffuser

Confined flows

Underlying Flow Regime 4-19

Description

Introduction

Compressible flow phenomena due to high speed and their interaction with turbulence are a very interesting scientific area of fluid mechanics. Flows with compressible characteristics are present in many internal and external mechanical design configurations such as external flows related to aeronautics, and confined/internal flows in inlets and around compressor blades in turbomachinery. Regarding the confined flows, a very interesting area of research is the experimental and computational study of compressible flows inside transonic diffusers, which is the topic of the current UFR.

The flow features that are present in transonic diffusers and characterize the flow field development can be found in supersonic inlets of air-breathing systems of missiles and aircrafts. As reported by Bogar et al. (1982), the flow patterns in the converging-diverging diffusers, occur in supercritical and subcritical inlets, in transonic airfoil flows, and in transonic compressor rotor passages. Studies of these patterns are very helpful for the design and optimization of propulsion systems such as ramjets. The basic characteristic of a transonic converging-diverging diffuser flow is the formation of a shock-wave in the “throat” of the diffuser. The position and the intensity of the shock-wave depends on the diffuser geometry and also strongly on the inlet and outlet boundary conditions. Additionally, there is a strong interaction between the formed shock-wave and the boundary layer development inside the diffuser. Downstream of the shock-wave there is a subsonic region with adverse pressure gradient and hence a strong possibility of boundary layer separation in the diverging part of the diffuser, depending on the inlet and outlet conditions. All the above make the current UFR very interesting for developing and testing various turbulence modelling and simulation techniques (RANS and or LES). However, there is limited information in the literature regarding the behavior of the turbulent correlations and turbulent energy budgets such as turbulent production, destruction, pressure strain- correlation and Reynolds-stress quantities distributions in the shock-wave and the wall regions.

The accurate modelling of the converging-diverging transonic diffuser flow is a considerable challenge for turbulence models. The models must be capable of predicting correctly the complex flow phenomena. Additionally, the turbulence models must be able to take into account all the mean density variations that become important due to the compressibility at high speeds and properly correlate them with the mean flow characteristics of the transonic/supersonic flow.

The test case investigated in the current contribution under the framework of the described UFR is the Sajben converging-diverging diffuser. Two flow field developments are examined, one with a weak and one with a strong shock-wave formed at the transonic diffuser throat. A characteristic sketch of the Sajben converging-diverging diffuser and the relative position of the two formed shock-waves are shown in fig.3.

Figure 3: View of the Sajben converging-diverging transonic diffuser

Review of UFR studies and choice of test case

In the literature, there are plenty of works that have examined computationally and experimentally the compressible flow field development in transonic diffusers together with the shock-wave formation. Before focusing on studies relating to the Sajben diffuser, a brief review is given on work performed on other diffuser geometries. A general review on turbulence modelling for compressible flows can be found in Vlahostergios and Yakinthos (2015). Biedron and Adamson (1988) investigated the unsteady 2D flow in a supercritical supersonic diffuser with asymptotic methods. They calculated the shock-wave response to imposed backpressure oscillations and the flow separation inside the diffuser. Handa et al. (2002) studied experimentally and computationally the multiple shocklets formation in a transonic diffuser. The experiments were performed with a high-speed CCD camera and the computations were based on the 1D Euler equations. The results showed that the shocklets formation is strongly related to the transonic diffuser geometry. Park et al. (2008) investigated numerically the effect of various parameters on a supersonic exhaust diffuser. They adopted a low-Reynolds number k-ε model and also incorporated Sarkar's compressibility corrections in order to take into account the effect of compressibility on turbulence. Ghosh et al. (2008) used LES with high-order numerical schemes for the simulation of the compressible flow in nozzles and diffusers. They studied a supersonic diffuser with an inlet Mach number equal to 1.8 and investigated the effect of extra strain and dilatation rates on turbulence structures. Yaga et al. (2013), studied experimentally the control of an unsteady transonic diffuser flow with a piezoceramic actuator.

The transonic converging-diverging diffuser which is the test case in the current contribution, is called Sajben transonic diffuser in the literature. It has been widely investigated experimentally and numerically. Various experimental setups of the Sajben diffuser were studied in the past with different experimental conditions, focusing on the design optimization of supersonic inlets of air-breathing propulsion systems of aircrafts and missiles such as ramjets. Salmon et al. (1982) carried-out detailed LDA measurements for the streamwise velocity component with and without externally induced periodic oscillations. Bogar et al. (1982) investigated experimentally the time scale characteristics of the flow with shock induced boundary layer separation for strong Mach numbers. Sajben et al. (1984) provided experimental data for the same diffuser with an exit-to-throat pressure-ratio of 1.52. Both studies concluded to useful results regarding the boundary layer shock-wave interaction. Finally, Bogar (1985) made two-component LDA measurements with self-exited oscillations and separated boundary layer.

The available experimental data and the relatively simple geometry setup regarding the CFD domain configuration, makes the test case very attractive for CFD code validation. Additionally, the test case involves many complicated flow phenomena interacting with each other. For instance, shock-wave/turbulent boundary layer interaction, combination of subsonic and transonic flow phenomena and recirculation region formation, depending on the Mach number and the shock-wave intensity. The above mentioned characteristics make it attractive for validating computational models and techniques for transonic flows. Although the experimental measurements of the Sajben diffuser involve unsteady characteristics and periodic pressure oscillations, in the literature only the steady state case has been extensively examined using CFD. Additionally, the turbulence models that have been implemented for the modelling of this specific flow are, (apart from the work of Neel et al. (2003) and the current contribution), simple algebraic zero-equation models or some widely used two-equation k-ω and low-Reynolds k-ε eddy-viscosity models.

The available measurements provide profiles on various cross sections for the statistically averaged axial velocity and static pressure distributions along the diffuser walls. A collection of five computational studies of the Sajben diffuser flow using various computational codes and turbulence models, thereby validating the performance of the various turbulence models, can be found in the NPARC Alliance CFD Verification and Validation Web site of NASA (http://www.grc.nasa.gov/WWW/wind/valid/archive.html). The five test cases of the NASA web site are described briefly below:

Study 1 (Contributor C. Towne ): The study compares different computational codes (WIND, PARC and NXAIR). For the validations only the weak Mach number case is examined with the use of a structured body-fitted computational grid. The computational grid was based on the study of Georgiadis et al. (1994). The adopted turbulence models were the algebraic two-zone turbulence model of Baldwin and Lomax (1978) (BL) (for the PARC and NXAIR codes) and the one-equation model of Spalart and Allmaras (1992) (SA) (for the WIND code). This study was last updated in 2008. Additional details can be found in the work of Bush et al. (1998).

Study 2 (Contributor D. Yoder ): The study compares both the weak and the strong Mach number cases calculated with the NPARC and WIND computational codes, using a structured computational grid. Two eddy-viscosity turbulence models have been adopted: the Chien k-ε model (in WIND and NPARC codes) and the k-ω SST model (in WIND code). Especially for the strong Mach number case, only the Chien k-ε model with the WIND code was examined with additional modifications in order to capture more accurately the compressibility phenomena. In particular, the Sarkar compressibility correction and the variable eddy-viscosity coefficient C_μ were adopted. The first correction increases the dissipation rate for higher Mach numbers and the second one reduces the computed high eddy-viscosity values. As an overall conclusion, the Chien k-ε model provided the better results, especially for the strong Mach number case with both the adopted corrections. This study was last updated in 2008.

Study 3 (Contributor J. Slater ): The study investigates only the weak Mach number case with 3 variants of the WIND structured code with the time marching scheme, by adopting the SA model and the SST model. The computational results were compared with the experimental velocity and the pressure distributions and were similar for both models, with the SST model giving slightly better distributions that were closer to the experiment. This study was last updated in 2008.

Study 4 (Contributor S. Mohler ): The study utilizes the WIND unstructured flow solver and computes the strong Mach number case with the adoption of the SA turbulence model. The results showed that the SA model calculates a recirculation region much larger than the one found in the experiment. This study was last updated in 2008. Further details can be found in the work of Mohler (2005).

Study 5 (Contributor J. Dudek ): The last study of the NASA CFD validation archive validates the performance of the WIND CFD code with the use of the SA and the SST k-ω turbulence models by using structured and unstructured grids with both the structured and unstructured solver versions of WIND. For the computational runs, three different grids were used i.e. a structured, an unstructured and an extended outlet unstructured grid. The last grid was used for stability reasons since without extension, the unstructured flow solver was not able to stabilize and reattach the resulting recirculation region up to the diffuser outlet boundary. The final results with the extended outlet were slightly improved regarding the recirculation reattachment but did not provide qualitative velocity distributions in comparison with the experiments. This study was last updated in 2012.

Further studies regarding the Sajben transonic diffuser are those of Georgiadis et al. (1994), who calculated the current UFR with the PARC code by using five different turbulence models. In particular they adopted three algebraic zero-equation models: the Thomas (1980) model, the BL and the modified mixing length Thomas model of Georgiadis et al. (1992). Regarding the two eddy-viscosity low-Reynolds number two-equation models, they adopted the Chien (1982) k-ε model with an implementation for the compressibility corrections and the Speziale et al. (1990) k-ε model. In their study they included both the weak and the strong Mach number cases. Additionally, they also studied a case in which the pressure at the outlet boundary was increased and no shock-wave was formed in the diffuser, referred to as the no-Mach number case. They provided velocity and pressure distributions for the averaged steady cases compared with experimental data for all cases and they concluded that, especially for the strong Mach number case, the eddy-viscosity models performed better among the five adopted turbulence models. Hosder et al. (2002) examined the weak and the strong Mach number Sajben diffuser test cases in order to validate CFD simulations with respect to various uncertainty parameters. They adopted the SA and the Wilcox k-ω turbulence models and concluded that the most difficult case for providing accurate results is the case with the strong Mach number where a flow separation is present. Neel et al. (2003) used only the weak Mach number case of the current UFR study in order to validate the GASP CFD code. They adopted various turbulence models such as the SA, the Chien k-ε, the Wilcox k-ω, the SST and the linear RSM model of Wilcox with also Wilcox compressibility corrections applied. They concluded that the RSM model predicted with better accuracy the core flow but failed to give qualitative correct results in the near wall regions. Xiao and Tsai (2003) modelled the Sajben transonic diffuser by adopting the Wilcox k-ω model combined with the "lag model" of Olsen and Coakley (2001). The incorporated "lag model" is able to calculate more accurately the transport of the turbulent eddy-viscosity in non-equilibrium turbulent flows. They modelled both the weak and strong Mach number cases for steady and unsteady flow conditions. The periodic unsteadiness of the flow field was imposed by an oscillating back pressure of the outlet boundary. They concluded that the implementation of the "lag model" to the Wilcox k-ω turbulence model improves significantly the flow field development compared with the experimental data for both steady and unsteady cases of the diffuser. Zha and Hu (2004) provided a new scheme which is based on the concept of upwind and split pressure (CUSP) and is able to provide improved solutions for resolving boundary layers and capturing crisp shock-waves. They selected for validation both weak and strong Mach number cases of the Sajben transonic diffuser. They provided only the pressure distributions along the diffuser walls and the position of the shock-wave by implementing for the turbulence modelling the algebraic Baldwin-Lomax model. The results were not in good agreement with the experiments, especially for the strong case, and they reported that a more sophisticated turbulence model should be adopted, as the choice of the turbulence model is a critical factor for accurately predicting the shock-wave/turbulent boundary layer interaction.

The Sajben diffuser is also the case for the current UFR contribution which comprises mainly additional calculations with different turbulence models including more advanced ones. The models used are based on different turbulence modelling concepts i.e. the eddy-viscosity assumption with both linear and non-linear Reynolds-stress expressions and the transport equations of the Reynolds-stresses. The adopted turbulence models are the linear eddy-viscosity (LEVM) model of Launder and Sharma (1974), the cubic non-linear eddy-viscosity model (NLEVM) of Craft et al. (1996) and a modified version of the non-linear Reynolds-stress model (RSM) of Craft (1998). Additionally, the effect of the compressibility correction of Sarkar et al. (1989) for the dilatation-dissipation on the performance of the adopted turbulence models was investigated. The current contribution is based on the work reported in detail in Vlahostergios and Yakinthos (2015) which is from here on referred to as VY.

An overview of the above mentioned computational studies of the Sajben transonic diffuser (including the present one) with the corresponding turbulence models is given in table 1.

Contributed by: Z. Vlahostergios, K. Yakinthos — Aristotle University of Thessaloniki, Greece