AC 6-12 Best Practice Advice

Front Page

Description

Test Data

CFD Simulations

Evaluation

Best Practice Advice

Steam turbine rotor cascade

Application Challenge 6-12               © copyright ERCOFTAC 2004

Best Practice Advice

Best Practice Advice for the AC

Key Fluid Physics

Turbomachinery internal flows belong to the most complex ones in practical applications of fluid dynamics. It follows from complicated geometry of flow passages, three-dimensional flow character with substantial effects of secondary flows, shock-wave/boundary-layer interaction, laminar-turbulent transition, heat transfer, rotation, and effect of further parameters.

Because of the complexity of transonic flow in the three-dimensional cascades, the attention is concentrated to the two-dimensional transonic flow through the blade cascade. The flow through the steam turbine rotor cascade at the transonic regime is the test case. The flow regime near the design conditions with the inlet angle β₁ = 70.7 deg and the isentropic exit Mach number M_2is = 1.198 was selected for the application challenge. The chosen flow regime is characterized by the supersonic exit. The supersonic compression accompanying by transonic expansion occurs on the suction side approximately at the half of the chord. The compression is a consequence of the discontinuity of the curvature of the suction side surface. This local supersonic compression precipitates the laminar/turbulent transition. The inner branch of the exit shock waves reflects on the suction side of the neighbouring profile in a regular structure at the interaction with the turbulent boundary layer. The wakes in the supersonic exit regime are relatively thin.

The test case experiment was made for the inlet angle β₁ = 70.7 deg with the exit isentropic Mach numbers changed in the range (0.489, 1.387). Besides the transonic regime with M_2is = 1.198 corresponding to nearly design conditions, the subsonic regime with M_2is = 0.716 was chosen for verification of CFD codes.

The governing aerodynamic and geometric parameters are the inlet Mach number, inlet flow angle, the isentropic outlet Mach number, and the outlet Reynolds number based on profile chord. Following parameters are used as crucial for the appraisal of CFD calculations:

• isolines of the Mach number and/or density in the flow field of the blade cascade;

• pressure and Mach number distribution on the profile surface;

• energy losses;

• exit flow angle.

For the appropriate simulation of the two-dimensional transonic flow through the blade cascade, the following important phenomena should be adequately modelled:

• stagnation point flow;

• shock-wave/boundary-layer interaction with possible flow separation;

• laminar/turbulent transition;

• boundary layers under pressure gradient.

The shock-wave/boundary-layer interaction seems to be the most important phenomenon and its adequate capture in numerical simulations is crucial for the description of the flow field and for the determination of energy losses. Besides the Underlying Flow Regime UFR2-06 “Flow around blades — transonic”, further Underlying Flow Regimes are important, especially “Shock/boundary-layer interaction” (UFR3-05), “Flow around blades — subsonic” (UFR2-04), “Laminar-turbulent boundary-layer transition” (UFR3-04), “2D boundary layers with pressure gradients” (UFR3-03), and “Stagnation point flow” (UFR3-12) for the steam turbine blade cascade.

2. Application Uncertainities

The analysis of flow structure in the blade cascade is based on the interferometric measurements only. Therefore, the position of the laminar/turbulent transition in not well defined, even though the transition on the suction side is most likely caused by the interaction with the shock wave. For the transonic regime, the shock-wave/boundary-layer interaction is dominant for the adequate capture of the flow field in the blade cascade. The effect of the laminar/turbulent transition is more significant in the subsonic regime (see UFR2-04).

Any data about turbulence characteristics are not known, especially turbulence level for the prescription of inlet boundary conditions for CFD calculation. This fact can influence the prediction of the development of shear layers and the resulting value of energy losses. Generally, the application of advanced turbulence models, as e.g. RSM models, should be avoided in case of absence of turbulence characteristics.

The transonic regime is very sensitive to small changes in blade geometry. The adequate attention should be given to the appropriate description of the blade surface in CFD modelling.

Computational Domain and Boundary Conditions

Computational domain is given by one and/or two blade pitch with profile located inside of the domain. Periodic boundary conditions on the upper-lower boundary have to be prescribed.

Inlet boundary conditions are prescribed by total values of flow parameters (three quantities are given and one is extrapolated) in the distance 1.5 chord upstream of the leading edge. Mean flow rate cannot be given as inlet boundary condition. Static pressure in the integral form is given at the outlet boundary in the distance 1.5-2 chords behind the cascade.

Inlet turbulence should be characterised according to used turbulence model. For two-equation models, the turbulence level and the length scale should be imposed from experimental data. In case such data are not at disposal, some typical values can be chosen (e.g. Tu ≈ 2 – 4%). The accuracy of the prediction is then rather limited.

Ensure that the code includes appropriate non-reflecting discretisation of the boundary conditions for the supersonic waves on the downstream boundary. End-wall influence of the cascade needs to be taken into account as well.

Discretisation and Grid Resolution

Discretisation scheme

Use a higher order scheme (second or higher) with small numerical dissipation as possible.

Use appropriate damping in the regions of high gradients in the shocks and near the leading and trailing edge.

Explicit schemes (TVD Mac Cormack, multistage Runge-Kutta, Roe, Ni) as well as some implicit schemes (especially upwind) give relatively good results for 2D viscous turbulent flows.

Grid and grid resolution

The grid topology should capture adequately high gradients in the flow field. The quadrilateral grids should be preferably used, even though acceptable results can be obtained with unstructured triangular grids as well. The orthogonal grid near the blade surface (e.g. O-H grid) gives best results for the all flow models. For the computational domain considering one blade pitch, a grid with (3-4) x 10⁴ cells has to be used for the appropriate prediction of turbulent flow.

The adaptive grid is to be preferred. The grid refinement is needed in regions with high gradients, i.e. near the leading and trailing edge, in the vicinity of shock waves generally, and near walls when a low-Reynolds-number turbulence model is used.

The grid has to be refined near the leading edge where approx. from 20 to 30 points around the leading edge radius should be applied. In shock wave regions, a grid resolution giving 1-3 grid points across the shock has to be used. A lower grid density can be used outside of the regions with shocks. Grid resolution close to the solid surfaces needs to be consistent with very thin shear layers on blades for accelerated flow.

Be aware that the inclusion of more grid points close to the blunt trailing edge will cause the unsteady vortex shedding from the trailing edge to be captured and cause convergence difficulties with a steady simulation.

Physical Modelling

Turbulence and transition modelling

The proper modelling of flow through the blade cascade is be conditioned by the application of adequate turbulence and transition models. Various turbulence models were used for numerical simulations:

• algebraic model (modified Baldwin-Lomax model);

• one-equation model (Spalart-Allmaras model);

• two-equation model (RNG k-eps model, Menter SST model with Kato-Launder correction)

Best results were obtained by the Spalart-Allmaras model and by the SST model. The Kato-Launder correction is suitable for flow in the vicinity of the leading edge, but the standard expression of the production term in the turbulent energy equation is preferable elsewhere (see UFR3-12).

The bypass transition generally occurs in turbomachinery internal flows. The transition models are mainly based on correlations of the momentum thickness Reynolds number for the transition onset with turbulence level and pressure gradient parameter. This non-local approach requires the computation of the boundary-layer thickness, which is rather complicated for unstructured grids.

The transition is induced by the shock-wave/boundary-layer interaction in the studied transonic regime and the application of empirical correlations is questionable. Therefore all simulations were carried out for turbulent flow only. The effect of the laminar/turbulent transition is important rather in the subsonic case.

Due to the strong flow acceleration in the blade cascade and thin shear layers, the capturing of the flow field and the prediction of pressure distribution with viscous codes is not so much sensitive to the turbulence model used. Flow structure in the boundary layers and in the wake is sensitive to the turbulence model and the position of transition, although in the highly accelerated flow the overall sensitivity of the flow-field to the turbulence model is low.

But for appropriate capturing of important phenomena of the transonic flow through the blade cascade, the prediction of the shock wave pattern and their interaction with boundary layers is crucial. The application of the numerical scheme of the higher order, adaptive grid near the shock region, and appropriate boundary conditions is necessary to capture the shock/boundary layer interaction adequately.

The appropriate prediction of the energy losses requires a high-order numerical scheme with low numerical viscosity and adapted grid in the shock-wave region and near the leading edge and the trailing edge. The main source of energy losses in the transonic regime is the existence of shock waves. The turbulence models used in the in-house codes give the loss coefficient approximately 20% lower than experimental data for both flow regimes.

Near wall model

Wall functions have to be excluded for advanced CFD simulations of turbomachinery flows, especially for flows with transition and separation. The low-Reynolds modification of the turbulence model should be preferred.

A coordinate y+ of the first grid point above the surface should be less than 5. The lower limit of grid points inside the boundary layer is about 10 for the accurate simulation.

Recommendations for Future Work

Future work will be focused on the application of more refined turbulence and transition models. The effects of other parameters, as e.g. wall curvature, rotation, wall roughness, should be taken into account. Non-linear two-equation models and RSM models should be preferred. Besides the advanced turbulence models for the RANS equations, models based on DES (Detached Eddy Simulations) approach should be used especially for capturing of unsteady effects.

The model of bypass transition should be implemented in computation codes used for simulation of internal flows. The transition model should be based on local variables, either using an empirical correlation or a transport equation.

The progress in physical model of flow should be accompanied by the corresponding progress in the numerical methods. The higher order schemes with small numerical dissipation and adaptive grids should be preferably used. Schemes and grids have to be able to consider effects of flow curvature, especially near the blunt leading edge because inaccuracy of the numerical solution near the leading edge is spreading along the blade surface.

For solution of complex flows, the numerical method should be tested together with the applied turbulence model. There is still permanent need of high-quality test cases for verification of CFD models in complex boundary conditions.

© copyright ERCOFTAC 2004

---

Contributors: Jaromir Prihoda; Karel Kozel - Czech Academy of Sciences

Front Page

Description

Test Data

CFD Simulations

Evaluation

Best Practice Advice