The flow field inside a cooling channel for the trailing edge of gas turbine blades has been numerically investigated with the aim to highlight the effects of channel rotation and orientation. A commercial 3D RANS solver including a SST turbulence model has been used to compute the isothermal steady air flow inside both static and rotating passages. Simulations were performed at a Reynolds number equal to 20000, a rotation number (Ro) of 0, 0.23, and 0.46, and channel orientations of

It is a matter of fact that the adoption of proper cooling techniques is a key factor in the development of high performance and reliable gas turbine engines, since the hot gas temperature can be far above the melting point of the material used to manufacture the engine components. Focusing the attention on the internal cooling of gas turbine blades, the experimental research conducted on laboratory scaled models has played a great role in the engines development, while more recently, the availability of powerful computational tools has allowed a deeper insight into the performance of cooling channels characterized by various cross-section shapes (squared, rectangular, and triangular) and layouts (single pass, double pass).

In this regard, significant examples concerning the simulation of cooling channels for nozzle blades, in static conditions, are represented by the works of Ooi et al. [

However, the recent adoption of blade profiles with a reduced thickness in the trailing edge (TE) region made the thermal protection of the TE of high pressure turbine blades one of the most challenging issues to deal with [

Furthermore, if rotor blade cooling channels are considered, the effects of Coriolis and centrifugal forces on the fluid flow must be taken into account as well. The main contributions that analyse the fundamental configuration of a radial channel of rectangular cross-section in orthogonal rotation (i.e., with the rotation axis parallel to the channel height) with outward flow are the ones of Hart [

Focusing the attention to flows in rotating cooling channels, a number of significant contributions can be found in the open literature. Reynolds averaged Navier stokes (RANS) solutions for the flow and thermal field in a rotating serpentine passage can be found in Iacovides et al. [

Conversely, if trailing edge specific applications are considered, only a limited number of experimental or numerical contributions are available, and moreover, the majority of the works concerns ducts for nozzle blades. Taslim et al. provided two experimental and numerical contributions [

For what concerns the geometries provided with cut-back, Choi et al. [

In the case of rotor blades channels, the only studies on cooling schemes with axial outflow, which resemble modern TE cavities, to the authors’ best knowledge, are the experimental thermal analyses of Chang et al. [

The literature review allows to conclude that only a limited number of papers dealing with flow field analysis in rotating ducts relevant to turbo-machinery applications are available, especially if looking at TE solutions. Therefore, since the knowledge gained on basic geometries cannot be applied straightforward to TE cooling geometries, an effort aimed at deepening the knowledge on these devices is required.

Concerning the present cooling channel geometry, the flow field has been described by means of detailed PIV and stereo-PIV measurements in static and orthogonally rotating conditions by Armellini et al. [

The present work is aimed at investigating the TE channel flow at varying the rotation number and channel orientation. The previous experimental investigations concerning a static channel and a single orthogonally rotating condition

The investigated channel geometry has the key features of a cooling channel suitable for TE blade cooling. It has a cross-section of high aspect ratio (at the channel inlet AR = 7.25), a radial inlet, and a redirecting wall at the channel leading side that deviates the flow towards the wedge shaped outlet section at the trailing edge. Inside the TE region, seven elongated pedestals are inserted. The coolant is discharged also at the channel tip through a perforated wall. All the geometrical details and dimensions of the test section are widely commented in [

Schematic (a–d) and 3-D view (e, f) of the test section investigated in the present work, further details in [

The experimental data used in the following for the validation of the present numerical simulations are already available in the literature [

Steady-state RANS numerical simulations have been performed using commercial software Ansys CFX v11.0. The convective terms were discretized by using the high resolution scheme which is a bounded second-order upwind scheme, while flow turbulence was modelled by means of the

Experimental data are not available for the channel orientations and rotation numbers other than the ones investigated in [

Overview and details of the mesh used in the present work.

Such a considerable number of cells results mainly from the need of using very fine elements in the regions close to the pedestal surfaces, where three-dimensional flow separation takes place. In these regions, o-grids methodology has been used in order to obtain high cell orthogonality.

All runs have been performed by assuming an isothermal air flow. The boundary conditions were applied according to a classical scheme for incompressible or low Mach number flow simulations. A uniform velocity distribution is imposed in the inlet section, while the ambient pressure (101325 Pa) is forced at the outlet.

For the assessment of numerical stability and convergence of the solution, local values of velocity components and pressure were continuously monitored during the simulations. For all the presented cases, no stability problems (i.e., significant fluctuations on the monitor quantities) were encountered and convergence was generally reached after about

In order to obtain an estimate of the discretization error of the computed results, a grid independence study was performed following the well-established method suggested by the Fluid Engineering Division of ASME [

In the present case, the GCI method was applied to a set of three similar grids characterized by different spatial resolution defined by a refinement factor of 1.3, according to [

Resulting GCI error band from the mesh sensitivity analysis for the profiles of the velocity magnitude in plane

Figures

In the experiments that provide the validation data for the present simulations [

The filter was modelled as an isotropic porous region by introducing an additional source term in the momentum equation [

Figure

Experimental [

The numerical results compare satisfactory the experimental ones, despite the limited channel length available for the flow development downstream of the honey-comb filter placed at the channel inlet (

The general good agreement of the numerical results with the experiments can be appreciated in the comparison of Figure

Comparison of time-averaged velocity field and stream tracers in plane

A more quantitative comparison between experimental and numerical data is made considering the flow approaching the pedestals. Figure

Experimental [

Nevertheless, the general flow structure is well captured in all cases and the complex three-dimensional interpedestal flow topology is correctly simulated for both

Flow field inside the interpedestal passage P4 at

Comparison of experimental [

At this stage of the analysis, it is important to note that for

In this section, the rotational effects are analysed on the basis of the numerical results obtained for channel configurations

Profiles of velocity component

This is evidenced in Figure

Contours of

The overall flow behaviour inside the channel can be commented by referring to the velocity maps and stream tracers in planes

Contours of the in plane velocity modulus

To support this explanation, distributions of velocity vectors along the

Velocity vector distributions at

In spite of these local effects on the flow direction, the overall effect of the channel rotation is to flatten the velocity distribution and to reduce the boundary layer thickness on the lower and upper walls. Consequently, the flow approaching the pedestal, after being deviated by the obstacle, does not produce any longer horseshoe vortices, as already commented in the previous section for

In this section, the numerical results obtained for different channel orientations, namely,

Figure

Contours of

Figure

Consistent with the rotational effects on the inlet flow commented above, the velocity distribution inside the main channel is not symmetric along the channel height, as shown by the velocity maps and stream tracers in Figure

Contours of the in plane velocity modulus

A more quantitative comparison is performed in the plots of Figure

Profiles of the velocity modulus

A proof of this effect is the reappearance of the horseshoe vortices on the upstream face of the first pedestals for

Flow field inside the interpedestal passages P2 (a), P4 (b), and P6 (c) at

P2

P4

P6

Finally, the mass flow through the different channel exits is not significantly affected by the variation of the channel orientation. Indeed, this depends on the fact that the pressure distribution inside the channel is only slightly affected by the different flow distributions caused by a change in the channel orientation.

In the present work, the combined effects of rotation and channel orientation on the flow field inside a modern cooling passage for the blade trailing edge were carried out through a numerical investigation performed by the SST turbulence model developed on Ansys CFX 11. The selected geometry was previously investigated by the authors in static

Coriolis-induced vortical structures arise inside the inlet portion of the channel. These vortices are weak for

At

As Ro increases, the separation bubble found at the channel tip increases progressively.

When the channel orientation is different from

Coriolis-induced vortical structures inside the inlet duct are no longer symmetric with respect to the y axis of the channel, and the higher velocities are found close to the channel bottom wall. Moreover, the rotational effects are lessened on the trailing side, with direct influence on the flow discharged close to the hub. In particular, for

The interaction between the asymmetric Coriolis vortices causes a flow separation all along the corner between the channel bottom and leading walls. This causes the separation bubble at the tip to have different extensions along the channel height, the larger size being found at the lowest elevations.

=

Channel width (m)

Hydraulic diameter (m)

Channel height

Turbulence intensity

Root mean square value

Mean velocity components along

r.m.s. velocity fluctuations along

Bulk velocity (m/s)

Setting chamber coordinate system (mm)

Radial, axial, and cross wise coordinates (channel reference frame) (mm)

Incidence angle (deg)

Turbulent dissipation (—)

Channel orientation (deg)

Turbulent kinetic energy (—)

Kinematic viscosity (

Density

Angular velocity (rad/s).

The present work has been supported by the Italian Ministry of University and Research (MiUR).