In order to validate the method for a single row of turbine blades, a CFD simulation of 3-D steady flow in a linear turbine cascade, which is the Durham Test Case (ERCOFTAC F1), is first conducted. This is a large scale, low speed cascade of turbine rotor blades with about 110 of turning causing strong secondary flows. The code used was the FLUENT 5 code. An unstructured hexahedral mesh with a mesh size of 311814 cells was created for a blade passage with periodic boundary. Different turbulence models were tested in the calculation including Reynolds Stress Model.

The static pressure distribution around the blade was compared for various spanwise distances from the end wall. The static pressure coefficient distribution predicted by the CFD was within the 0.5% of the experimental data from the near end wall region to the mid-span, apart from close to the leading edge. With respect to the secondary flow prediction, the RSM turbulence model gave the best results. The total pressure loss contours at a plane 28% of the axial chord downstream of the trailing edge, showed that the CFD gave nearly the same loss distribution as the experimental results, but with a higher value generally. As a result, the pitch averaged total pressure loss from the CFD gave higher loss at the mid-span but generally the same shape as the experimental results. The higher mid-span loss means a higher profile loss is predicted. The profile loss is generated in the blade surface boundary layers and the mixing process after the trailing edge. In the experiment, the boundary layer on the blade surface was found to be transitional but the CFD assumed a fully turbulent blade surface boundary layer. This is probably the reason why the CFD gives higher loss at the mid-span. The flow angles from the CFD were also compared with the experimental results with generally good agreement. Overall the results confirmed the validity of the CFD method.

For unsteady blade interaction calculation, a one and a half stage turbine test case from Aachen (ERCOFTAC U1) was simulated. This is a subsonic ( ) stator – rotor – stator combination, with the first and second stators being identical. The low aspect ratio results in strong secondary flows. A mesh with three different fluid regions was created for stator1, rotor and stator2. The mesh was a combination of prismatic cells and hexahedral cells with total of 1.7 million cells. The blade interaction effect was simulated by employing the sliding mesh model so that between the fluid regions, two grid interfaces were established. Due to the large mesh size, the case was run on four CPU's in parallel. After periodic convergence had been achieved, the results were sampled at different time steps.

The mass flow rate from the computation was 8.16 kg/s compared to the test data of 8.00 kg/s. This difference is thought be due to the fact that the tip gap was not included in the simulation and so the efficiency was a little higher than expected. With upstream and downstream pressure boundaries taken from the experiment, a higher mass flow would result. The instantaneous entropy at the mid-span was studied which showed the wake interaction with the blade rows. However the wakes were seen to be diffusing too quickly, indicating that even this large grid is not fine enough. The time averaged circumferential averaged yaw angle and Mach number from the CFD and the experiments were compared at three test planes, downstream from the trailing edge of the first stator row, downstream from the trailing edge of the rotor row, and downstream from the trailing edge of the second stator row. Generally the agreements for Mach number and yaw angle were good for the first two planes, although the yaw angle after the rotor did not capture the secondary flows very well, partly due to not modeling the tip clearance. Downstream of the second stator, the agreement was not so good. The unsteady computational secondary flow vectors were compared with those measured downstream of the rotor for different time steps. Although the comparison showed some qualitative agreement, the secondary flow predicted by the CFD was smaller than the experiments. This is probably because the gird was not fine enough or because of the turbulence model used (Spalart-Allmaras model).

The CFD code FLUENT 5 has been validated against the steady case, which is the Durham test case. The results show that the CFD code is capable of accurately capturing the complicated 3-D effect in this turbine cascade. The sliding meshes model was used to simulate the ERCOFTAC U1 test case. Overall agreement between numerical and experimental results for time- dependent quantities is promising. All these calculations used unstructured meshes as computational grid. The advantage of the unstructured mesh is that it can be done automatically. This could save design engineers a lot of time on mesh generation, and so speed up the design process.

purchase the full-text of this paper (price £20)

go to the previous paper
go to the next paper
return to the table of contents
return to the book description
purchase this book (price £85 +P&P)