CFD Simulations AC6-15

Front Page

Description

Test Data

CFD Simulations

Evaluation

Best Practice Advice

CFD Simulations

Solution Strategy

The computations reported here were performed with the ANSYS-FLUENT (Manual ANSYS Fluent v.17.1) code using the two built-in popular linear eddy-viscosity models (k-ω-SST and realizable k-ε), the Re-stress LRR model (Launder, Reece, & Rodi, 1975) with the linear pressure strain and wall-echo terms, and a DES (based on Menter's k-ω SST model). In parallel, for reference, LES with the WALE subgrid-scale viscosity model (Nicoud & Ducros, 1999) was carried out on finer grids.

The high-Re-number realizable k-ε model and the basic RSM were solved using the standard wall functions. A test with the enhanced wall treatment and the non-equilibrium wall function available in the FLUENT code produced no significant differences in the results. For the k-ω SST model we used the enhanced-wall-treatment ω-equation model (EWT-ω) (ANSYS Fluent v.17.1 Theory Guide).

The computations were performed using the finite-volume method on structured grids. The coupling of the velocity and pressure fields for incompressible flow was ensured using the SIMPLE-C procedure. For the URANS models the convective terms in all equations were discretized by a second-order upwind scheme, whereas the second-order central difference scheme was used for LES and DES (in the LES region). The time derivatives were approximated by an implicit second-order scheme. The time step was set by imposing a CFL<2 constraint. The average CFL number for the 6M grid was 0.35 and for 19.3M grid 0.42. In the bulk of the draft tube the CFL number was almost everywhere less than 1.0 with a maximum of about 1.6 localised in very small areas close to the inlet. Some peaks exceeding the value of 2.0 appeared close to the guide-vane and runner blades, especially their tips, locally reaching values up to 3.0 and even 5.0 for the two respective grids, but caused no numerical instabilities. The statistics were gathered for each run during about 20 sec of real time.

Computational Domain and Boundary Conditions

The computational domain included all the elements constituting the turbine system (guide vane, runner and draft tube) except for the intake channel (Fig.3). Since the intake channel was not considered in the calculations, the boundary conditions were set at the inlet to the turbine guide vanes by imposing a fixed flowrate measured in the experiment.

Figure 3: Computational domain. Left: outside view of different rig components; right: domain interior displaying the “turbine” model

As the LES and DES require initial time-dependent forcing mimicking turbulence, random velocity fluctuations were imposed at the inlet, generated by the method proposed in Smirnov, Shi, and Celik (2001). The inflow profiles of the mean velocity and turbulence properties at the inlet to the turbine guide vanes were generated by a precursor steady RANS computation (with the k-ε realisable model), of the whole experimental set-up. For the latter, the inflow conditions were evaluated by specifying a uniform velocity, turbulence intensity ${k^{1/2}/U}$of 3%, and the equivalent diameter of the annular passage of 0.2 m, from which the inflow turbulent energy dissipation rate ${\varepsilon }$ was evaluated. It is noted that the focus of the present work is on the draft tube for which the entry conditions are generated by the unsteady solutions of flow through the turbine, so that the inflow conditions into the guide vanes are not very influential (Aakti, Amstutz, Casartelli, Romanelli, & Mangani, 2015). The design of the draft tube has two outlets, which is a typical situation for the hydroelectric units operated at the HPP. In the numerical simulation, the conditions of a fixed pressure were set at the outlets.

A specific issue in the computer simulation of hydraulic turbines is the treatment of the rotating runner and the rotor-stator interaction. Several approaches can be found in the literature, i.e. dynamic sliding and moving grid methods and those based on a moving reference frame. The latter is the most common and the simplest way to model the runner rotation and has been used in most of the references cited above, (Zadravec, Basic, & Hribersek, 2007), (Aakti et al., 2015), (Lenarcis et al., 2015). It assumes that the runner is fixed and the equations are solved in a rotating reference frame. This formulation is often referred to as the "frozen rotor" approach. In this paper, the modelling of the runner rotation was performed in the rotated reference frame for the runner zone. The obtained results are then rotated with the runner rotation speed and as such imposed as the inflow field at the inlet into the draft tube. The earlier test calculations proved that this approach is credible for describing the integral flow characteristics including the dominant flow pulsations (Minakov, Platonov, Dekterev, Sentyabov, & Zakharov, 2015a, 2015b, 2015c). A comparison with the computationally more demanding method using sliding meshes showed that for this type of flows with a focus on draft tube dynamics the results are almost the same.

---

Contributed by: A. Minakov [1,2], D. Platonov [1,2], I. Litvinov [2], S. Shtork [2], K. Hanjalić [3] — 

[1] Institute of Thermophysics SB RAS, Novosibirsk, Russia,

[2] Siberian Federal University, Krasnoyarsk, Russia,

[3] Delft University of Technology, Chem. Eng. Dept., Holland.

Front Page

Description

Test Data

CFD Simulations

Evaluation

Best Practice Advice