CFD Simulations AC614
Contents
Swirling flow in a conical diffuser generated with rotorstator interaction
Application Challenge AC614 © copyright ERCOFTAC 2020
Overview of CFD Simulations
A series of numerical simulations was undertaken to study a highly swirling turbulent flow generated by rotorstator interaction in a swirl generator [2]. The purpose was to assess the applicability of different turbulence models in a swirling flow with a high level of unsteadiness and a significant production and dissipation of turbulence in the flow away from the wall. Nine turbulence models are compared: four highReynolds number models URANS, two lowReynolds number models URANS and three hybrid URANSLES models. These are the standard , SST , realizable , RNG , LaunderSharma , LienCubic , delayed DES SpalartAllmaras [11], DDES SST [13] and improved DDESSA [14] models. The URANS models are capable of capturing the main unsteady feature of this flow, the socalled helical vortex rope, which is formed by the strong centrifugal force and an onaxis recirculation region. However, the size of the onaxis recirculation region is overestimated by the URANS models. Although the lowReynolds number URANS formulations resolve the boundary layers in the runner and the draft tube more accurately, they still encounter difficulties in predicting the main flow features in the adverse pressure gradient region in the draft tube. It is shown that a more detailed resolution, which is provided by the hybrid URANSLES methods, is necessary to capture the turbulence and the coherent structures.
SIMULATION CASE CFD
Solution Strategy
The calculations reported herein are made using the finitevolume method in the OpenFOAM1.6ext CFD code. The secondorder central differencing scheme is used to discretize the diffusion terms. The linearupwind differencing is used in URANS simulations to approximate the convection term. The blended numerical scheme is used in the hybrid method. The scheme is a combination of linearupwind differencing in the URANS region and a limited linear total variation diminishing (TVD) scheme with a conformance coefficient in the LES region. The convection term in the LES region is interpolated by 15% linearupwind differencing and 85% central differencing. The larger the part of the central differencing in the LES region is, the smaller the timestep required. Furthermore, the secondorder van Leer TVD scheme is used to approximate the convection term in the hybrid method. The numerical schemes have only small effects on the timeaveraged values. Time marching is performed with an implicit secondorder accurate backward differentiating scheme.
Computational Domain
Figure 5 shows the complete computational domain. The domain is meshed in four regions in ICEM CFD using a structured multiblock approach with O–grids around the blades and in the draft tube. The strut region is included in the highReynolds number model simulations, but omitted in the lowReynolds number model and hybrid URANSLES simulations. Those simulations employ the interpolated data from the URANS simulation as inlet condition before the guide vanes.
Figure 5: Computational domain and GGI applied between the four regions used by the highReynolds number models. 
Three mesh resolutions are created, one for highReynolds number URANS, one for
lowReynolds number URANS, and one for hybrid URANSLES model.
Figure 6 shows the mesh for the hybrid URANSLES simulations.
Figure6: Coarse mesh used by the hybrid URANSLES models. 
The General Grid Interface (GGI) is used at the interfaces between the rotating and
stationary regions, and to simplify the mesh generation of the strut region.
The General Grid Interface (GGI) connections refer to the class of grid connections
where the grid on either side of the two connected surfaces does not match.
In general, GGI connections permit nonmatching of node location, element type,
surface extent, surface shape and even nonmatching of the flow physics across the
connection.
Table 1
shows the details of the mesh resolution studies of the highReynolds
number models and lowReynolds number models.
Mesh  Strut  Guide vane  Runner  Draft tube  Total 

HighReynolds Coarse  3 × 10^{5}  7 × 10^{5}  7.6 × 10^{5}  1 × 10^{6}  2.76 × 10^{6} 
HighReynolds Fine  3 × 10^{5}  8 × 10^{5}  1.1 × 10^{6}  2.85 × 10^{6}  5.05 × 10^{6} 
LowReynolds Coarse  —  9.3 × 10^{5}  1.13 × 10^{6}  1.35 × 10^{6}  3.41 × 10^{6} 
LowReynolds Fine  —  9.3 × 10^{5}  1.13 × 10^{6}  2.66 × 10^{6}  4.72 × 10^{6} 
The refinement is mainly done in the draft tube, which is the main area of interest in the
present study.
Figure \ref{meshInd} shows that the axial and tangential velocity profiles at W1
(see Fig. 1)
are mesh independent for both the highReynolds number and lowReynolds number model simulations.
The survey axes, , at sections W0 – W2, are normalized by the throat radius,
= 0.05m, and the velocity is normalized by the bulk velocity at the throat,
= 3.81m/s.
The survey axes, , begins at zero at the wall where the window is located,
see Fig. 1.
The coarse meshes are used for the rest of the study.
Table 2 shows the details of the mesh resolution studies of the hybrid URANSLES turbulence models.
Mesh  Guide vane  Runner  Draft tube  Total  

Coarse  2.45 × 10^{6}  2.4 × 10^{6}  8.4 × 10^{6}  13.25 × 10^{6}  23.82  39.2 
Fine  2.45 × 10^{6}

3.62 × 10^{6}

13.2 × 10^{6}

19.27 × 10^{6}  18.27  41.23 
The main difference between the coarse and the fine mesh is again in the draft tube. The wallparallel mesh resolution units are defined as
where is instantaneous axial velocity, is the kinematic viscosity and is the tangential position. The wallnormal mesh resolution unit is defined as
where is the wallspacing of the first cell, is the friction velocity and is the wall shear stress. The resulting values are comparable with those used before in simulations of turbulent swirling flow in a circular pipe [1]. Therefore, the wallparallel mesh resolution in the draft tube is sufficient for the DDESSA model. has a maximum value of 8.1 at the blade leading edge where there is a stagnation point. The grid spacings normalized with the throat radius, , in the axial, radial, and tangential directions in the draft tube are in the range of [8 × 10^{4} — 0.02], [8 × 10^{5} — 0.018] and [4 × 10^{3} — 0.028], respectively. The wall spacings normalized with the throat radius, , in the runner are in the range of [2 × 10^{4} — 1.16 × 10^{3}].
Boundary Conditions
For the highReynolds number models, a constant velocity corresponding to the volume flow rate is imposed upstream of the struts. Constant values for , and are applied at the inlet boundary, using a turbulence intensity of 10% and a viscosity ratio of = 10. A series of outlet boundary conditions are studied for the pressure, and the one with the least upstream effects, the homogeneous Neumann condition, is applied at the outlet boundary. The homogeneous Neumann condition is also applied for the turbulence quantities at the outlet boundary. The inletOutlet condition, which is a homogeneous Neumann condition with blockage of a backflow, is applied at the outlet boundary for the velocity. The logarithmic law of the wall is applied at the walls in highReynolds number models simulations.
Application of Physical Models
The lowReynolds number and hybrid models have the inlet applied just upstream of the guide vanes, at the location of the first General Grid Interface (GGI) of the highReynolds number cases, see Fig. \ref{Comp_domain}. The inlet data is extracted from the URANS averaged results at that location, and reconstructed by spline curves where six points are used in the viscous sublayer. The number of data points with a normalized wall distance below 10 characterizing the viscous sublayer is often used as an indicator of the resolution of the turbulent boundary layer. This method is also verified by Gyllenram et al. [8], and Javadi and Nilsson [1, 9] for a highly turbulent swirling flow. To assess the sensitivity of the inlet boundary condition, Fig. \ref{fig7} shows a comparison between the LaunderSharma results using the abovementioned boundary condition and that using constant values corresponding to the volume flow rate. The results show that the constant value and the resolution of the inlet profile has a small effect on the flow features in the draft tube. Since the extracted inlet profile yields a slightly smaller onaxis recirculation region, and closer agreement with the experimental results, that is used in the following. In the case of hybrid models, no wallfunction is used.
Computational Details
The parallel processing is done through MPI and domain decomposition. To achieve a nearoptimal parallel load balancing, the computational meshes are subdivided into blocks of equal size, which are submitted to individual cores of an AMD Opteron 6220 Linux cluster. The finest mesh resolution is run on 12 nodes with 16 cores each over more than 520000 iterations (4 iterations per timestep), where each timestep requires a wallclock time of about 75s. The timestep corresponds to 0.028 degrees of runner rotation.
The LaunderSharma simulation with the fine mesh is advanced in time with
a maximum CourantFriedrichsLewy (CFL) number of 2.5 and a mean CFL number of 0.03.
The effect of the CFL number on the instantaneous and averaged solution of the
highReynolds number models was examined, showing that the CFL number up to 4 has a
negligible effect on the results.
In the simulations using the hybrid methods, the maximum CFL number is 1.3.
The maximum CFL number occurs near the nozzle, where a strong axial flow passes through
a dense mesh region.
The results demonstrate that little is gained by reducing the timestep and switching to
a more refined numerical scheme when a relatively coarse mesh in the runner is used.
Contributed by: A. Javadi^{a}, A. Bosioc^{b}, H Nilsson^{a}, S. Muntean^{c}, R. SusanResiga^{b} — ^{a}Chalmers University of Technology, Göteborg, Sweden; ^{b}University Polytehnica Timişoara, Timişoara, Romania; ^{c}Center for Advanced Research in Engineering Sciences, Romanian Academy, Timişoara Branch, Timişoara, Romania
© copyright ERCOFTAC 2020