Description of the Test Case: Separated flow in a three-dimensional diffuser
Name of Authors: Florian Menter
Company:ANSYS Germany GmbH
Staudenfeldweg12, 83624 Otterfing, Deutschland
Telephone: +49 (0) 8024 9054 15Fax: +49 (0)8024 9054 17
Email:
July 2009
Test case description
Experiments were performed to determine the mean velocity field in two three-dimensional diffusers with the same fully-developed channel inlet but slightly different expansion geometries. Magnetic Resonance Velocimetry was used to collect velocity data. Both diffuser flows exhibited three-dimensional boundary layer separation but the size and shape of the separation bubble exhibited a high degree of geometric sensitivity dependent on the dimensions of the diffuser.
Geometry of the diffusers
A schematic of the recirculating flow loop used in the experiments of Cherry et al, 2006 is shown in Figure 1. The test diffuser is attached directly to the development channel exit. Figure 2 shows detailed diagrams of the two diffusers and Table 1 summarizes their dimensions. Diffuser 1 has a rectangular inlet of height 1 cm and aspect ratio 1:3.33 and a 4 cm square outlet, giving an area expansion ratio of 4.8. The diffuser is 15 cm long. One side wall expands at an angle of 2.56 degrees, and the top wall expands at an angle of 11.3 degrees. The other two walls are straight. Diffuser 2 is also 15 cm long and has the same inlet as Diffuser 1, but its outlet is 4.51cm×3.37cm, giving an area expansion ratio of 4.56. The top wall of Diffuser 2 expands at an angle of 9 degrees and its side wall expands at an angle of 4 degrees.For both diffusers, the origin of coordinates coincides with the intersection of the two non-expanding walls at the beginning of the diffuser’s expansion.
Figure 1. Flow system schematic.
Figure 2. Geometrical details of the two diffuser configurations.
Table 1. Geometric features of Diffusers 1 and 2.
Experimental flow parameters
The working fluid for all of the experiments was water.Acentrifugal pump circulated water at a flow rate of 20.3 L/min. The Reynolds number of bothdiffusers based on the height of the inlet channel (1 cm) and bulk inlet velocity (1 m/s) was set to approximately 10,000. At the inlet sections of both diffusers, the flow is assumed to be fully developed.
Available experimental data
Velocity and coordinate data are available online at The data are seven 3D Matlab matrices. The x, y, and z matrices give the coordinates of each point in the coordinate system shown in Fig. 2. The units are meters. The vx, vy, and vz matrices give the corresponding velocity components for each point in m/sec. The matrix mg gives the relative signal magnitude detected by the MRI machine. At the ATAAC web page, simple Matlab scripts are available to export the data from Matlab matrices into text data files supported by Tecplot, as well as ready Tecplot files.
Experimental data for the pressure coefficient in Diffuser 1 are available here. The coordinate system is the same as the coordinate system described in the corresponding manuscript (see References). The Cpcoefficient is defined as (P-Pref)/(0.5*ρ*V2), where Pref is the pressure at x=0 at the midpoint of the bottom flat wall (opposite the wall expanding at 11.3 degrees), ρ is the density, and V is the bulk inlet velocity. The data were taken in a line along the bottom wall of Diffuser 1 at constant y and z coordinates. L indicates the length of the diffuser.
Recommended grid
The computational grids for both diffusers can be generated using a special utility written in Fortran. The source code and examples of input text file with mesh parameters are available at the ATAAC web page. Meaningof the names of parameters used in the input file is the following:
Plot3D output file with diffuser grid name of the output file containing the grid for the diffuser in Plot3D format.
Plot3D output file with inlet grid name of the output file containing the grid of the inlet section in Plot3D format; the grid has two nodes in streamwise direction.
Lx_inlet, Lx_diffuser, Lx_outlet length in x-direction of the inlet, diffuser and outlet sections, respectively (see also Figure 3).
Inlet: dx_start, dx_end, dx_SF the first two parameters are the grid steps in x-direction at the beginning and at the end of the inlet section, respectively, and dx_SF is the stretching factor (ratio of two adjacent grid steps).
Diffuser: dx_diffuser, dx_SF_inlet, dx_SF_outletgrid step in x-direction in the middle of the diffuser, stretching factor to the inlet section, stretching factor to the outlet section.
Outlet: dx_start, dx_end, dx_SF the first two parameters are the grid steps in x-direction at the beginning and at the end of the outlet section, respectively, and dx_SF is the stretching factor.
Ly_inlet, Ly_outlet, R_curvature length in y-direction of the inlet, diffuser and outlet sections, respectively (see also Figure 3).
Inlet: dy_wall, dy_max, dy_SF the first two parameters are the grid steps in y-direction near the wall and in the middle of the inlet section, respectively, and dy_SF is the stretching factor. Grid step sizes in the diffuser and outlet sections increase proportionally to domain extension.
Lz_inlet, Lz_outlet, R_curvature length in z-direction of the inlet, diffuser and outlet sections, respectively.
Inlet: dz_wall, dz_max, dz_SF the first two parameters are the grid steps in z-direction near the wall and in the middle of the inlet section, respectively, and dz_SF is the stretching factor. Grid step sizes in the diffuser and outlet sections increase proportionally to domain extension.
Figure 3. Definition of some parameters used by the utility for mesh generation.
Number of nodes in all directions is computed automatically by the code.For each diffuser, a sequence of three meshes (Mesh-1, Mesh-2 and Mesh-3) was generated at ANSYS. Input text files for the utility and also ready mesh files are available at the ATAAC web page. The medium meshes (Mesh-2, ~1,500,000 nodes) provided grid-independent solutions for RANS simulations done with ANSYS CFX and FLUENT solvers using the SST turbulence model. The y+ values for all meshes are lower than unity. Meshesare stored in Plot3D format and can be imported into Gambit or ICEM CFD tools for surface patch definition and export to any desired format. Also, the mesh generation utility outputs the mesh for the inlet section. This mesh is actually a part of the whole diffuser mesh which contains only two grid planes in the streamwise direction.
Emphazise of main points
Along with the turbulence anisotropy typical of rectangular channel flows, the flow involves an adverse pressure gradient causing separation. This separation has proven very sensitive to details of turbulence modeling (ERCOFTAC, 2008). It seems clear that the anisotropy of the normal stresses has to beaccounted for in order to avoid the formation of an incorrect flow topology. The computation of the diffuser shows that the inclusion of the stress anisotropy leads to a drastic improvement of the results for this case. The flow topology matches much better the experimentally observed flow and the wall pressure distribution improves significantly.
References
Cherry, E. M., Iaccarino, G., Elkins C. J., and Eaton,J. K. (2006): "Separated flow in a three-dimensional diffuser: preliminary validation", Center for Turbulence Research, Stanford University, Annual Research Brief 2006, pp. 31-40. This reference is available online at
Cherry, E.M., Elkins, C.J. and Eaton, J.K. (2007): "Geometric Sensitivity of 3-D Separated Flows", Proc. of 5th International Symposium on Turbulence and Shear Flow Phenomena - TSFP5, Munich, August 27-29.
ERCOFTAC/IAHR (2008) 13th workshop on refined turbulence modelling, Sept. 2008. (
Guidelines for results submission
Pressure coefficient Cp
Pressure coefficient must be plotted at y=0 (along the lower, flat wall) and z/B=1/2 (central plane)in accordance with the experimental data.
Streamwise velocity contours
Streamwise velocity contour plots in 2-D cuts at five streamwise locations (2cm, 5cm, 8cm, 12cm and 15cm) in accordance with Figure 4 in the work of Cherry et al. (2008, IJHFF, Vol. 29(3)) should be provided.Examples of the plot at one location for different turbulence models (SST and ANSYS EARSM) are shown below in comparison with the experimental data.
The purpose of these plots is to get a qualitative picture of the flow fields.
Turbulence quantity contours
Similar as for the streamwise velocities, the contour plots of the urms/Ubulk x 100 in 2-D cuts at five streamwise locations (2cm, 5cm, 8cm, 12cm and 15cm) in accordance with Figure 9in the work of Cherry et al. (2008, IJHFF, Vol. 29(3)) should be provided.Those using eddy-viscosity models should compute it from the corresponding stress-strain relationship. An example of the plot is shown below in comparison with the experimental data.
The purpose of submitting these plots is to get a qualitative picture of the turbulence fields.