# Test Case Study

## Brief Description of the Study Test Case

A detailed description of the chosen test case (TC with L = 3.7D) is available at this link. So here we present only its brief overview.

A schematic of the airflow past the TC configuration is shown in Figure 1. The model is comprised of two cylinders of equal diameter aligned with the streamwise flow direction. The polar angle, ${\displaystyle {\theta }}$, is measured from the upstream stagnation point and is positive in the clockwise direction.

 Figure 1: Schematic of TC configuration [3]

Geometric and regime parameters defining the test case are summarized in Table 1.

Table 1: Flow parameters
Parameter Notation Value
Reynolds number Re=${\displaystyle U_{0}D/\nu }$ 1.66×105
Mach number M 0.128
Separation distance ${\displaystyle L/D}$ 3.7
TC aspect ratio ${\displaystyle L_{z}/D}$ 12.4
Cylinder diameter ${\displaystyle D}$ 0.05715 m
Free stream velocity ${\displaystyle U_{0}}$ 44 m/s
Free stream turbulence intensity ${\displaystyle K}$ 0.1%

The principal measured quantities by which the success or failure of CFD calculations are to be judged are as follows:

• Mean Flow
• Distributions of time-averaged pressure coefficient, ${\displaystyle C_{p}\leq (p-p_{0})\geq (1/2\rho _{0}U_{0}^{2})}$, over the surface of both cylinders;
• Distribution of time-averaged mean streamwise velocity ${\displaystyle {\left.\langle u\rangle /U_{0}\right.}}$ along a line connecting the centres of the cylinders;
• Distributions of the root-mean-square (rms) of the pressure coefficient over the surface of both cylinders;
• Power spectral density of the pressure coefficient (dB/Hz versus Hz) on the upstream cylinder at ${\displaystyle \theta }$ = 135°;
• Power spectral density of the pressure coefficient (dB/Hz versus Hz) on the downstream cylinder at ${\displaystyle \theta }$ = 45°;
• Turbulence kinetic energy
• x – y cut of the field of time-averaged two-dimensional turbulent kinetic energy ${\displaystyle {\text{TKE}}={\frac {1}{2}}\left(\langle u'u'\rangle +\langle \nu '\nu '\rangle \right)/U_{0}^{2}}$;
• 2D TKE distribution along* y = 0;
• 2D TKE distribution along* x = 1.5 D (in the gap between the cylinders);
• 2D TKE distribution along* x = 4.45 D (0.75 D downstream of the centre of the rear cylinder).

All these and some other data are available on the web site of the BANC-I Workshop.

## Test Case Experiments

A detailed description of the experimental facility and measurement techniques is given in the original publications [2-4] and available on the web site of the BANC-I Workshop. So here we present only concise information about these aspects of the test case.

 Figure 2: TC configuration in the BART facility [3]

Experiments have been conducted in the Basic Aerodynamic Research Tunnel (BART) at NASA Langley Research Center (see Figure 2). This is a subsonic, atmospheric wind-tunnel for investigation of the fundamental characteristics of complex flow-fields. The tunnel has a closed test section with a height of 0.711 m, a width of 1.016 m, and a length of 3.048 m. The span size of the cylinders was equal to the entire BART tunnel height, thus resulting in the aspect ratio Lz / D = 12.4. The free stream velocity was set to 44 m/s giving a Reynolds number based on cylinder diameter equal to 1.66 × 105 and Mach number equal to 0.128 (flow temperature T = 292 K).

The free stream turbulence level was less than 0.10%. In the first series of the experiments [2, 3], in order to ensure a turbulent separation from the upstream cylinder at the considered Reynolds number, the boundary layers on this cylinder were tripped between azimuthal locations of 50 and 60 degrees from the leading stagnation point using a transition strip. For the downstream cylinder, it was assumed that trip-like effect of turbulent wake impingement from the upstream cylinder would automatically ensure turbulent separation. However, later on [4] it was found that the effect of tripping of the downstream cylinder at L/D = 3.7 is also rather tangible (resulted in reduced peaks in mean Cp distribution along the rear cylinder, accompanied by an earlier separation from the cylinder surface, a reduced pressure recovery, lower levels of mean TKE in the wake and reduced levels of peak surface pressure fluctuations). For this reason, exactly these (with tripping of both cylinders) experimental data [4] were used for the comparison with fully turbulent CFD.

In the course of experiments, steady and unsteady pressure measurements were carried out along with 2-D Particle Image Velocimetry (PIV) and hot-wire anemometry used for documenting the flow interaction around the two cylinders (mean streamlines and instantaneous vorticity fields, shedding frequencies and spectra).

Information on the data accuracy available in the original publications [2-4] is summarized in Table 2. Most absolute values are given based on nominal tunnel conditions or on an average data value. Percentage values are quoted for parameters where the uncertainty equations were posed in terms of the uncertainty relative to the nominal value of the parameter.

Table 2: Estimated Experimental Uncertainties
Quantity Uncertainty
Drag Coefficient 0.0005
PIV: Umean, Vmean 0.03 (normalized)
PIV: Spanwise velocity 1.8 (normalized)
PIV: TKE 4%
Power Spectral Density (PSD) 10 – 20%
Cp' rms 5 – 11%
Diameter, D; Sensor spacing Δz 0.005 inch

## CFD Methods

The key physical features of the UFR (Section 1) present significant difficulties for all the existing approaches to turbulence representation, whether from the standpoint of solution fidelity (for the conventional (U)RANS models) or in terms of computational expense for full LES (especially if the turbulent boundary layers are to be resolved). For this reason, most of the computational studies of multi-body flows, in general, and the TC configuration, in particular, are currently relying upon hybrid RANS-LES approaches. This is true also with regard to simulations carried out in the course of the BANC-I and II Workshops and in the framework of the ATAAC project, where different hybrid RANS-LES models of the DES type were used (see Table 3) [1].

Table 3: Summary of simulations
Partner Turbulence Modelling approach Compressible/Incompressible Lz Grid Side Walls
Beijing Tsinghua University BTU SST DDES Compressible 3D Mandatory Slip
German Aerospace Center, Göttingen DLR SA DDES Compressible 3D Mandatory Slip
New Technologies and Services, St.-Petersburg, Russia NTS SA DDES

SA IDDES

Incompressible and Compressible 3D, 16D Mandatory Slip
Technische Universität Berlin TUB SA DDES

SA IDDES

Incompressible 3D Mandatory Slip
SST - k–ω Shear Stress Transport model [9]; SA - Spalart-Allmaras model [10]; SA and SST DDES - Delayed DES based on the SA and SST models [11]; SA IDDES - Improved DDES based on the SA model [12].

As mentioned in Section 4, in the experiments the boundary layers on both cylinders were tripped ahead of their separation, thus justifying the "fully turbulent" simulations.

   All the partners used their own flow solvers.

   Particularly, *BTU* employed  in-house  /compressible/  Navier-Stokes  code
with weighted, central-upwind, approximation  of  the  inviscid  fluxes
based on a modification of the  high-order  symmetric  total  variation
diminishing scheme. The method combines 6th order central and 5th order
WENO schemes. For the time integration, an implicit LU-SGS algorithm is
applied with Newton-like sub-iterations.

   *DLR*  used  their  unstructured  TAU   code   with   a   finite   volume
/compressible/  Navier-Stokes  solver.  The  solver  employs  a  standard
central scheme with matrix dissipation with dual time stepping strategy
of Jameson. The 3W Multi-Grid cycle was applied for  the  momentum  and
energy equations, whilst the SA transport equation was  solved  on  the
finest grid only. Time  integration  was  performed  with  the  use  of
explicit 3-level Runge-Kutta scheme. The method is of the 2nd order  in
both space and time.

   *NTS* used in-house NTS finite-volume  code.  It  is  a  structured  code
accepting   multi-block   overset   grids   of   Chimera   type.    The
/incompressible/ branch of the code employs Rogers and Kwak  scheme  [13]
and  for  /compressible/  flows  Roe  scheme  is  applied.  The   spatial
approximation of the inviscid fluxes within these methods is  performed
differently  in  different  grid  blocks  (see  Figure  3  below).   In
particular, in the outer block, the 3rd-order upwind-biased  scheme  is
used,  whereas  in  the  other  blocks,  a  weighted  5th-order upwind-
biased/4th-order central  scheme  with  automatic  (solution-dependent)
blending function [14] is employed. For the time integration,  implicit
2nd-order backward Euler scheme with sub-iterations was applied.

   Finally, *TUB* applied their in-hose multi-block structured code ELAN  in
the framework of  the  /incompressible/  flow  assumption.  The  pressure
velocity coupling is based on the SIMPLE algorithm. For the  convective
terms a hybrid approach [15] with blending  of  2nd-order  central  and
upwind-biased TVD schemes was used. The time integration was similar to
that of NTS.

   The viscous terms of the governing  equations  in  all  the  codes  are
approximated with the 2nd order centered scheme.


1. Some participants of the BANC Workshops have used pure LES rather than DES-like approaches but these computations had the most difficulty simulating the high Reynolds aspects of the flow [5].

Contributed by: A. Garbaruk, M. Shur and M. Strelets — New Technologies and Services LLC (NTS) and St.-Petersburg State Polytechnic University