Semi-Confined Flows

Underlying Flow Regime 3-34

Test Case

Brief Description of the Study Test Case

A 3D sketch of the experimental setup is shown in Fig. 1. The configuration presents a GlauertGoldschmied type body consisting of a relatively long fore body and a relatively short concave ramp comprising the aft part of the model mounted between two glass endplate frames with both leading edge and trailing edges faired smoothly with a wind tunnel splitter plate.

Figure 1: 3D sketch of experimental setup [‌1], [‌2]

Major geometric and flow parameters of the TC are presented in Fig.2 and summarized in Table 1 (note that in the “baseline” experiment considered here the slot shown in Fig.2 was closed).

Figure 2: Schematic of TC geometry of the flow parameters

Table 1: Major geometrical and flow parameters Parameter

Notation

Value

Free stream velocity

U

34.6 m/s

Hump chord

c

0.42 m

Crest height

h

0.0537 m

Reynolds number

Re=Uc/ν

936, 000

Mach number

M

0.1

The experimental data are available at http://cfdval2004.larc.nasa.gov/case3expdata.html (Case 3), at https://turbmodels.larc.nasa.gov/nasahump_val.html, and also enter the ERCOFTAC

�Classic Collection http://cfd.mace.manchester.ac.uk/ercoftac under number C.83. The data set includes: streamwise distributions of the surface pressure and skin-friction coefficients, C P and C f , and mean velocity and Reynolds stresses fields in the tunnel center-plane, roughly covering the region 0.63 < x/c < 1.39.

Test Case Experiments

A photo of the experimental rig is presented in Fig.3.

Figure 3: Photo of the experimental rig

The experiments were performed in the NASA Langley 20′′×28′′ shear flow tunnel. The flow was nominally 2D, although with side-wall effects (3D flow) expected near the endplates. The reference “chord” length of the model, c, is defined as the length of the hump on the wall and is equal to 420mm. The maximum thickness of the hump, h, is equal to 53.7mm. The model was equipped with 153 centre-span static pressure ports and 20 dynamic pressure ports in the vicinity of the separated flow region. Sixteen spanwise pressure ports were located on the fore body (x/c = 0.19) and on the ramp at (x/c = 0.86). Two-dimensional PIV data were acquired in a plane, along the model centreline and normal to the surface, starting from right upstream of the slot and ending well beyond the reattachment location at x/c ≈ 1.4. Stereoscopic PIV (3D) data were acquired in planes perpendicular to the flow direction, arranged to intersect the 2D plane from x/c = 0.7 to 1.3 in steps of approximately 0.1. Oil-film interferometry was used to quantify the skin friction over the entire model, from the region upstream of the hump to beyond the reattachment location. Two-dimensionality of the flow in the separated and reattachment region was thoroughly assessed via three methods: by considering the spanwise pressures on the ramp in the separated region, performing 3D PIV measurements in planes perpendicular to the flow direction, and by means of the surface oil-film flow visualization. Spanwise distribution of the surface pressure was also measured on the fore body of the model. It was shown that the spanwise variations of the flow parameters are small (e.g., at the test condition, the pressure variation over the central half of the model (–0.25 ≤ z/c ≤ 0.25) is ∆CP = ±0.005) and that departures from twodimensionality are observed mainly near the wall. At the inflow location (x/c = –2.14), pitot-probe and hot-wire anemometer data were compared with 2D and 3D PIV. Inflow skin friction was also documented using oil-film interferometry. Resulting inflow velocity profile which was used in the numerical studies as a benchmark for imposing boundary conditions at the inflow of the computational domain (see the next section) is shown in Fig.4.

Figure 4: Experimental profile of streamwise velocity at x/c = -2.14 (momentum thickness Re_θ=7200)

Experimental uncertainties reported in the original experimental papers are summarized in Table 2. Note that there is also an operational uncertainty associated with the endplates blockage effect, which should be compensated in the quasi-2D simulations (see next sub-section).

CFD Codes and Methods

As mentioned in the Introduction, the present document focuses on the three groups of CFD studies of the considered test case, namely, on its predictions obtained with the use of different RANS models [7], hybrid RANS-LES models [8], [9] and WRLES [6] (see Table 3).

Naturally, corresponding numerical procedures and codes are quite different.

In particular, the RANS based computations, results of which are presented on the NASA Turbulence Modeling Resource portal were carried out with the use of two long-standing compressible Navier-Stokes CFD codes developed at NASA Langley Research Center for solving 2D and 3D compressible flows on structured (CFL3D code https://cfl3d.larc.nasa.gov/) and unstructured (FUN3D code https://fun3d.larc.nasa.gov/) grids. The grids used in the computations are built according to the well-know guidelines for solving RANS equations (the grids are available on the portal [7]) and both codes return virtually identical results, thus suggesting code- and (indirectly) grid-independence of the obtained solutions.

The RANS-LES computations carried out in [8], [9] employed two enhanced hybrid models equipped with special tools for the “Grey-Area” Mitigation (GAM): a non-zonal method Delayed DES (DDES) [10] with Shear-Layer Adapted (SLA) subgrid length scale [11] and a zonal Improved DDES (IDDES) [12] combined with Synthetic Turbulence Generator (STG) [13] or Synthetic Eddy Method (SEM) [14], [15] for imposing boundary conditions at the RANS-IDDES interface. The shear-layer adapted subgrid length scale [11] replaces the length scale of the original DDES equal to the maximum grid spacing . It accounts for strong anisotropy typical of the grids in the initial part of separated shear layers and the quasi-2D character of the flow in this region. This substitution results in a considerable reduction of the subgrid eddy-viscosity, thus ensuring a rapid development of 3D turbulence structures.

A matrix of the performed simulations and appropriate references to original publications which provide a detailed outline of the approaches used are presented in Table 4.

The non-zonal simulation was conducted with the use of the well-established in-house finite- volume structured multi-block code NTS, whereas for the zonal ones, along with this code, an unstructured compressible finite-volume code TAU of DLR was employed.

The incompressible branch of the NTS code used in the simulations is based on the flux- difference splitting method of Rogers and Kwak [18]. The approximation of the inviscid fluxes in the code depends on the turbulence representation approach: in the zonal RANS-IDDES computations, it is a 3rd-order upwind-biased scheme in the RANS zone and a 4th-order central scheme in the WMLES zone, whereas for the non-zonal DDES the hybrid (weighted 3rd-order upwind-biased / 4th-order central) scheme [19] is used. The viscous fluxes are approximated with the 2nd-order central scheme. For the time integration, an implicit 2nd-order backward Euler scheme with sub-iterations is applied.

The TAU code employs a low-dissipation low-dispersion (LD2) scheme [16] which is based on the 2nd-order energy-conserving skew-symmetric convection operator combined with a minimal level of 4th-order artificial matrix dissipation for stabilization. The central flux terms employ an additional gradient extrapolation that effectively increases the discretization stencil and is used to reduce the dispersion error of the scheme. Both ingredients are essential in terms of turbulence resolution with the unstructured TAU code. Note that in the present zonal RANS-WMLES computations, the LD2 scheme is only active in the respective IDDES region downstream of the interface. The temporal discretization is based on an implicit dual-time stepping scheme which is also of 2nd-order accuracy.

All the hybrid simulations were performed in the same computational domain and on the same grid (“mandatory” grid in the Go4Hybrid project).

The computational domain in the XY-plane is shown in Fig. 5. Its size in the spanwise direction is equal to 0.4c (this has been proven sufficient to arrive at a span-independent solution within the ATAAC project [4]). As recommended in [7], the contour of the upper (slip) wall of the domain was modified (moved somewhat downwards in the area above the hump) in order to compensate the blockage effect of the endplates (see Fig. 1 above).

Figure 5: Schematic of computational domain in XY-plane and wall boundary conditions [8], [9]

The inflow and outflow conditions in the simulations performed with the use of the TAU and NTS codes were somewhat different since the former code is compressible and in the latter one its incompressible branch was employed. In both cases velocity and turbulence quantities (k and .) at the inflow boundary (x/c = -2.14) were specified from a precursor SST RANS of the zero pressure gradient boundary layer carried out to match the experimental value of the momentum thickness based Re-number (see Fig. 4 above). In the incompressible simulations (NTS code), the inflow static pressure was defined by the linear extrapolation of the values in the nearby interior cells of the domain, whereas in the compressible simulations (TAU code) flux boundary conditions were used together with an extrapolation of the pressure from the interior. At the outflow boundary, in the NTS code a constant static pressure is specified and all the other flow variables are defined by linear extrapolation from the interior cells of the domain, which is similar to TAU’s flux conditions with an imposed fixed exit pressure. Finally, in all simulations the boundary conditions in the spanwise direction were periodic.

Contributed by: E. Guseva, M. Strelets — Peter the Great St. Petersburg Polytechnic University (SPbPU)