### 12.2.1. Globally Unstable Flows

#### 12.2.1.1. Flow Physics

The classical example of a globally unstable flow is a flow past a bluff body. Even when computed with a classical URANS model, the simulation will typically provide an unsteady output. Figure 12.17 shows the flow around a triangular cylinder in crossflow as computed with both the SAS-SST and the DES-SST model. It is important to emphasize that the flow is computed with steady-state boundary conditions (as would be employed for a RANS simulation). Still, the flow downstream of the obstacle turns quickly into unsteady (scale-resolving) mode, even though no unsteadiness is introduced by any boundary or interface condition.

From a physical standpoint, such flows are characterized by the formation of new turbulence downstream of the body. This turbulence is independent from, and effectively overrides, the turbulence coming from the thin, attached boundary layers around the body. The turbulence in the attached boundary layers has very little effect on the turbulence in the separated zone. The attached boundary layers can, however, define the separation point/line on a smoothly curved body and so affect the size of the downstream separation zone. This effect can be tackled by a suitable underlying RANS model.

Typical members of this family of flows are given in the list below. Such flows are very common in engineering applications and are also the type of flows where RANS models can exhibit a significant deterioration of their predictive accuracy.

Examples of globally unstable flows include:

- Flows past bluff bodies include:

  - Flow past buildings

  - Landing gears of airplanes

  - Baffles in mixers

  - Side mirrors of cars

  - Stalled wings/sails

  - Re-entry vehicles

  - Trains/trucks/cars in crossflow

  - Tip gap of turbomachinery blades

  - Flows past orifices, sharp nozzles

  - Cavities

  - Flows with large separation zones (relative to attached boundary layer thickness)

- Flows with strong swirl instabilities include:

  - Flow in combustion chambers of gas turbines

  - Flows past vortex generators

  - Some tip vortex flows in adverse pressure gradients

- Flows with strong flow interaction include:

  - Impinging/colliding jets

  - Jets in crossflow

The color scheme of the preceding points above identifies flows that are clearly within the definition of globally unstable flows (black) and those where the type of the flow depends on details of its regime/geometry (gray). Such flows fall in-between globally and locally unstable flows (see Section 12.2.2).

#### 12.2.1.2. Modeling

Of all flows where SRS modeling is required, globally unstable flows are conceptually the easiest to handle. Typically they can be captured by a global RANS-LES model such as SAS, DDES, SDES, or SBES. Such models cover the attached and mildly separated boundary layers in RANS mode, thereby avoiding the high costs of resolving wall turbulence. Due to the strong flow instability past the separation line, there is no need for specifying unsteady inlet turbulence nor to define specific LES zones. Globally unstable flows are also the most beneficial for SRS, as experience shows that RANS models can fail with significant margins of error for such flows. A large number of industrial flows fall into this category.

The safest SRS model for such flows is the SAS approach. It offers the advantage that the RANS model is not affected by the grid spacing and thereby avoids the potential negative effects of (D)DES-type models (gray zones or grid induced separation). The SAS concept reverts back to (U)RANS in case the mesh/time step is not sufficient for LES and thereby preserves a backbone of modeling that is independent of space and time resolution, though at the increased cost that is associated with any transient SRS calculation. SAS also avoids the need for shielding, which for internal flows with multiple walls can suppress turbulence formation in DDES models.

The alternatives to SAS are DDES, SDES, and SBES. If proper care is taken to ensure LES mesh quality in the detached flow regions, these models will be operating in the environment for which they were designed, typically providing high-quality solutions. DDES has shown advantages for flows at the limit of globally unstable flows (see Figure 12.52) where the SAS model can produce URANS-like solutions. In cases like these, DDES still provides SRS in the separated regions. As noted, the DDES has been superseded by the SDES and SBES model family.

For globally unstable flows, the behavior of all global hybrid models is often very similar.

#### 12.2.1.3. Meshing Requirements

The part of the domain where the turbulence model acts in RANS mode has to be covered by a suitable RANS grid. It is especially important that all relevant boundary layers are covered with sufficient resolution (typically a minimum of 10–15 structured cells across the boundary layer). It is assumed that you are familiar with grid requirements for RANS simulations.

The estimate for the lowest possible mesh resolution in the detached SRS region is based on the assumption that the largest relevant scales are similar in size to the width of the instability zone. For a bluff body, the width is the diameter D of the body; for a combustor, the width is the diameter of the core vortex; for a jet in crossflow, the width is the diameter of the jet; and so on. Experience shows that the minimum resolution for such flows is of the order:

| (12–28)

This resolution requires more than 20 cells per characteristic diameter, (in some applications with very strong instabilities, even 10 cells across the layer may be sufficient). As is generally the case for SRS, it is best to provide isotropic (cubic) cells, or at least to avoid large aspect ratios (aspect ratios smaller than 5 would be optimal, but cannot always be achieved in complex geometries).

With the above estimate for , there is a good chance of resolving the main flow instability and the resulting strong turbulent mixing processes associated with the global flow instability (an effect often missed by RANS models). For acoustics simulations, it might also be important to resolve the turbulence generated in the (often thin) shear layer that is separating from the body. Resolving this turbulence poses a much more stringent demand on grid resolution on the simulation, as the shear layer scales with the boundary layer thickness at separation and so can be much smaller than the body dimension. This situation is covered in Section 12.2.2.

#### 12.2.1.4. Numerical Settings

The general numerical settings are described in Section 12.3. Globally unstable flows are relatively forgiving with respect to numerics, at least as far as the mean flow characteristics are concerned. The recommended choice for the advection terms is the Bounded Central Difference (BCD) scheme, especially for complex geometries and flows. For such flows, the classical Central Difference (CD) scheme can be unstable or produce unphysical wiggles in the solution (see Figure 12.60). The BCD scheme is slightly more dissipative, but is substantially more robust and is therefore frequently the optimal choice. If a visual inspection of the flow (see Section 12.5.1) shows that turbulence structures are not produced in agreement with the expectations for the flow, you can switch to CD. If this switch is made, it is advisable to closely monitor the solution (visually and numerically through residuals) to ensure that wiggles are not dominating the simulation. With SAS the “Least Square Cell Based” or the “Node-Based Green Gauss” gradient method should be used in ANSYS Fluent. The latter allows a slightly better representation of the second derivative of the velocity field that is required for the model formulation (von Karman length scale).

In ANSYS CFX, the default hybrid numerical option switches explicitly between the High Resolution Scheme (in the RANS region) and the CD scheme (in the LES region). For most applications, it appears that the use of the BCD scheme should also be favored in ANSYS CFX (see also Section 12.3.1.1)

#### 12.2.1.5. Examples

The following examples have been computed before the availability of the SBES model family. They are therefore based on the SAS/DDES model formulations. Due to the strong flow instability in these flows, the choice of model formulation is marginal and all hybrid models provide fairly similar solutions.

##### 12.2.1.5.1. Flow around a Fighter Aircraft

Figure 12.15 shows a highly complex, globally unstable flow field, around a generic fighter aircraft geometry at high angle of attack as computed with the SAS-SST model. The grid consists of 108 hybrid cells. This simulation is currently in progress within the EU project ATAAC and no detailed discussion of this flow is intended. Figure 12.15 demonstrates the complex regional appearance of resolved turbulence around the aircraft. It is obvious that the application of global models like SAS or DDES greatly simplifies the set up for such flows compared to using ELES/ZLES, where you would have to define the LES regions and suitable interfaces between the RANS and LES regions in a preprocessing step. In contracts, when using global models, the simulation is first carried out in standard RANS mode. Starting from that RANS solution, the model is then simply switched to the SAS or DDES variant of the RANS model, the solver is set to unsteady mode, and the numeric is adjusted according to Section 12.2.1.4. No further adjustment is required in order to produce the solutions shown in Figure 12.15.

Figure 12.15: Turbulence structures for flow around a generic fighter aircraft (Q-criterion) as computed by SAS-SST model

##### 12.2.1.5.2. Flow around a Triangular Cylinder

Figure 12.16 shows the grid around a triangular cylinder in crossflow. The Reynolds number based on the freestream velocity (17.3 [m/s]) and the edge length is 45,500. Periodic boundary conditions have been applied in the spanwise direction. The simulations have been run with ANSYS Fluent using the BCD (Bounded Central Difference) and CD (Central Difference) advection schemes and a time step of (CFL~1 behind cylinder). The grid features 26 cells across its base. It is extended in the spanwise direction to cover 6 times the edge length of the triangle with 81 cells in that direction. Due to the strong global instability of this flow, such resolution was sufficient and has produced highly accurate solutions for mean flow and turbulence quantities (Figure 12.17).

It should be noted that not all flows produce such strong instability as the triangular cylinder, and a higher grid resolution might be required for flows with less instability. Figure 12.17 shows that the grid does not provide resolution of the boundary layer on the walls of the triangular body. This is not a problem in the current case because the wall boundary layer has no influence on the global flow, as it separates at the corners of the triangle. In real flows, this might not always be the case and the boundary layer should be resolved with a RANS-type mesh (that is, a finer mesh in the near-wall region with higher aspect ratios being acceptable).

Figure 12.16: Grid around cylinder in crossflow

Figure 12.17 shows a visual representation of the flow using the DDES-SST and the SAS-SST models with the Q-criterion (see Section 12.5.1). Both simulations have been carried out using the BCD scheme. Both models generate resolved turbulence structures in agreement with the expectation for the grid provided. Figure 12.18 shows a comparison with the experimental data (Sjunnesson et al., 1992 [28]) for the wake velocity profiles as well as for turbulence characteristics.

Figure 12.17: Turbulence structures for flow around a cylinder in crossflow

Figure 12.18: Velocity profiles and turbulence RMS profiles for three different stations downstream of the triangular cylinder (x/a=0.375, x/a=1.53, x/a=3.75). Comparison of SAS-SST, DES-SST models, and experiment. (a) U-velocity, (b) urms, (c) vrms, (d) u’v’

Figure 12.19 shows a comparison of the CD and the BCD scheme for the triangular cylinder using the SAS-SST model. The turbulence content is almost identical, except that some smaller scales are present in the CD simulation downstream of the body. A comparison with experimental data showed results that are almost identical to the ones shown in Figure 12.18 and independent of whether the CD or the BCD scheme was used.

Figure 12.19: SAS-SST simulation for flow around a triangular cylinder using the BCD and the CD scheme for the convective fluxes

##### 12.2.1.5.3. ITS Combustion Chamber

The SAS-SST model is applied to the flow in a single swirl burner investigated experimentally by Schildmacher et al., 2000 [26] at ITS (Institut für Thermische Strömungsmaschinen) of the University of Karlsruhe. The ITS burner is a simplified industrial gas turbine combustor. It concentrates on the swirl flow in the combustion region. Similar to the triangular cylinder test case, the wall boundary layers are not important, which means that this test case is also accessible to pure LES simulations. However, in many industrial combustion chambers wall boundary layers and auxiliary pipe flows have to be considered, which makes them unsuitable for pure LES.

There are two co-axial inlet streams and both are swirling in the same direction. The swirl is generated by means of the two circumferential arrays of blades, which are not included in the current computational domain. The axisymmetric velocity profiles with the circumferential component corresponding to the given swirl number are used as the inlet boundary conditions. The swirl gives the flow a strong global instability, which can be captured well by global SRS models.

Figure 12.20 shows the geometry. The grid shown in Figure 12.21 consists of tetrahedral elements. As stated, the wall boundary layers are not important and are therefore not resolved on this tetrahedral mesh. The simulation was run with ANSYS CFX, which internally converts the grid to a polyhedral grid with control volumes around the grid points for the node-based solver. This means that the polyhedral grid cells are larger than the visual impression from Figure 12.21 with ~20–30 cells covering the relevant length scale , shown in Figure 12.21. The grid does not feature any near-wall boundary layer resolution. It is recommended that you provide such a boundary layer grid for industrial flows (typically more than 10 structured cells across the boundary layer), as in some geometries the separation characteristics near the burner entrance can depend on such details. The convection scheme selected was the default hybrid scheme; however, BCD should also work well.

Figure 12.20: Computational domain for the ITS swirl burner

Figure 12.21: Unstructured grid on the symmetry plane and boundary locations for the ITS swirl burner and relevant length scale, L

The flow structures from the SAS-SST computations of the non-reacting and the reacting flow at a given instance in time are shown in Figure 12.22 using the -criterion (, see Section 12.5.1). The isosurface in Figure 12.22 is given by . The main turbulence structures seem to be captured well in the simulations. Clearly, small-scale turbulence cannot be resolved on such a grid. The grid resolution used here should not be considered as a recommendation for combustion chambers, but as the lowest limit for which such SRS models can be applied.

Figure 12.23 shows a comparison of the standard RANS and SAS results at a given distance from the burner entrance. It shows the level of improvement that results from the application of SRS methods. Many more details of this simulation can be found in Egorov et al., 2010 [6] or in a more detailed analysis of a more complex combustion chamber in Widenhorn et al., 2009 [38].

Figure 12.22: SAS solution for ITS combustion chamber (a) Non-reacting, (b) Reacting flow

Figure 12.23: Reacting flow velocity profiles at the axial distance from the inlet x=103 mm (a) Axial velocity, (b) Tangential velocity

Release 18.2 - © ANSYS, Inc. All rights reserved.