Transonic/Supersonic External Aerodynamics: Steady State RANS Approach

Recommended Domain Settings

Use a spherical far-field boundary, with domain extents around 8–10 body lengths or wing spans, whichever is larger, from the body. The mesh size on this boundary can be large: typically of the order of the body length.
- When replicating a wind-tunnel test, modeling the wind-tunnel walls is appropriate if blockage effects are important. In this case, slip walls are often defined at the tunnel walls, and no prism layers are constructed.
Use a freestream boundary condition type at the far-field.
Using a half-body with a symmetry plane is appropriate for cases with no sideslip. Take care to match the symmetry plane mesh growth with the volume mesh growth.
Optional: Angles of attack/sideslip are typically defined by changing the far-field boundary condition flow direction, not the orientation of the body.

Recommended Physics Setup

To set up a transonic/supersonic external aerodynamics model using the steady state RANS approach, choose the following physics models in order:


Group Box	Model
Space	Three Dimensional
Time	Steady
Material	Gas
Flow	Coupled Flow
Equation of State	Ideal Gas
Optional Physics Model	Coupled Energy (Selected automatically)
Viscous Regime	Turbulent
Turbulence	Reynolds-Averaged Navier-Stokes (Selected automatically)
Turbulence	SST K-Omega or Spalart-Allmaras

To select the specific turbulence model, choose from the following:

The SST K-Omega model is preferred. This model is robust, is well-behaved near walls, and does well in recirculation regions.
Either the low y+ or all y+ boundary treatments can be used with this model, depending on the mesh. This model works best when complex geometric protrusions exist, bluff body separation occurs, and at supersonic speeds.
The Spalart-Allmaras turbulence model can be used in cases of streamlined geometries without large base separation regions. This model works best for attached boundary layers or mildly separated flows (that is, flow past a wing at or below stall), and at subsonic speeds.

Recommended Mesh Settings

Both polyhedral and trimmed meshes have proven successful on this class of problem. In either case, typical rules for good meshing practices apply and are important. The mesh should give proper resolution of geometry and flow field features, along with good cell quality.

For instance, refine the mesh:

Around leading and trailing edges of lifting surfaces, control surfaces, and other protrusions.
At tips of lifting surfaces and control surfaces in order to capture vortices that are shed in these locations.
At body/lifting-surface junctions.
Where shocks exist.
To resolve any bluff-body wakes.
On airfoil leading edges. Use aligned surface meshes in these regions when possible.
If feasible, use at least two cells to resolve thin blunt leading edges, or other thin step-like protrusions.

Note

External aerodynamics simulations can be sensitive to the quality of the surface geometry representation. Care must be taken when using the surface wrapper such that junctions/intersections result in smooth, well-defined edges. Whenever possible, the preferred approach is to start with clean CAD geometry and bypass surface wrapping.

Polyhedral Meshes

Polyhedra have the advantage of smooth growth away from the body.
Due to the smooth growth behavior, polyhedral are typically preferred when aerodynamic coefficients are of key importance.
Due to the pseudo-random orientation of the faces, polyhedra also generally give better results than trimmed meshes when large sweeps in flow direction (such as angle of attack or sideslip) are used.
Typical polyhedral meshes contain 2–20 million cells, depending on the complexity of the geometry and flow field, and the near-wall treatment.
Use Volume Growth Rate, with the expansion rate set between 1.05 and 1.15.

Note	Be careful when using volumetric controls with polyhedral meshes: abrupt changes in cell size can occur if there is a significant difference in the sizes that are specified on the surface and in the volumetric control.

Trimmed Meshes

If you are modeling a single flow direction, or only small variation in flow, a trimmed mesh with the grid lines aligned with the flow often provides the most efficient approach to getting good answers.
Typical trimmed meshes contain 4–40 million cells, depending on the complexity of the geometry and flow field, and the near-wall treatment.
In order to capture the near field properly, set the volume growth rate to Slow or Very Slow.

Prism Layers

Proper resolution of the boundary layer is critical. Choose the thickness of the prism layer such that the entire boundary layer is contained within it.
The use of wall functions rather than integrating to the wall can be appropriate for the SST K-Omega turbulence model depending on several factors, including
- Desired accuracy
- Relative importance of skin friction drag
- Importance of transition
- Existence/importance of separation/reattachment on smooth boundaries
- For integrating to the wall, 20–30 prism layers are typically used, with the near-wall y+ being of the order 1.
- For wall functions, 5–8 prism layers are typically used, with the near-wall y+ being of the order 50–150.

When using the Spalart-Allmaras Turbulence model, integrate to the wall (do not use wall functions).

Solution Procedure

To improve convergence, especially as the Mach number increases, order the cells in the general direction of the flow using directional reordering.

Initialization

Grid sequencing initialization with default values typically works well for this type of problem, and is recommended up to around Mach 2.
The flow field can be initialized to uniform conditions matching the far-field boundary—recommended for Mach numbers greater than 2. However, an arbitrary linear boundary layer profile in the initialization (using a field function) may be required.

Solution

The Expert Driver with default values works well.
Appropriate CFL values are dependent on mesh quality and Mach number.
For a high-quality mesh, a general rule-of-thumb is $C F L \approx 20 / M a c h$ for this regime. For example $C F L \approx 40$ for Mach 0.5, and $C F L \approx 10$ for Mach 2.

If the Expert Driver is used, CFL ramping is necessary only if poor-quality cells are present or if the flow field is especially complex.
Residuals may drop by only 2–3 orders of magnitude for this type of problem, especially if grid sequencing initialization is used (because grid sequencing initialization provides a better initial estimate of the flow field).
Monitor the forces and moments on the object to determine convergence.