A review of guidelines and best practices for subsonic aerodynamic simulations using RANS CFD

Abstract

This paper presents a review of guidelines and best practices for low-speed aerodynamic simulations of aircraft using finite volume RANS CFD methods. Recommendations for geometry preparation, domain size as well as surface and volume mesh refinements are given. It is found that 100 surface cells in the flow direction are usually appropriate for most aircraft components. RANS wall treatment methods are crucial, and only a full discretization of the boundary layer is appropriate in aerodynamic simulations. Different aspects of choosing temporal discretization, boundary conditions and solver algorithms are briefly presented. It is recommended to use a pressure-based solver due to its distinct advantages in low-speed flows. Both Spalart-Allmaras and Menter's SST turbulence models have proven accurate for aerodynamic flows. Turbulence models should be adjusted with non-linear constitutive relations that greatly enhance prediction accuracy. The paper also presents multiple guidelines for checking plausibility that focus on flow visualizations of different components.

Full text

ISBN number 978-1-925627-40-4
A review of guidelines and best practices for subsonic aer-
odynamic simulations using RANS CFD
Falk Goetten, D. Felix Finger, Matthew Marino, Cees Bil
School of Engineering, RMIT University, 264 Plenty Road, Bundoora, Victoria 3083, Australia
goetten@fh.aachen.de, f.finger@fh-aachen.de, matthew.marino@rmit.edu.au, cees.bil@rmit.edu.au
Marc Havermann, Carsten Braun
Department of Aerospace Engineering,
FH Aachen University of Applied Sciences, Hohenstaufenallee 6, 52064 Aachen, Germany
havermann@fh-aachen.de, c.braun@fh-aachen.de
Abstract. This paper presents a review of guidelines and best practices for low-speed aerody-
namic simulations of aircraft using finite volume RANS CFD methods. Recommendations for
geometry preparation, domain size as well as surface and volume mesh refinements are given.
It is found that 100 surface cells in the flow direction are usually appropriate for most aircraft
components. RANS wall treatment methods are crucial, and only a full discretization of the
boundary layer is appropriate in aerodynamic simulations. Different aspects of choosing tem-
poral discretization, boundary conditions and solver algorithms are briefly presented. It is
recommended to use a pressure-based solver due to its distinct advantages in low-speed flows.
Both Spalart-Allmaras and Menter’s SST turbulence models have proven accurate for aerody-
namic flows. Turbulence models should be adjusted with non-linear constitutive relations that
greatly enhance prediction accuracy. The paper also presents multiple guidelines for checking
plausibility that focus on flow visualizations of different components.
NOMENCLATURE
A cell face area
CAD computer-aided design
CD drag coefficient
Cf skin friction coefficient
CFD computational fluid
dynamics
CV control volume
E additive constant
I identity matrix
IGES initial graphics
exchange specification
L/D lift-to-drag ratio
RANS Reynolds-averaged
Navier-Stokes
Rex Reynolds number with
length x
S source term
s height of first cell adjacent
to wall
SDR specific dissipation rate
STEP standard for the exchange of
product model data
STL stereolithography
T stress tensor
T’ fluctuating stress tensor
TKE turbulent kinetic energy
U velocity vector
U∞freestream velocity
V cell volume
y wall distance
p
averaged pressure
U
averaged velocity vector
u+ normalised velocity
uτ friction velocity
y+ normalised wall distance
Γ diffusion coefficient
δxturbulent boundary layer
thickness
κ von Kármán constant
μ dynamic viscosity
μtturbulent viscosity
ρ density
τw wall shear stress
Φ any flow variable

INTRODUCTION
The steady increase of computational power in conjunction with the advancements in simulation soft-
ware have fundamentally changed the way numeric simulations for low-speed aircraft aerodynamic
analyses are applied today. Volume resolving Reynolds-Averaged-Navier-Stokes (RANS) methods are
in widespread use, both in early and detailed design stages. The increasing commodity of finite volume
RANS Computational Fluid Dynamics (CFD) methods is not only a result of increased computational
capacities but also due to the significant enhancements in commercial and non-commercial simulation
software, algorithms and user-friendliness. While these improvements allow engineers to generate sim-
ulation models very quickly, it does not diminish the necessity to take enormous care in each step and
to choose from a vast amount of simulation settings.
Numerous publications (e.g. (Georgiadis et al. 1995), (Menter et al. 2003), (Spalart and Rumsey 2007)
and (Ewing 2015)) provide guidelines for different aspects of the RANS finite-volume simulation setup,
often referring to individual use cases and flight regimes. The amount of guidelines is further increased
by the user manuals of commercial software like FLUENT (ANSYS Inc. 2019b) or StarCCM+ (Siemens
PLM Software 2019). Following the relevant and up-to-date guidelines for low-speed aerodynamic sim-
ulations can be very complicated. Some publications might deal with a very specific topic (e.g. a mesh
setting) in depth, but understandably do not cover other aspects of a simulation setup. User manuals of
CFD software can easily be confusing, as they need to cover the complete functionalities of the program.
The capabilities of modern commercial CFD software goes far beyond aerodynamic simulations, which
is reflected in the user guides. Specific information for aerodynamic cases might therefore be hard to
detect. The literature currently lacks an overview document that comprises the most important guide-
lines for low-speed RANS aerodynamic simulation of aircraft. This paper aims to close this gap by
providing a broad overview of the most common configuration settings one might encounter. It focuses
on low-speed subsonic flight regimes typical for general aviation and unmanned aircraft. These simu-
lations aim to model the aerodynamic behavior of a complete aircraft or individual aircraft components.
Interior flow systems like air conditioning or engine cooling are not considered.
The reviewed guidelines are kept as generic as possible to make them applicable to a wide variety of
software. Specific features of individual software packages are therefore omitted. The guidelines de-
scribed in this publication are based on multiple analyses performed by the authors and findings of other
researchers. It is clearly indicated whenever the authors provide guidelines and recommendations based
on their own experience. In any other case, the reference that provides the information is given.
The paper is structured according to the characteristic workflow for performing aerodynamic analyses
of aircraft. Within each step, the guidelines for the individual actions found in the literature are sum-
marized and, where possible, supported by analyses and test cases. This publication is by no means
exhaustive and the reader is referred to additional literature on multiple occasions.
GEOMETRY PREPARATION AND IMPORT
The first step in performing a CFD analysis of an aircraft is usually the preparation of the aircraft’s
geometry. This step is crucial as it has the potential of affecting the complete analysis process. A well-
designed geometry that is tailored to the requirements for CFD can smoothen the whole analysis process,
while a geometry designed for another purpose usually leads to additional workload. It is common to
use dedicated Computer Aided Design (CAD) software to provide an aircraft’s geometry. The authors
recommend using NASA’s Open Vehicle Sketch Pad (OpenVSP), see (Gloudemans et al. 1996) for
quick geometry creation of complete configurations. This software allows a parametric definition of
multiple aircraft components and has proven extremely valuable in several analyses of the authors (Göt-
ten et al. 2018a⁠; Götten et al. 2018b), (Finger et al. 2018), (Götten et al. 2019a).
Four fundamental CAD design rules are recommended:
1. Create individual bodies for each aircraft component and use a rigorous naming convention (wing,
fuselage, h-tail, etc.). This allows treating aircraft components individually during meshing and
post-processing. Individual bodies also allow calculating force and moment coefficients for each
body separately. This is very valuable during a drag breakdown or a trim analysis.

2. Create a clean surface without imperfections and omit tiny details (rivets, door panels, etc.). Small
details or imperfections can increase discretization effort disproportionally to their aerodynamic
effects (Lanfrit 2005). This, of course, depends on the size and location of the neglected compo-
nents. One should start by cleaning the surface from unwanted details and perform tests by adding
them in later analysis stages.
3. Avoid sharp edges commonly found at trailing edges of
lifting surfaces. This might lead to highly skewed and low-
quality cells causing numerical instabilities (Ewing 2015).
The authors found it convenient to round off sharp edges
with a tiny radius. In this way, most standard meshing al-
gorithms recognize this radius as a location of high curva-
ture and automatically provide the necessary refinement at
the trailing edge. The trailing edge radius should be small
(on the order of 1-5 ‰ of the chord length). A comparison
of the cell skewness angle near a sharp and round trailing
edge of a NACA 4415 airfoil is shown in Figure 1. The
mesh is created with the hybrid prism-polyhedral approach
of StarCCM+. In case a sharp trailing edge is used, the
algorithm creates cells with skewness angles of up to 70
degrees. Such cells can result in poor numerical stability
and reduced convergence. In contrast, the case with a
round trailing edge shows much smaller skewness angles
with a maximum value of 45.
4. Create a watertight surface and close any holes in the ge-
ometry. These are typically ventilation outlets or static ports in an aircraft analysis. Several CFD
meshing algorithms have functions for detecting holes in the geometry and close them automati-
cally. However, this could result in an alteration of surface curvature, which should be handled with
utmost care.
Most CAD software allow exporting the geometry in vendor-neutral file formats that can be read by
CFD software. Popular vendor-neutral file formats are “.stl” (Stereolithography), “.iges” (Initial
Graphics Exchange Specification) and “.step” (Standard for the Exchange of Product Model Data). The
following section gives a small description of the formats, including several recommendations for their
use in CFD.
The stereolithography (STL) file format discretizes the geometry with flat-faced triangles and has its
origins in rapid prototyping (Kai et al. 1997). It can only describe the outer surface of a body and has
no means of creating solid components. The export of this file format requires a surface triangulation
already in the CAD tool. Curvature is captured by reducing triangle size. The authors recommend that
the stereolithographic discretization is much smaller than the intended surface discretization of the CFD
mesh. In such, the user needs to have an estimate of the desired surface cell size already when exporting
the CAD geometry. It is necessary to export all aircraft components individually and recombine them
in the CFD environment to have individual bodies available.
The Initial Graphics Exchange Specification (IGES) (Nagel et al. 1980) is a file format designed to
exchange various types of product data. It uses a combination of multiple simple geometry elements
(lines, splines, arcs, cones, etc.) to create a complete product. This is advantageous as those elements
can directly capture curvature. When aircraft components are created as individual bodies, IGES keeps
such information, and individual bodies are available in the CFD environment. In this way, only a single
IGES file can represent a complete aircraft.
The Standard for the Exchange of Product Model Data (STEP) (ISO 10303-21 1994) is a universal file
exchange format which uses the EXPRESS data modelling language. Its basic technique is comparable
to the IGES approach. When used appropriately, all described file formats are well suited for providing
adequate input geometries for CFD software. The authors recommend using IGES and STEP when
dealing with a significant amount of individual bodies, as only one file has to be exported.
a)
b)
Figure 1. Cell skewness angle at a)
sharp and b) round trailing edge

FLOWFIELD DIMENSIONS
External aerodynamic simulations of aircraft are usually performed as freestream simulations. These
types of simulations aim to analyze the aircraft in free atmospheric flight conditions. The flow field
surrounding the aircraft model must, therefore, be large enough to represent this, both physically and
numerically. If the flow field dimensions are too small, the prescribed boundary conditions can signif-
icantly affect the simulation results. For low Mach number cases velocity based inlet and pressure based
outlet conditions are appropriate, (Ferziger and Perić 2002). The flow at inlet and outlet boundary must
be smooth, and flow disturbances from the aircraft body should have diminished. The flow domain
might be bullet-shaped (ANSYS Inc. 2019b), (Siemens PLM Software 2019). This allows using the
curved surface as the inlet and the rear surface as the outlet condition.
The scientific literature provides multi-
ple guidelines for flow field extents.
These flow domain extensions are
specified with reference to a character-
istic length of the analysis body. For
2D airfoils, this is usually the chord
length, while for complete aircraft the
maximum body length is more com-
mon. Both (Hirsch 2002) and (Spalart
and Rumsey 2007) recommend a flow
domain of at least 50 body length for
3D simulations of a wing. (Versteeg
and Malalasekera 2007) indicate that
the outlet boundary condition should be
positioned significantly more than ten
reference lengths behind the body in a
3D simulation. (ANSYS Inc. 2019b) and (Siemens PLM Software 2019) recommend extending the
domain 25-50 maximum body lengths around an aircraft in 3D.
The recommendations for 2D domain extents are significantly larger than for 3D domains as disturb-
ances decrease slower in 2D. (Haase et al. 1992) show that domain extents of far more than 40 chord
lengths are necessary in a 2D airfoil simulation. (Rumsey 2014) investigated the influence of the flow
domain size on the results of a 2D simulation of a NACA 0012 airfoil at high lift conditions. His essen-
tial findings are presented in Figure 2. Both lift and drag coefficient show changes with an increase in
domain size. The effect is reduced for large domains. Deviations between a domain size extending 100
chord lengths and 500 chord lengths are in the order of 1%. (Rumsey 2014) therefore recommends that
a domain length of 500 chords is by far enough. The influence of the domain size also depends on the
chosen mesh type, mesh density, and physical settings.
The literature findings suggest that for 3D simulations the domain should extend at least 50 body lengths,
while for 2D simulations 200 reference lengths might be appropriate. The authors’ experience confirm
these findings. Nevertheless, an adequate domain size can still depend on the individual problem and
one should perform tests with various domain sizes in order to guarantee solutions that are independent
of the domain extents.
FINITE VOLUME DISCRETIZATION AND MESH GENERATION
Most commercial CFD packages and several open source codes use an unstructured finite volume dis-
cretization in the numerical solution of the governing transport equations (Siemens PLM Software
2019), (ANSYS Inc. 2019a), (ANSYS Inc. 2019b), (Fluidyn 2019), (OpenFOAM 2010). This discreti-
zation technique applies an integral form of the transport equations on small control volumes. The
following sections outline the very basics of the finite volume method and describe frequently used
control volume types. Additional information for creating an adequate volume mesh in aerodynamic
simulations is provided.
Figure 2. Effect of domain extent on lift and drag coeffi-
cient of a NACA0012 at α=15° and Re= 6x10
6 with data
from (Rumsey 2014)
0 100 200 300 400 500 600
0.0278
0.0280
0.0282
0.0284
0.0286
0.0288
0.0290
0.0292
1.5055
1.5060
1.5065
1.5070
1.5075
1.5080
1.5085
1.5090
0 100 200 300 400 500 600
C
D
CL
Domain extents in chord lengths
CL CD

Finite Volume Discretization
The integral form of the general transport equation for any fluid property

is shown in Eq. (1). The
first term on the left-hand side describes the rate of change of the total amount of fluid in the respective
control volume (transient term). The second term is the net rate of decrease in fluid property due to
convection out of the surface of the control volume (convective flux). The left term on the right-hand
side is the net rate of increase of fluid property due to diffusion through the control volume’s surface
(diffusive flux). The right term on the right-hand side gives the rate of increase of the fluid property
due to sources inside the control volume (source term). Different methods for calculating surface and
volume integrals are available and specific to the individual CFD code. Industry-standard commercial
codes frequently use second-order accurate methods (Siemens PLM Software 2019), (ANSYS Inc.
2019a) (ANSYS Inc. 2019b). A review of the finite volume method is beyond the scope of this paper.
A further description can be found in (Moukalled et al. 2016). The choice of the general shape of the
control volume can have a significant influence on the overall simulation process. Not only are different
meshing algorithms associated with different types of control volumes, but the choice of control volume
type also affects overall cell count and convergence behavior. The three most prominent cell types in
the finite volume method are tetrahedron, hexahedron, and polyhedron (Versteeg and Malalasekera
2007), see Figure 3.



 +n. (U)

=n. ()

+

 (1)
a)
b)
c)
Figure 3. a) Tetrahedron cell, b) Hexahedron cell, c) Polyhedron cell
The algorithms used to create those different cell types might differ between individual codes, and no
attempt is made to outline them here. In general, creating tetrahedral cells is often the fastest way to
generate a computational mesh and requires the least amount of memory. Polyhedral cells are generated
by transferring an initial mesh consisting of tetrahedral cells to polyhedral ones. This is usually time-
consuming. The generation of polyhedral cells is regarded as the most complex mesh generation. Hex-
ahedral cells can be directly generated and their creation is well parallelizable. One common algorithm
is the Cartesian cut-cell (trimmed) approach that aims for cube-like cells. Time and memory consump-
tion form a good compromise between tetrahedral and polyhedral cells, see (Versteeg and Malalasekera
2007).
A sufficient number of cells must be used to discretize the computational domain in order to achieve a
certain level of accuracy. The necessary number of cells differs for the above-described control volume
types. (Sosnowski et al. 2017) found that more than three times the amount of tetrahedral cells are
necessary to achieve the same level of accuracy compared to polyhedral cells. (Perić and Ferguson
2005) state that in many practical test cases, polyhedral meshes achieve the same level of accuracy like
tetrahedral meshes with about four times fewer cells and about one-fifth of the computation time. Pol-
yhedral cells have more neighboring cells than hexahedral or tetrahedral elements. Information spreads
faster throughout the domain as it is transferred through the element’s cell faces. This enhances gradient
approximation and results in faster convergence with fewer cells. The authors find that hexahedral cells
are often a good compromise between accuracy and computational cost. Multiple tests showed that
besides the advantages stated for polyhedral cells, hexahedral cells using a trimmed cut-cell approach
are more convenient in some cases. In general, the user’s mesh creation control using local volumetric
and surface refinements as well as mesh growth rates is more intuitive with hexahedral cells than with
polyhedral cells. Additionally, the mesh creation time using a hexahedral trimmed cut-cell approach is
significantly shorter compared to polyhedral cells.
A universally valid statement which cell type should be preferred for aerodynamic calculations is not
possible. Tetrahedral cells have disadvantages compared to both hexahedral and polyhedral cells and
should be avoided, if possible. Hexahedral trimmed meshes are beneficial due to their advantageous

combination of fast mesh creation and good accuracy. Especially in simulations that involve a large
number of individual bodies and a generally high cell count, (typical for full aircraft simulations) the
creation time of hexahedral meshes is much faster compared to polyhedral meshes. The authors have
noted that this can significantly reduce overall turnaround time from mesh creation to final solution. In
case multiple simulations with the same geometry are performed (for instance a parametric study, (see
(Götten et al. 2019a))) polyhedral meshes have the distinct advantage of fast convergence and should
be preferred.
Volume Meshing
The goal of creating the volume mesh is to provide a discretization that allows solving the transport
equations with sufficient accuracy. The required level of discretization depends on the individual prob-
lem. A uniform mesh resolution within the overall domain is practically impossible for aerodynamic
simulations of aircraft. Due to the large extents of the domain, this would result in an excessive number
of cells. An unstructured meshing approach, therefore, relies on having different cell sizes throughout
the domain. The aim is to provide a fine discretization where it is needed and a coarser level where
appropriate. As a general rule of thumb, the required mesh resolution is anti-proportional to the flow
gradients in this region. Flow gradients far away from the aircraft’s body will be quite small, as the
flow is undisturbed. The control volume size (cell size) might be large in these regions, without harming
solution quality. In contrast, flow gradients in the close vicinity of the aircraft will be much higher.
Capturing all related effects in these regions may requires a much finer mesh resolution.
The following section provides a list of regions, which need a fine discretization in almost any case.
Recommendations for several cell sizes are given.
Lifting surfaces
About 80-100 cells in the chord wise direction are appropriate as determined in multiple grid independ-
ence studies by the authors. If transition models are used, the surface discretization needs to be finer,
on the order of 100-200 cells in the chord wise direction (Menter et al. 2015). Both leading and trailing
edges need to be refined. Care should be taken that the leading edge curvature is accurately captured.
A good starting value is to create leading and trailing edge cells with about 0.1% chord length, (Mav-
riplis et al. 2009). Depending on the case, one might need a significant wake refinement, especially in
high lift conditions involving separation.
Fuselage
The authors recommend that the basic guidelines for a lifting surface mesh apply as well. Cases in
which the fuselage has a relatively blunt tail require wake refinements to capture flow fluctuations in
this region.
Landing gear
Landing gears often behave like bluff bodies. Depending on the flow conditions and geometry, this
might result in significant flow oscillations in the landing gear’s wake. These oscillations are associated
with high flow gradients that need to be captured by local refinements. Meshing the landing gear is
often considered a challenge, as its dimensions are small compared to other components like the air-
craft’s fuselage. Very small cells are required to capture the complex geometry, which can lead to an
excessive cell count. The authors recommend taking the guidelines for lifting surfaces as a start value
for tire and strut discretization but note that occasionally one has to accept a coarser mesh in order to
keep the overall cell count tolerable.
Attachments
For wing-like components (e.g. flat antennas), the same recommendations like for lifting surfaces apply.
At least 100 cells should be used to discretize the circumference of spherical bodies like UAV’s gimbals.
This strongly depends on the exact geometry and flow conditions. The authors have also experienced
cases at very low Reynolds numbers in which grid independent solutions required more than 400 cells
in the circumferential direction (Götten et al. 2019b).

Mesh independence
Finding an appropriate discretization is
somewhat different from case to case and
can be time-consuming. A mesh independ-
ence study aims to find a level of discreti-
zation that allows solving the transport
equations accurately. Mesh independence
studies are usually undertaken considering
one or more parameters of interest. In air-
craft aerodynamics, lift, drag or moment co-
efficients are often used, see (Haase et al.
1992). In case, a complete aircraft is simu-
lated, one should analyze lift, drag and mo-
ment of each component, and check for
mesh independency. Consider Figure 4 as
an example for a grid independence study
of UAV simulation conducted by the au-
thors. The total lift-to-drag ratio seems to
be mesh independent using more than 15 million cells. One might be compelled to stop the mesh inde-
pendency study at this point. However, the individual drag coefficient of a small antenna still changes
significantly using a finer mesh. This cannot be seen considering only overall lift-to-drag ratio, as the
influence of the antenna’s drag is small.
Finer meshes can be created by decreasing all cells in the domain by a certain percentage. This, how-
ever, might significantly increase global cell count and affect regions in which a finer discretization is
not necessary. Adaptive mesh refinements have gained significant attention in recent years and have
been implemented and partly automated in most commercial CFD packages (ANSYS Inc. 2019a), (AN-
SYS Inc. 2019b), (Siemens PLM Software 2019). These algorithms detect regions, which require a
finer discretization by analyzing flow solutions starting with coarse meshes. A common approach is to
analyze turbulent quantities or velocity gradients. The mesh is then only refined in these regions and
the simulation re-executed. The process is continued until a mesh independent solution is achieved.
The advantage of this method is its high level of automation with minimal human interaction and very
efficient mesh refinements. A visualization of the regions that are refined by detecting high values of
turbulent kinetic energy for a reconnaissance UAV is presented in Figure 5. The authors have frequently
used turbulent kinetic energy as a refinement criterion for subsonic aircraft and especially recommend
using it, when wake effects are critical. Other detection methods might be used depending on the indi-
vidual case. (Hartmann and Houston 2009) found that the overall time to achieve a mesh independent
solution could be reduced considerably using adaptive mesh refinements. Numerous tests by the authors
confirm this, and it is recommended to apply adaptive refinement methods whenever possible.
Figure 5. Regions detected for local volumetric refinement based on turbulent kinetic energy
Figure 4. Mesh independence study based on L/D and
the individual drag coefficient of a small antenna
0.0
0.2
0.4
0.6
0.8
1.0
1.2
1.4
1.6
1.8
2.0
20.0
21.0
22.0
23.0
24.0
25.0
0 5 10 15 20 25 30
CDAntenna x10- 4
L/D
Cell count in millions
L/D
CD Antenna

Wall Treatment
RANS simulations require special treatment of near-wall regions that are affected by the bodies’ bound-
ary layers. The near wall region is described by the law of the wall that connects the dimensionless
velocity u+ and the dimensionless wall distance y+ via the relationships shown in Eq. (2) and Eq. (3),
(Ferziger and Perić 2002). The near wall region is divided into three fundamental layers shown in
Figure 6. The viscous sublayer in which viscous effects are dominant (y+<5), the buffer layer in which
both viscous and turbulent stresses are dominant (5<y+<30) and the log-law layer in which turbulent
stresses are dominant (30<y+<500).
=
=󰇡
󰇢=() (2)
=
 (3)
There are two options in treating the near-
wall region in RANS simulations: One has
to either properly resolve the viscous sub-
layer or use wall functions to approximate
flow quantities within the turbulent bound-
ary layer. A proper resolution of the vis-
cous sublayer (low-y+ approach) requires
that enough cells are located within this
layer and increases discretization effort in
near-wall regions. Using wall functions
(high-y+ approach) allows a coarser mesh
and does not require a resolution of the vis-
cous sublayer. (Ferziger and Perić 2002)
show that wall functions should only be
used when near wall effects are not the pri-
mary concern as they have deficits in pre-
dicting flow separation and assume a
boundary layer profile without actually simulating these effects. The viscous sublayer can get very thin
for high Reynolds numbers, which can lead to excessive discretization effort. However, this is usually
not the case for low-speed subsonic conditions. The authors therefore recommend always resolving the
viscous sublayer and using a low y+ approach.
Most finite volume RANS codes provide specific meshing algorithms that are used to create an appro-
priate mesh in the near wall region. Typical terms are “prism layer mesher” or “thin mesher”, (Ewing
2015), (ANSYS Inc. 2019b). These types of algorithms are designed to create very thin cells close to
the wall with increased spacing in the y-direction (see Figure 7a). Multiple ways of defining the prop-
erties of a prism layer mesh exist. The most common one is to specify the height of the cell adjacent to
the wall, the total prism layer thickness, and the number of layers used to discretize the prism layer
thickness. The distribution of prism layers might follow a hyperbolic tangent function like proposed by
(Vinokur 1980). Such functions provide a better resolution of the boundary layer by providing a non-
linear cell growth rate from the wall. (Menter et al. 2015) shows that this greatly enhances the accuracy
of the boundary layer discretization. The authors recommend using such functions whenever possible.
The height of the cell adjacent to the wall depends on the chosen y+ approach. A conceptual sketch of
a low and high y+ mesh near a wall is given in Figure 7. When resolving the viscous sublayer (low-y+),
one should aim for a cell height that guarantees a y+ of the first cell in the order of one. (Menter 1994)
describes in the derivation of the SST turbulence model that its wall boundary condition requires y+< 3.
(Georgiadis et al. 1995) investigated the effects of y+ on a flat plate boundary layer and state that values
of smaller than two are required to match experimental data properly. These findings are confirmed by
(Menter et al. 2015) who additionally found that when using transition models, one should aim for a y+
that is smaller than one. In case a high-y+ with wall functions is used, one should avoid the buffer layer
Figure 6. Velocity in the near wall region, experimental
data from
(Schlichting and Gersten 2017)
0
5
10
15
20
25
0.1 1 10 100 1000
u+
log (y+)
u+ experiments
u+=y+
u+=1/κ ln(Ey+)
viscous sublayer
buffer layer
log law layer

and roughly aim for 30<y+<300, (Ewing 2015). The actual y+ values used in the simulation can only be
analyzed after the solution has converged. Before meshing, one needs to estimate an appropriate cell
height that will result in the desired y+. An estimation is conveniently possible by applying flat-plate
boundary layer theory. The computations involve calculating the length-based Reynolds number, an
empirical skin friction coefficient, and the wall shear stress. The relevant equations are shown below
with Δs being the first cell height (White 2011).
=
 =.


 =

  =

 (4-7)
It is crucial to do this estimation for each aircraft component individually, as different reference lengths
(e.g. wing chord vs. fuselage length) lead to different Reynolds numbers and therefore different cell
heights. The total prism layer thickness should cover the complete boundary layer. The boundary
layer’s thickness is, again, only available with the final solution and needs to be estimated for initial
meshing. An appropriate way is to use an empirical correlation for a fully turbulent flat plate boundary
layer, see Eq. (8). The authors advise to increase the result of Eq. (8) by a safety factor of 1.5, as it does
not account for any 3D effects. Again, this computation must be performed for every aircraft compo-
nent. The boundary between prism layer- and volume mesh should be smooth and cell sizes should not
vary too much. This sometimes requires an adjustment of the prim layer mesh thickness.
=.

. (8)
The total number of layers must be large enough to ensure a sufficient discretization of the boundary
layer. It is common to either directly specify the number of layers or to provide a stretching factor in
wall-normal direction. In case the number of layers is specified, their distribution can be defined by
recalculating a stretching ratio starting from the
first grid cell. (Menter et al. 2015) find that 30 cell
layers discretizing the boundary layer are suffi-
cient even for transition models that require an ex-
tra-fine resolution. Numerous test cases of the
authors have shown that one can expect to use be-
tween 20-40 prism layers to discretize the near
wall region. The stretching ratio for such num-
bers is commonly between 1.05 and 1.2. This is
confirmed by analyses of (Moshfeghi et al. 2012)
and best practices guides found in (Siemens PLM
Software 2019) and (ANSYS Inc. 2019b).
PHYSICS AND SOLVERS
The following paragraphs give a very brief overview about relevant physical settings that can affect the
simulation and its numerical stability. The descriptions and recommendations are kept in a general
manner to make them applicable, considering most RANS CFD codes. Individual codes might use
slightly different notation and terms for specific aspects. The authors advise the reader to refer to the
user guides of the respective software for further reading.
Boundary Conditions
The physical simulation setup has to represent the desired flight conditions that should be analyzed.
Flow properties like freestream pressure, temperature, density, velocity, and flow orientation have to
appropriately account for this. A more complex problem is the determination of adequate turbulence
quantities. Most turbulence models require the specification of a turbulence intensity and a viscosity
ratio. It is also common to prescribe a turbulence length scale instead of a viscosity ratio. These values
are then used to compute the transported variables at the freestream boundary. Atmospheric freestream
simulations have very small turbulence intensities often in the order of 0.1%. This is desirable as ex-
periments show that values below this do not alter the laminar-turbulent transition location anymore
(Young 1989). The turbulent viscosity ratio at boundary conditions is usually between unity and ten
a)
b)
Figure 7. Sketch of a near-wall mesh using a)
low-y+ and b) high-y+
approach. Green dots indi-
cate cell centers of the cell adjacent to the wall.

(ANSYS Inc. 2019b) for external aerodynamic flows. Such recommendation are also specific to the
chosen turbulence model and further information can be found in the relevant literature, see for example
(Spalart and Rumsey 2007) or (Menter 1994).
Temporal discretization
In CFD, flows can be handled as either steady or unsteady. The appropriate choice depends on the flow
regime and the geometry. If it is expected, that the flow solution does not change with time, the steady
approach should be chosen. This is often the case for streamlined bodies that are not affected by sepa-
ration (Thwaites 1987). If the flow solution is expected to change with time, one needs to treat the flow
as unsteady. Aircraft simulations may require an unsteady approach if oscillations in the wake of blunt
bodies (e.g. landing gear) occur. Another prominent factor requiring an unsteady solution is flow sep-
aration. The authors recommend choosing the steady-state approach in any case where flow properties
and geometry allow doing so. A steady-state solution typically allows much faster turnaround times
compared to unsteady ones (Ferziger and Perić 2002). If unsteady flow behavior is observed during a
steady-state solution, one can switch to the unsteady flow model and use the already computed solution
as an initialization for the unsteady solver. This reduces overall computational time. The choice of
time-step is critical for any unsteady flow solution, both in terms of physical representation and stability.
For wake shedding, one must ensure a sufficient number of time steps per oscillation period. The authors
recommend using at least 50 time-steps per oscillation due to their experience with unsteady flows in
aircraft aerodynamics. The oscillation frequency might be estimated based on the Strouhal number of
similar components, see (White 2011). Implicit time integration schemes should be preferred as they
can tolerate higher time-steps which is usually advantageous in general aircraft aerodynamics, see
(Blazek 2004).
Solvers
Two solver types are commonly integrated into most CFD packages. A density-based solver and a
pressure-based solver. Due to their nature, they are often called a coupled solver and a segregated solver
respectively.
Coupled Flow Solver
The coupled (density-based) solver solves the conservation equations coupled and simultaneously. The
velocity field is derived from the momentum equations, while the continuity equation is used to obtain
the pressure. Density is evaluated from the equation of state. A good description of this solver type,
especially for unstructured meshes, can be found in (Demirdžić and Muzaferija 1995). The solver is
suited for any flow regime, however, becomes inefficient at low Mach numbers. With flows being
almost incompressible, the speed of sound increases sharply. This requires an appropriate reduction in
time-step to fulfill stability criterions. It is advisable to avoid the density-based solver in low-speed
aircraft aerodynamic simulations, due to this drawback.
Segregated Flow Solver
The segregated (pressure-based) flow solver solves the conservation equations decoupled in sequential
order. It is based on the derivation of a pressure correction equation. An intermediate velocity field is
computed by first solving the momentum equations only. This is used to solve the pressure correction
equation and to update both the pressure and velocity field. A further description of the algorithm for
unstructured meshes can be found in (Mathur and Murthy 1997). The pressure-based solver has its
origins in purely incompressible flows, as it does not suffer from the particular disadvantage of the
coupled flow solver in this regime (see above). A widely-used algorithm is the Semi-Implicit Method
for Pressure-Linked Equations (SIMPLE) originally derived by (Caretto et al. 1973). It was further
developed multiple times (see e.g. (Patankar 1980) and (van Doormaal and Raithby 1984)) and has seen
extensive use in almost all commercial and non-commercial CFD codes. Modified versions can handle
compressible flows as well. However, the coupled flow solver is described to have advantages in cap-
turing shock waves (ANSYS Inc. 2019b). For low-speed aircraft aerodynamics, the pressure-based flow
solver is highly recommended by the authors. It usually leads to much shorter turnaround times com-
pared to the coupled flow solver. A further advantage is its 1.5-2.0 times lower memory consumption.

The SIMPLE algorithm can get unstable if
flow properties change too much from one
iteration step to another. Pressure and veloc-
ity changes are therefore restricted by multi-
plying their newly found values with under-
relaxation factors for each iteration step.
Depending on the specific type of SIMPLE
algorithm, different values might be appro-
priate. The authors have found that under-
relaxing pressure with a factor of 0.3 and ve-
locity with 0.7 usually leads to converged
solutions in steady-state aircraft aerody-
namic simulations. The recommended val-
ues are chosen as a compromise between
solution stability and convergence perfor-
mance. They are conservative in most cases.
Simple geometries often allow a slight in-
crease in both factors. Transient simulations tolerate higher values as the transient term introduces ad-
ditional stability. Turbulent variables allow high under-relaxation factors in the order of 0.8-1.0.
Under-relaxation factors can have a significant effect on convergence behavior. Higher under-relaxation
factors lead to faster convergence. In such, it is desirable to find optimal factors for individual problems.
Figure 8 shows the convergence behavior of a representative 2D airfoil simulation at different levels of
under-relaxation factors using the code StarCCM+. The simulations are stopped when the lift-to-drag
ratio has reached an asymptotic goal that is kept constant for all simulations. This specific simulation
allows increasing the under-relaxation factors beyond the recommended ones (0.7/0.3) and shows the
fastest convergence using a factor of 0.8 to under-relax velocity and 0.4 to under-relax pressure. In-
creasing them further leads to divergence. The recommended values are conservative and increase sim-
ulation time by about 15% compared to the optimum under-relaxation factors. This conservatism can
be useful in simulation studies with various inflow conditions or geometries. The optimum under-re-
laxation factors are usually on the edge of stability. There is no guarantee that the optimum under-
relaxation factors for one specific case do lead to a converged solution in another similar one. In such,
having a slight stability margin can be extremely helpful.
It is sometimes possible to increase one under-relaxation factor further while keeping the other one
constant. In the example shown in Figure 8, the pressure under-relaxation factor can be increased be-
yond 0.4 when the velocity factor is limited to 0.7. This does not reduce turnaround times for the given
example. In this specific case, the velocity under-relaxation has a more profound effect on turnaround
time than the pressure one. However, it was not possible to increase the velocity under-relaxation factor
beyond 0.8 without experiencing divergence.
If divergence occurs within the first iterations, the authors recommend ramping-up the under-relaxation
factors from very small values at the beginning to their desired values over 10-100 iterations. This
damps initial oscillations and often avoids initial divergence.
TURBULENCE MODELLING
Turbulence modelling is an integral part of today’s computational fluid dynamics approach in full-scale
aircraft aerodynamic simulations. Scale resolving approaches are too time-consuming for complete air-
craft simulations and will remain so in the near future. (Spalart 2000) estimates that large eddy simula-
tions of full aircraft configurations will be theoretically possible in 2045. This refers to the pure
possibility in terms of computational resources. Industrial use will come much later. Until then, engi-
neers will rely on models to predict turbulence quantities. Turbulence modelling is a complex problem
and can substantially alter flow predictions and overall simulation results. It is an intense area of re-
search and far too complex to be comprehensively addressed here. This paragraph, therefore, only gives
a short and general outline of the turbulence modelling approach and introduces the most common mod-
elling families that are relevant for low-speed aerodynamic flows.
Figure 8. Effect of under-relaxation factors on the
convergence
behavior of a 2D airfoil analysis
0
1000
2000
3000
4000
5000
0.4/0.1 0.6/0.2 0.7/0.3 0.8/0.4 0.7/0.5 0.8/0.2
Iteration number for convergence
Under-relaxation factors for velocity / pressure

The RANS equations are derived by decomposing the instantaneous flow variables into an averaged
part and a fluctuating part. This averaging is often referred to as Reynolds averaging and exemplarily
depicted for a flow variable

in Eq. (9). Introducing this averaging into the momentum transport
equation yields Eq. (10), neglecting body forces.
=
+󰆒 (9)

(
)+(

)= +(+󰆒) (10)
The last term in Eq. (10) is the fluctuating stress tensor
T’
that needs to be modelled with a turbulence
model. The most common approach for this is using an eddy viscosity model. These models aim to
represent the transfer of momentum caused by turbulent eddies as an artificial viscosity, frequently
called the eddy viscosity or turbulent viscosity μt. The fluctuating stress tensor can then be calculated
using a constitutive relation like the linear Boussinesq approximation shown in Eq. (11).
󰆒= 2
(
) (11)
(Spalart 2000) and (Hellsten 2005) proposed using quadratic or cubic relationships in the Boussinesq
approximation, which significantly enhances the prediction accuracy of anisotropy of turbulence. A test
case showing the enormous accuracy increase is presented later on.
Numerous different models for estimating the turbulent viscosity have been developed in the past. The
conventional approach is to add one or more transport equations that are discretized and solved together
with the Navier-Stokes equations. They are then used to calculate the turbulent viscosity in each cell of
the flow field. The three most common families of turbulence models that are used in aerodynamic
calculations are outlined below:
Spalart-Allmaras one-equation model
The Spalart-Allmaras (S-A) one-equation model was initially derived by (Spalart and Allmaras 1992)
and solves one additional transport equation that is used to determine the turbulent viscosity. It comes
at a relatively low computational cost, as only one additional equation must be solved. The model is a
low-Reynolds number model and therefore requires an appropriate discretization of the viscous sub-
layer. It has been widely used in the aerospace community and was revised and extended multiple times
by different researchers (e.g. (Edwards and Chandra 1996) or (Shur et al. 2000)). It has shown good
accuracy for attached quasi 2D flows but has problems with 3D flows, including strong separation or
free shear flow (Wilcox 2010). It is best suited for mildly complex problems, including attached flows
over wings or fuselages (ANSYS Inc. 2006).
k-ε model family
The first version of the k-ε turbulence model was presented by (Jones and Launder 1972). It was orig-
inally designed as a high Reynolds number model that uses wall functions for the viscous sublayer. Two
additional transport equations are solved, one for the turbulent kinetic energy k and one for the eddy
dissipation rate ε. Numerous authors further improved the model, and it became one of the most recog-
nized industrial turbulence models. (Rodi 1991) developed a two-layer approach that allows for a direct
discretization of the viscous sub-layer without using wall functions. Today it is most widely used with
the “realizable” modification from (Shih et al. 1994) that contains a new transport equation for the eddy
dissipation rate. Its use of wall functions made it initially not very popular in the aerospace industry
although the model variant developed by (Shih et al. 1994) is described to handle boundary layer sepa-
ration and vortex shedding behind bluff bodies (ANSYS Inc. 2006).
k-ω model family and Menter’s Shear Stress Transport model
The original k-ω model was derived by (Wilcox 1988) and is a well-recognized turbulence model in the
field of aerodynamics. It was revised numerous times and is comprehensively described in (Wilcox
2010). The model uses the specific eddy dissipation rate (eddy dissipation rate per unit of turbulent
kinetic energy) instead of the dissipation rate as the second variable. It can be used throughout the
viscous sublayer (low y+ approach) without modification and has shown superior performance in bound-
ary layer flows with adverse pressure gradient and separation (Wilcox 2010), (ANSYS Inc. 2006).

Boundary layer computations with the original model showed high sensitivity to the specific eddy dis-
sipation rate of the freestream. This, in turn, made boundary layer computations very sensitive to
freestream boundary conditions. Such a problem does not occur in k-ε models. (Menter 1994) addressed
this by effectively using the k-ε approach in the far field and the k-ω formulation close to walls in his
Shear Stress Transport (SST) turbulence model. This combines the advantages of a k-ω formulation in
the boundary layer with the insensitivity to turbulence boundary conditions in the k-ε formulation. The
SST model has become very popular for aerodynamic flows and is widely used for aircraft simulations
(Menter et al. 2003), (Frink 2006).
The authors have extensive experience using this model and found it accurate for predicting full aircraft
aerodynamics as well as bluff body flows (Götten et al. 2018b) and (Götten et al. 2019b). The authors
recommend using the SST model whenever one deals with boundary layer flow in adverse pressure
gradient (typical for airfoils/wings). The original SST model was revised multiple times by different
authors (e.g. (Hellsten 1998), (Smirnov and Menter 2009)) in order to improve its accuracy for various
applications.
Recent developments are the local correlation based γ-Reθ transition model (Menter et al. 2006) and the
γ-transition model (Menter et al. 2015) that are coupled with the SST model. These sub-models allow
simulating transition effects, including laminar separation bubbles at low Reynolds numbers (Langtry
et al. 2006). The authors have validated the γ-Reθ model for numerous airfoils in a recent publication
and recommend using it in aerodynamic simulations, see (Götten et al. 2019a).
Improvements to the classic turbulence modelling approach
The following section gives an overview about two critical modifications of classic turbulence models
and their effect on the flow solution. These modifications are universal and can principally be applied
to all described models. They do not include individual corrections developed to overcome specific
disadvantages of one or the other model. The additions and modifications are shown in the context of
the SST model.
Non-linear constitutive relations
The constitutive relation describes the process in which the turbulent viscosity determined by the re-
spective turbulence model is transferred into the fluctuating stress tensor. The classic approach is to use
the linear Boussinesq approximation. This linear relationship is known to under-predict the effects of
anisotropy of turbulence (Spalart 2000). Using non-linear constitutive relations can significantly in-
crease prediction accuracy.
Figure 9. V-velocity profiles of NACA 4412 at 14° angle of attack and Re= 1.52x106 - computed
with SST turbulence model, experimental data from (Coles and Wadcock 1979)
-0.20 -0.15 -0.10 -0.05 0.00 0.05 0.10
0.00
0.05
0.10
0.15
0.20
0.25
0.30
0.00
0.05
0.10
0.15
0.20
0.25
0.30
-0.20 -0.15 -0.10 -0.05 0.00 0.05 0.10
y [m]
v/uref
x/c=0.675 Coles & Wadcock
x/c=0.675 linear
x/c=0.675 quadratic
x/c=0.675 cubic
x/c=0.897 Coles & Wadcock
x/c=0.897 linear
x/c=0.897 quadratic
x/c=0.897 cubic

(Spalart 2000) proposed a quadratic relationship that involves the local strain rate tensor and the rotation
tensor. Both tensors are used to define a new non-linear fluctuating stress tensor that is added to the one
determined from the Boussinesq approximation. (Hellsten 2005) proposed a cubic relationship that is
essentially derived from an explicit algebraic Reynolds stress model proposed by (Wallin and Johansson
2000). Figure 9 shows the significant effect of non-linear constitutive relations on velocity profiles
normal to the surface of a NACA 4412. The computations are performed in 2D using the SST turbulence
model. The experimental data is taken from (Coles and Wadcock 1979). Both quadratic and cubic
constitutive relationship significantly increase the accuracy compared to the linear relationship. The
cubic constitutive relation gives results that are very close to the experimentally found values. The
authors found the computational overhead well manageable and recommend using non-linear constitu-
tive relationships whenever possible. However, the authors have also noted some numerical stability
issues with the cubic constitutive option. It was found that the cubic relationship is very sensitive to cell
quality, which can be critical, especially at sharp trailing edges. In such cases, the authors recommend
solving the flow with a quadratic relationship first and using this as an initial condition for the solution
with the cubic constitutive relationship.
Controlled turbulence decay
A central problem with freestream aerodynamic simulations is the fact that turbulence variables speci-
fied on the freestream boundary conditions numerically decay. This numerical decay is dependent on
the individual flow problem and the spatial discretization. The aircraft body located in the center of the
flow domain can experience different turbulent freestream values than specified by the user at the bound-
ary conditions. The problem was comprehensively described by (Spalart and Rumsey 2007). They
propose the introduction of additional terms in turbulence models that effectively cancel the destructive
terms in the freestream. The effects of the new terms in the boundary layer are usually negligible. The
modification is termed “controlled decay”. An example simulation showing the effect of turbulence
decay and the corresponding controlled decay with the SST model is presented in Figure 10. An empty
bullet-shaped flow domain is discre-
tized with hexahedral cells of uni-
form size. The initial conditions for
all cells correspond to the boundary
conditions. No variable should
change within the flow field as no
body disturbs the flow. Neverthe-
less, both turbulent kinetic energy
and turbulent viscosity ratio decay
over the length of the flow domain.
The aircraft body would be situated
in the center. At this location, the
turbulent kinetic energy in the
freestream is only about one-fifth of
the value specified at the boundary.
The turbulent viscosity ratio has de-
cayed by about 12%. The controlled
decay keeps both turbulence varia-
bles constant. Using this option is
recommended for any aerodynamic
analysis case.
CONVERGENCE AND PLAUSIBILITY
Convergence in RANS simulations is often judged by analyzing the solutions’ residuals. A residual
represents the absolute error in the solution of a flow variable. In perfectly converged solutions, the
residuals would approach the round-off error of float or double variables. Most codes show a residual
plot with only one residual per transport variable for the complete simulation domain. This is obtained
by averaging the respective residual of all cells. A solution is often termed converged when the residuals
Figure 10. Turbulence variables along the centerline of an
empty flow domain
- computed with SST turbulence model
0.0 0.2 0.4 0.6 0.8 1.0
1.0
1.2
1.4
1.6
1.8
2.0
2.2
2.4
0.0
0.2
0.4
0.6
0.8
1.0
1.2
1.4
0.0 0.2 0.4 0.6 0.8 1.0
μt/μ
k x1000 [J/kg]
Normalised flowfield length
k - controlled decay off k - controlled decay on
μt/μ -controlled decay off μt/μ -controlled decay on
typical location
of aircraft model

do reach an asymptotic minimum. An exemplary
residual plot of a 2D analysis is given in Fig-
ure 11. Several CFD codes normalize the residu-
als to the first iterations as their absolute value can
vary significantly. The amount of residual de-
crease depends on the individual problem and the
normalization approach, see (Ferziger and Perić
2002). Due to this, no general statement of re-
quired residual decrease is possible. In aircraft
aerodynamic simulations, it is therefore recom-
mended to monitor integrated parameters like lift,
drag or moment. In steady simulations, one can
expect that these values converge asymptotically.
As with mesh independence studies, it is essential
to examine the convergence behavior of each air-
craft component individually.
Once a simulation is converged, it should be checked for plausibility. The authors find the following
investigations useful and recommend using them as a routine baseline for plausibility analyses.
1. Disable any cell interpolation of scalar variables when analyzing visualizations. Interpolations can
often purport an appropriate discretization, as changes between cells seem artificially smooth.
2. Visualize the y+ distribution around all bodies and check that all cells have appropriate values.
3. Visualize the pressure distribution around all bodies. Validate that they match expectations (e.g.
reduced pressure and higher velocities around curved surfaces).
4. Visualize the velocity near the body. Check that flow disturbances that are associated with the
aircraft’s body diminish smoothly further away from the body. Sudden changes that are associated
with mesh coarsening usually indicate inappropriate discretization.
5. Check the location of stagnation conditions as well as stagnation pressure and velocity. A non-zero
stagnation velocity is an indication for poor discretization.
6. Check the propagation of wake regions. The wake region should mix with the surrounding
smoothly. Any sudden changes associated with a coarsening mesh might indicate inappropriate
discretization.
7. Visualize vectors of the wall shear stress on the aircraft’s body. This gives a representation of the
flow direction very close to the surface. Validate that the flow direction is as expected and that
separation occurs at meaningful locations.
CONCLUSION
This paper reviewed and summarized existing guidelines and best practices for low-speed aerodynamic
simulations using RANS CFD methods. It showed the importance of an adequate preparation of the
CAD geometry as well as the most popular approaches to transfer this geometry in the CFD domain.
An overview about common cell types and associated meshing algorithms gives indications on how cell
types can affect solution convergence and turnaround time. Several recommendations for an appropriate
surface and volume discretization are presented. These recommendations allow generating an adequate
mesh for most geometries that is then ready for further optimization. The importance of wall treatment
in RANS simulations is highlighted, and guidance in creating an adequate boundary layer mesh is pro-
vided. Both the choice of temporal discretization and solver type are briefly explained with a focus on
pressure-based solvers and an adequate setting of under-relaxation factors. Turbulence modelling is
presented as an integral part of today’s numerical flow simulation, and the most common models for
aerodynamic simulations are outlined. The paper further highlights the effects of non-linear constitutive
relations and shows how this modification can significantly increase the prediction accuracy of turbu-
lence models. Several methods for judging convergence an analyzing the plausibility of the solution
complete the paper.
Figure 11. Normalized residual plot
1.E-09
1.E-08
1.E-07
1.E-06
1.E-05
1.E-04
1.E-03
1.E-02
1.E-01
1.E+00
0 500 1000 1500 2000
Residual
Iteration
Continuity
X-momentum
Y-momentum
TKE
SDR

Reference List
ANSYS Inc. (2006), “Modeling Turbulent Flows. Introductory FLUENT Training”, available at:
<http://www.southampton.ac.uk/~nwb/lectures/GoodPracticeCFD/Articles/Turbulence_Notes_Flu
ent-v6.3.06.pdf> (accessed 14 June 2019).
ANSYS Inc. (2019a), CFX Documentation, Canonsburg Pennsylvania.
ANSYS Inc. (2019b), Fluent Documentation, Canonsburg Pennsylvania.
Blazek, J. (2004), Computational fluid dynamics: Principles and applications, 1st ed., Elsevier,
Amsterdam, 0080430090.
Caretto, L.S., Gosman, A.D., Patankar, S.V. and Spalding, D.B. (1973), “Two calculation procedures
for steady, three-dimensional flows with recirculation”, in Proceedings of the Third International
Conference on Numerical Methods in Fluid Mechanics, Lecture Notes in Physics, 19th ed.,
Springer, Berlin, 10.1007/BFb0112677.
Coles, D. and Wadcock, A.J. (1979), “Flying-Hot-wire Study of Flow Past an NACA 4412 Airfoil at
Maximum Lift”, AIAA Journal, Vol. 17 No. 4, pp. 321–329, 10.2514/3.61127.
Demirdžić, I. and Muzaferija, S. (1995), “Numerical method for coupled fluid flow, heat transfer and
stress analysis using unstructured moving meshes with cells of arbitrary topology”, Computer
Methods in Applied Mechanics and Engineering, Vol. 125 1-4, pp. 235–255, 10.1016/0045-
7825(95)00800-G.
Edwards, J.R. and Chandra, S. (1996), “Comparison of eddy viscosity-transport turbulence models for
three-dimensional, shock-separated flowfields”, AIAA Journal, Vol. 34 No. 4, pp. 756–763,
10.2514/3.13137.
Ewing, P. (2015), “Best Practices for Aerospace Aerodynamics”, in Star South East Asian Conference
2015, Singapore.
Ferziger, J.H. and Perić, M. (2002), Computational Methods for Fluid Dynamics, 3rd ed., Springer,
Berlin, 3-540-42074-6.
Finger, D.F., Götten, F., Braun, C. and Bil, C. (2018), “Initial Sizing for a Family of Hybrid-Electric
VTOL General Aviation Aircraft”, in German Aerospace Congress 2018, Bonn,
10.25967/480102.
Fluidyn (2019), Fluidyn Documentation, St Denis.
Frink, N.T. (2006), 3rd AIAA CFD Drag Prediction Workshop: 2-Day Workshop Preceeding the 25th
APA Conference, Reston ,VA, available at: <https://aiaa-
dpw.larc.nasa.gov/Workshop3/workshop3.html>.
Georgiadis, N.J., Dudek, J.C. and Tierney, T.P. (1995), “Grid Resolution and Turbulent Inflow
Boundary Condition Recommendations for NPARC Calculations. NASA-TM 106959”, in AIAA,
ASME, SAE, ASEE (Ed.), 31st Joint Propulsion Conference and Exhibit, Langley Field, VA,
10.2514/6.1995-2613.
Gloudemans, J., Davis, P. and Gelhausen, P. (1996), “A rapid geometry modeler for conceptual
aircraft”, in 34th Aerospace Sciences Meeting and Exhibit, Reno,NV,U.S.A, AIAA, Reston, VA,
10.2514/6.1996-52.
Götten, F., Finger, D.F., Havermann, M., Braun, C., Gómez, F. and Bil, C. (2018a), “On the Flight
Performance Impact of Landing Gear Drag Reduction Methods for Unmanned Air Vehicles”, in
German Aerospace Congress 2018, Bonn, 10.25967/480058.
Götten, F., Finger, D.F., Havermann, M., Marino, M. and Bil, C. (2019a), “A highly automated
method for simulating airfoil characteristics at low Reynolds number using a RANS - transition
approach”, in German Aerospace Congress 2019, Darmstadt, Germany.
Götten, F., Havermann, M., Braun, C., Gómez, F. and Bil, C. (2018b), “On the Applicability of
Empirical Drag Estimation Methods for Unmanned Air Vehicle Design”, in 18th AIAA Aviation

Technology Integration and Operations Conference, Atlanta, AIAA, Reston ,VA, 10.2514/6.2018-
3192.
Götten, F., Havermann, M., Braun, C., Gómez, F. and Bil, C. (2019b), “RANS Simulation Validation
of a Small Sensor Turret for UAVs”, Journal of Aerospace Engineering, Vol. 32 No. 5, p.
4019060, 10.1061/(ASCE)AS.1943-5525.0001055.
Haase, W., Bradsma, R., Elsholz, E., Leschziner, M. and Schwamborn, D. (1992), Notes on Numerical
Fluid Mechanics Volume 42: EUROVAL - An European Initiative on Validation of CFD Codes,
Brussels.
Hartmann, R. and Houston, P. (2009), “Error estimation and adaptive mesh refinement for
aerodynamic flows”, in Proceedings of the 36THCFD/Adigma course on HP-adaptive and HP-
multigrid methods, Belgium, 10.1007/978-3-642-03707-8_24.
Hellsten, A. (1998), “Some Improvements in Menter's k-w SST Turbulence Model”, in 29th AIAA
Fluid Dynamics Conference, AIAA, Reston ,VA, 10.2514/6.1998-2554.
Hellsten, A.K. (2005), “New Advanced k-w Turbulence Model for High-Lift Aerodynamics”, AIAA
Journal, Vol. 43 No. 9, pp. 1857–1869, 10.2514/1.13754.
Hirsch, C. (2002), Computational methods for inviscid and viscous flows, Wiley series in numerical
methods in engineering, Reprinted., Wiley, Chichester, 0471924520.
ISO 10303-21 (1994), STEP-file - Industrial automation systems and integration - Product data
representation and exchange - Part 21: Implementation methods: Clear text encoding of the
exchange structure 10303-21, available at: <https://www.iso.org/standard/63141.html>.
Jones, W.P. and Launder, B.E. (1972), “The prediction of laminarization with a two-equation model of
turbulence”, International Journal of Heat and Mass Transfer, Vol. 15 No. 2, pp. 301–314,
10.1016/0017-9310(72)90076-2.
Kai, C.C., Jacob, G.G.K. and Mei, T. (1997), “Interface between CAD and Rapid Prototyping systems.
Part 2”, The International Journal of Advanced Manufacturing Technology, Vol. 13 No. 8, pp.
571–576, 10.1007/BF01176301.
Lanfrit, M. (2005), Best practice guidelines for handling Automotive External Aerodynamics with
FLUENT, Darmstadt, Germany, available at:
<https://www.southampton.ac.uk/~nwb/lectures/GoodPracticeCFD/Articles/Ext_Aero_Best_Pract
ice_Ver1_2.pdf> (accessed 3 June 2019).
Langtry, R.B., Menter, F.R., Likki, S.R., Suzen, Y.B., Huang, P.G. and Völker, S. (2006), “A
Correlation-Based Transition Model Using Local Variables—Part II. Test Cases and Industrial
Applications”, Journal of Turbomachinery, Vol. 128 No. 3, p. 423, 10.1115/1.2184353.
Mathur, S.R. and Murthy, J.Y. (1997), “A Pressure-Based Method for Unstructured Meshes”,
Numerical Heat Transfer, Part B: Fundamentals, Vol. 31 No. 2, pp. 195–215,
10.1080/10407799708915105.
Mavriplis, D.J., Vassberg, J.C., Tinoco, E.N., Mani, M., Brodersen, O.P., Eisfeld, B., Wahls, R.A.,
Morrison, J.H., Zickuhr, T., Levy, D. and Murayama, M. (2009), “Grid Quality and Resolution
Issues from the Drag Prediction Workshop Series”, Journal of Aircraft, Vol. 46 No. 3, pp. 935–
950, 10.2514/1.39201.
Menter, F.R. (1994), “Two-equation eddy-viscosity turbulence models for engineering applications”,
AIAA Journal, Vol. 32 No. 8, pp. 1598–1605, 10.2514/3.12149.
Menter, F.R., Kuntz, M. and Langtry, R. (2003), “Ten Years of Industrial Experience with the SST
Turbulence Model”, in Turbulence, Heat and Mass Transfer 4: Proceedings of the Fourth
International Symposium, Heat and Mass Transfer, Begell House, Inc, New York.

Menter, F.R., Langtry, R.B., Likki, S.R., Suzen, Y.B., Huang, P.G. and Völker, S. (2006), “A
Correlation-Based Transition Model Using Local Variables—Part I. Model Formulation”, Journal
of Turbomachinery, Vol. 128 No. 3, p. 413, 10.1115/1.2184352.
Menter, F.R., Smirnov, P.E., Liu, T. and Avancha, R. (2015), “A One-Equation Local Correlation-
Based Transition Model”, Flow, Turbulence and Combustion, Vol. 95 No. 4, pp. 583–619,
10.1007/s10494-015-9622-4.
Moshfeghi, M., Song, Y.J. and Xie, Y.H. (2012), “Effects of near-wall grid spacing on SST-K-ω
model using NREL Phase VI horizontal axis wind turbine”, Journal of Wind Engineering and
Industrial Aerodynamics, 107-108, pp. 94–105, 10.1016/j.jweia.2012.03.032.
Moukalled, F., Mangani, L. and Darwish, M. (2016), The Finite Volume Method in Computational
Fluid Dynamics: An Advanced Introduction with OpenFOAM® and Matlab, Fluid Mechanics and
its Applications, Vol. 113, 1st ed. 2016, Springer International Publishing, Cham, 978-3-319-
16873-9.
Nagel, R.N., Braithwaite, W.W. and Kennicott, P.R. (1980), Initial Graphics Exchange Specifications
ICES Version 1.0, available at: <https://nvlpubs.nist.gov/nistpubs/Legacy/IR/nbsir80-1978.pdf>
(accessed 1 July 2019).
OpenFOAM (2010), OpenFOAM Guide Finite Volume Method, available at:
<https://openfoamwiki.net/index.php/OpenFOAM_guide/Finite_volume_method_(OpenFOAM)>
(accessed 4 June 2019).
Patankar, S.V. (1980), Numerical heat transfer and fluid flow, Series in computational methods in
mechanics and thermal sciences, Hemisphere Publ. Co, New York, 0-89116-522-3.
Perić, M. and Ferguson, S. (2005), The advantage of polyhedral meshes, available at:
<https://pdfs.semanticscholar.org/51ae/90047ab44f53849196878bfec4232b291d1c.pdf>.
Rodi, W. (1991), “Experience with Two-Layer Models Combining the k-epsilon Model with a One-
Equation Model Near the Wall”, in 29th Aerospace Sciences Meeting, Reston ,VA.
Rumsey, C. (2014), “Turbulence Modeling Resource 2D NACA 0012 Airfoil Validation Case. Effect
of Farfield Boundary”, available at:
<https://turbmodels.larc.nasa.gov/naca0012_val_ffeffect.html> (accessed 4 June 2019).
Schlichting, H. and Gersten, K. (2017), Boundary-Layer Theory, 9th ed. 2017, Springer Berlin
Heidelberg, Berlin, Heidelberg, s.l., 9783662529195.
Shih, T.-H., Liou, W.W., Shabbir, A., Yang, Z. and Zhu, J. (1994), A New k-epsilon Eddy Viscosity
Model for High Reynolds Number Turbulent Flows-Model Development and Validation: NASA-
TM-106721, Cleveland, Ohio.
Shur, M.L., Strelets, M.K., Travin, A.K. and Spalart, P.R. (2000), “Turbulence Modeling in Rotating
and Curved Channels. Assessing the Spalart-Shur Correction”, AIAA Journal, Vol. 38 No. 5, pp.
784–792, 10.2514/2.1058.
Siemens PLM Software (2019), StarCCM+ Documentation, Plano, Texas.
Smirnov, P.E. and Menter, F.R. (2009), “Sensitization of the SST Turbulence Model to Rotation and
Curvature by Applying the Spalart–Shur Correction Term”, Journal of Turbomachinery, Vol. 131
No. 4, p. 41010, 10.1115/1.3070573.
Sosnowski, M., Krzywanski, J., Gnatowska, R., Suwała, W., Dudek, M., Leszczyński, J. and Łopata,
S. (2017), “Polyhedral meshing as an innovative approach to computational domain discretization
of a cyclone in a fluidized bed CLC unit”, E3S Web of Conferences, Vol. 14 No. 2, p. 1027,
10.1051/e3sconf/20171401027.
Spalart, P.R. (2000), “Strategies for turbulence modelling and simulations”, International Journal of
Heat and Fluid Flow, Vol. 21 No. 3, pp. 252–263, 10.1016/S0142-727X(00)00007-2.

Spalart, P.R. and Allmaras, S.R. (1992), “A One-Equation Turbulence Model For Aerodynamic
Flows”, in 30th Aerospace Sciences Meeting and Exhibit, Reston ,VA, 10.2514/6.1992-439.
Spalart, P.R. and Rumsey, C.L. (2007), “Effective Inflow Conditions for Turbulence Models in
Aerodynamic Calculations”, AIAA Journal, Vol. 45 No. 10, pp. 2544–2553, 10.2514/1.29373.
Thwaites, B. (Ed.) (1987), Incompressible aerodynamics: An account of the theory and observation of
the steady flow of incompressible fluid past aerofoils, wings, and other bodies, Fluid motion
memoirs, Dover, New York.
van Doormaal, J.P. and Raithby, G.D. (1984), “Enhancements of the SIMPLE Method for Predicting
Incompressible Fluid Flows”, Numerical Heat Transfer, Vol. 7 No. 2, pp. 147–163,
10.1080/01495728408961817.
Versteeg, H.K. and Malalasekera, W. (2007), An introduction to computational fluid dynamics: The
finite volume method, 2nd ed., Pearson/Prentice Hall, Harlow, 978-0-13-127498-3.
Vinokur, M. (1980), On One-Dimensional Stretching Functions for Finite-Difference Caluclations:
NASA-CR-3313, available at:
<https://ntrs.nasa.gov/archive/nasa/casi.ntrs.nasa.gov/19800025680.pdf> (accessed 1 July 2019).
Wallin, S. and Johansson, A.V. (2000), “An explicit algebraic Reynolds stress model for
incompressible and compressible turbulent flows”, Journal of Fluid Mechanics, Vol. 403, pp. 89–
132, 10.1017/S0022112099007004.
White, F.M. (2011), Fluid mechanics, 7. ed., McGraw-Hill, New York, NY, 978-0-07-352934-9.
Wilcox, D.C. (1988), “Reassessment of the scale-determining equation for advanced turbulence
models”, AIAA Journal, Vol. 26 No. 11, pp. 1299–1310, 10.2514/3.10041.
Wilcox, D.C. (2010), Turbulence modeling for CFD, 3. ed., 2. print, DCW Industries, La Cañada,
Calif., 978-1-928729-08-2.
Young, A.D. (1989), Boundary Layers, AIAA education series, AIAA Education Series, Washington,
DC, 0930403576.