Design of an Overset Mesh Methodology for Forest Protection

Design of an Overset Mesh Methodology for
Forest Protection Aircraft Droplet Release
by
Daniel Fieger
BScE, University of Applied Science HS Karlsruhe, 2012
A THESIS SUBMITTED IN PARTIAL FULFILLMENT OF
THE REQUIREMENTS FOR THE DEGREE OF
Master of Science in Mechanical Engineering
In the Graduate Academic Unit of Mechanical Engineering
Supervisor:
Andrew G. Gerber, PhD, Mechanical Engineering
Examining Board: Andy Simoneau, PhD, Mechanical Engineering, Chair
Tiger Jeans, PhD, Mechanical Engineering
A. Gordon L. Holloway , PhD, Mechanical Engineering
Virendrakumar C. Bhavsar, PhD, Computer Science
This thesis is accepted by the
Dean of Graduate Studies
THE UNIVERSITY OF NEW BRUNSWICK
October, 2015
c
Daniel
Fieger, 2016
Abstract
Canada’s forests are exposed to persistent threats from insect outbreaks,
which are mitigated by pesticides (and increasingly bio-pesticides) released
from aircrafts. The trajectory of the pesticide droplets into a forest canopy
is heavily influenced by the aircraft wake and atmospheric turbulence leading to a potential for off-target drift. Off-target drifts are subject to heavy
environmental regulations, and buffer zones are required to adhere to the
regulations, which restrict the target areas. Advanced aerial operators make
use of spray drift models to predict the droplet trajectories into the canopy
in advance and compensate for drift. The models are based on simplified
analytic approaches for vortex swirling and atmospheric ground effects, and
they do not adequately predict the spray distribution or deposition. A better
evaluation of the spray droplet transport can be obtained with a full-physics
representation using Computational Fluid Dynamics. This approach can be
used to create a reliable database (relative to experiments) once proven to
improve existing real-time spray drift models. The objective of the present
work is to lay the ground work for the accomplishment of such a full-physics
ii
representation.
A full-physics CFD simulation with a single mesh is not possible without geometric changes or active mesh re-generation at each time-step due to
the movement of the aircraft relative to a complex forest canopy. A method
to resolve this issue is the use of an overset mesh, where the computational
domain consists of separate, independent, nested mesh systems that can move
relative to one another. Flow solution data is transferred between the meshes
via interpolation at shared boundaries using a donor-receiver methodology.
The implementation and demonstration of an overset methodology in the
hybrid multicore-manycore EXN/Aero CFD software is one of the main objectives of this work. Another objective is the demonstration of an aircraft
simulation. Both, the overset methodology and the knowledge gained by
the aircraft simulation will be incorporated into the broad objectives of the
research program.
iii
Table of Contents
Abstract
ii
Table of Contents
vi
List of Tables
vii
List of Figures
xiv
Abbreviations
xv
1 Introduction
1
1.1
Aerial Spraying . . . . . . . . . . . . . . . . . . . . . . . . . .
1
1.2
Objectives . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3
1.3
AGDISP System . . . . . . . . . . . . . . . . . . . . . . . . .
4
1.4
Physical Understanding and Research Motivation . . . . . . .
7
1.5
Overset Mesh Method . . . . . . . . . . . . . . . . . . . . . . 11
2 Turbulent Flow Modeling
23
2.1
Fluid Equations of Motion . . . . . . . . . . . . . . . . . . . . 24
2.2
Turbulence SST-Model . . . . . . . . . . . . . . . . . . . . . . 26
iv
3 Numerical Methods
31
3.1
Computational Solution Procedure . . . . . . . . . . . . . . . 31
3.2
EXN/Aero Software Design . . . . . . . . . . . . . . . . . . . 34
3.3
3.2.1
EXN/Aero Features
. . . . . . . . . . . . . . . . . . . 34
3.2.2
EXN/Aero Domain Decomposition . . . . . . . . . . . 35
3.2.3
Additive Correction Multi-grid Methodology . . . . . . 39
Design for Manycore Computing . . . . . . . . . . . . . . . . . 44
4 Overset Mesh Technique
47
5 Validation of EXN/Aero
62
5.1
Fluid Domain and Boundary Conditions . . . . . . . . . . . . 62
5.2
Flow Result, Verification and Validation . . . . . . . . . . . . 65
6 Single Mesh AT802 Air Tractor Study
71
6.1
Air Tractor Geometry . . . . . . . . . . . . . . . . . . . . . . 72
6.2
Fluid Domain and Boundary Conditions . . . . . . . . . . . . 73
6.3
6.2.1
Mesh Sensitivity Study . . . . . . . . . . . . . . . . . . 76
6.2.2
Mesh Topology . . . . . . . . . . . . . . . . . . . . . . 76
Flow Results and Verification . . . . . . . . . . . . . . . . . . 81
7 Testing the Overset Meshing Algorithm
7.1
92
Fluid Domain and Boundary Conditions . . . . . . . . . . . . 93
7.1.1
Mesh Topology . . . . . . . . . . . . . . . . . . . . . . 94
7.1.2
Mesh Sensitivity Study . . . . . . . . . . . . . . . . . . 95
v
7.2
Flow Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . 97
7.3
Verification and Validation . . . . . . . . . . . . . . . . . . . . 101
8 Conclusion and Future Work
106
8.1
Conclusion . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 106
8.2
Future Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . 108
A Blade Element Theory
118
A.1 Propeller Sub-domain . . . . . . . . . . . . . . . . . . . . . . . 118
A.2 Cp values at the Wing Surface . . . . . . . . . . . . . . . . . . 121
Curriculum Vitae
vi
List of Tables
2.1
Closure coefficients for turbulence SST-model . . . . . . . . . 30
5.1
Flow geometry of the backward-facing step . . . . . . . . . . . 64
5.2
Boundary conditions of the backward facing step
6.1
Boundary conditions of the computational domain . . . . . . . 75
6.2
Number and types of elements of the air tractor mesh . . . . . 79
7.1
Boundary conditions of the sliding lid computational domain . 94
7.2
Alternations of the primary vortex center location between
. . . . . . . 64
different mesh sizes . . . . . . . . . . . . . . . . . . . . . . . . 96
7.3
Alternations of the secondary vortex length between different
mesh sizes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 96
List of Figures
1.1
Air tractor AT802 depiction . . . . . . . . . . . . . . . . . . .
vii
2
1.2
Comparing full-physics CFD with low order modelling of droplet
release and transport from an AT802 aircraft. . . . . . . . . .
6
1.3
Structured, unstructured and hybrid mesh types . . . . . . . .
9
1.4
Sketch of the aerial spraying domain including the aircraft
AT802 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10
1.5
Major background mesh superimposed by a minor mesh enclosing the aircraft body . . . . . . . . . . . . . . . . . . . . . 12
1.6
Depicting arrangement of mesh systems for spray droplets released from an aircraft and a subsequent transport on to the
forest canopy . . . . . . . . . . . . . . . . . . . . . . . . . . . 13
1.7
Rectangular background mesh with a superimposed curvilinear cylindrical mesh enclosing a solid body . . . . . . . . . . . 14
1.8
Data transfer between overlapped meshes at their fringe points
and illustration of hole-points . . . . . . . . . . . . . . . . . . 15
1.9
Illustration of the Stencil walk . . . . . . . . . . . . . . . . . . 16
1.10 Data structured of an Alternating Digital Tree . . . . . . . . . 17
1.11 Air tractor AT802 and corresponding CAD model. . . . . . . . 19
3.1
Computational solution procedure including overset executions 33
3.2
Cell and interfaces of a 2D mesh . . . . . . . . . . . . . . . . . 36
3.3
Simplified background and overset mesh systems . . . . . . . . 38
3.4
Multi-grid methodology V-cycle . . . . . . . . . . . . . . . . . 40
3.5
Performance gap between CPUs and GPUs . . . . . . . . . . . 45
viii
3.6
Design differences between CPUs and GPUs . . . . . . . . . . 46
4.1
Showing two individual meshes and their overset composition . 48
4.2
Creation of individual BBs for each cell block . . . . . . . . . 49
4.3
Dividing of BBs in VSBs . . . . . . . . . . . . . . . . . . . . . 50
4.4
Hiding of VSBs that do not contain any CV centroids . . . . . 51
4.5
Segment of the overset mesh showing its fringe CVs which are
flagged as receiver nodes . . . . . . . . . . . . . . . . . . . . . 52
4.6
VSB of the donor mesh containing the CV center coordinates
of the receiver CV . . . . . . . . . . . . . . . . . . . . . . . . . 53
4.7
Control volume intersection check . . . . . . . . . . . . . . . . 54
4.8
Check if control volume encloses centroid . . . . . . . . . . . . 55
4.9
Identification of potential donors adjacent to the initial donor
node containing the receiver center point coordinates . . . . . 56
4.10 Slice through the center of mesh A with superimposed receiver
CVs of mesh B. . . . . . . . . . . . . . . . . . . . . . . . . . . 57
4.11 Slice through the center of mesh B with superimposed receiver
CVs of mesh A. . . . . . . . . . . . . . . . . . . . . . . . . . . 58
4.12 A segment of a structured background and overset mesh showing donors, receivers, buffer layer and, hole points . . . . . . . 59
4.13 Cross section of the three dimensional domain showing donors,
receivers, and calculated CVs of both meshes . . . . . . . . . . 60
ix
4.14 A segment of an unstructured background and overset mesh
showing donors, receivers, buffer layer, and calculated CVs . . 61
5.1
Schematic of the backward facing step . . . . . . . . . . . . . 63
5.2
Prism inflation layer along the wall, which is transitioning
smoothly into the isotropic tetrahedral mesh away from the
wall . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 65
5.3
Turbulent kinetic energy contours and velocity vectors in the
region after the step . . . . . . . . . . . . . . . . . . . . . . . 66
5.4
Skin friction coefficient Cf as a function of the channel length
x/H . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 67
5.5
Pressure coefficient Cp as a function of the channel length x/H 68
5.6
Reattachment at 6.22H downstream of the step . . . . . . . . 69
5.7
Normalized u-velocity profile over the channel height y/H at
x/H = −4 upstream of the step. . . . . . . . . . . . . . . . . . 69
5.8
Normalized u-velocity profile over the channel height y/H at
different locations downstream of the step . . . . . . . . . . . 70
6.1
Air tractor AT802 and corresponding CAD model. . . . . . . . 72
6.2
Air Tractor AT802 geometry (side view) . . . . . . . . . . . . 73
6.3
Air Tractor AT802 geometry (top and front view ) . . . . . . . 74
6.4
Air Tractor AT802 wireframe view. The aircraft length L ≈
is approximately 11m. . . . . . . . . . . . . . . . . . . . . . . 75
x
6.5
Plane at the centerline of the air tractor’s fuselage normal to
the z − axis showing the hybrid mesh structure . . . . . . . . 77
6.6
Air Tractor AT802 surface mesh. Unstructured surface mesh
with anisotropic extrusion at the wing and stabilizer leading
and trailing edge . . . . . . . . . . . . . . . . . . . . . . . . . 78
6.7
Anisotropic surface mesh at the trailing edge of the wing with
a section showing the prism inflation layer . . . . . . . . . . . 79
6.8
Prism inflation layer around the wing smoothly transitioning
into the isotropic tetrahedral far-field mesh . . . . . . . . . . . 80
6.9
Velocity streamlines showing the upward movement before and
the downward movement behind the wing . . . . . . . . . . . 81
6.10 Velocity vectors showing the wake vortex evolution in the
vicinity of the wing and contours showing the turbulent kinetic energy . . . . . . . . . . . . . . . . . . . . . . . . . . . . 82
6.11 Velocity streamlines showing the wake vortex evolution and
the the roll-up process . . . . . . . . . . . . . . . . . . . . . . 83
6.12 Pressure distribution at different locations downstream of the
leading edge . . . . . . . . . . . . . . . . . . . . . . . . . . . . 83
6.13 Velocity streamlines showing the vortex evolution and boundary layer separation and color contours showing the pressure
distribution and the magnitude of the z-component of the velocity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 85
xi
6.14 Axial view of the vortex evolution and boundary layer separation at the chord wise location x/c = 0.95. The color contours
show the axial vorticity indicating the evolution of the tip vortex 86
6.15 The wing surface is showing the Cp contours and the figures
show a comparison of the Cp values between the EXN/Aero
and CFX solutions at different span-wise positions . . . . . . . 87
6.16 Vorticity contours and mean velocity vectors at 10 and 50
meters planes downstream of the air tractor. . . . . . . . . . . 88
6.17 Vorticity contours and mean velocity vectors at 100 and 200
meters planes downstream of the air tractor. . . . . . . . . . . 89
6.18 Turbulence kinetic energy contours and mean velocity vectors
at 10 and 50 meters planes downstream of the air tractor. . . . 90
6.19 Turbulence kinetic energy contours and mean velocity vectors
at 100 and 200 meters planes downstream of the air tractor. . 91
7.1
Sliding lid fluid domain and boundary condition . . . . . . . . 93
7.2
Sliding lid overset mesh systems . . . . . . . . . . . . . . . . . 95
7.3
Parameters and conventions used for the validation of the sliding lid problem . . . . . . . . . . . . . . . . . . . . . . . . . . 97
7.4
Sliding lid velocity fields. Showing the overset mesh positioned
beside the background mesh and the composite mesh; Re = 400 98
xii
7.5
Three-dimensional sliding lid (Sim 2) velocity field at a plane
normal to the y-axis at y = 0.5m. Showing the overset mesh
positioned beside the background mesh (left side) and the composite mesh (right side); Re = 400. . . . . . . . . . . . . . . . 99
7.6
Three-dimensional sliding lid velocity field (Sim 3) at a plane
normal to the y-axis at y = 0.5m including a solid core. Showing the overset mesh positioned beside the background mesh
(left side) and the composite mesh (right side); Re = 400. . . . 99
7.7
Sliding lid velocity field including a part of the overset mesh
and the coarser background mesh . . . . . . . . . . . . . . . . 100
7.8
v-velocity results along a horizontal line through geometric
center of cavity . . . . . . . . . . . . . . . . . . . . . . . . . . 101
7.9
u-velocity results along a vertical line through geometric center
of cavity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 102
7.10 v-velocity results along a horizontal line through geometric
center of cavity. . . . . . . . . . . . . . . . . . . . . . . . . . . 103
7.11 u-velocity results along a horizontal line through geometric
center of cavity. . . . . . . . . . . . . . . . . . . . . . . . . . . 104
7.12 Ratio of the upstream vortex height d to the total side height
z as a function of the Reynolds number . . . . . . . . . . . . . 105
7.13 Location of the primary vortex center as a function of the
Reynolds number . . . . . . . . . . . . . . . . . . . . . . . . . 105
xiii
A.1 Propeller blade disk. . . . . . . . . . . . . . . . . . . . . . . . 119
A.2 Propeller blade cross-section with velocities and forces. . . . . 119
A.3 Comparison of the Cp values between the EXN/Aero and CFX
solution at different span-wise positions (y/b = 0.15 and y/b =
0.49). . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 121
A.4 Comparison of the Cp values between the EXN/Aero and CFX
solution at different span-wise positions (y/b = 0.63 and y/b =
0.88). . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 122
A.5 Comparison of the Cp values between the EXN/Aero and CFX
solution at span-wise position y/b = 0.63. . . . . . . . . . . . . 123
xiv
List of Symbols, Nomenclature
or Abbreviations
AABB
ADT
AGDISP
ALU
BB
BSL
BSP
CBMM
CFD
CGNS
CPU
CV
CVBB
DES
DNS
FPL
GPU
IDW
LES
MP
\Axis Aligned Bounding Box
\Alternating Digital Tree
\Agriculture Dispersal
\Arithmetic Logic Unit
\Bounding Box
\Baseline Model
\Binary Space Partioning
\Cell Based Mapping Module
\Computational Fluid Dynamics
\CFD General Notation System
\Central Processing Unit
\Control Volume
\Control Volume Bounding Box
\Detached Eddy Simulation
\Direct Numerical Simulation
\Forestry Protection Limited
\Graphics Processing Unit
\Inverse Distance Weighting
\Large Eddy Simulation
\Multi Processing
xv
MPI
NS
OOP
PDE
PM
RANS
SST
TVD
UNB
VSB
\Message Passing Interface
\Navier Stokes
\Object Oriented Programming
\Partial Differential Equation
\Polygonal Mapping
\Reynolds Averaged Navier-Stokes
\Shear Stress Transport
\Total Variation Diminishing
\University of New Brunswick
\Vision Space Bin
xvi
α
β
β∗
δij
Γ
γ
λ
n
ν
νT
ω
ω
φ
φ
φ̃
ψ
σω
σk
τ
τw
#”
c
#”
D
#”
L
#”
n
#”
Ui
#”
Ur
#”
U
A
a1
Aw
AW
b
\convergence rate
\blade pitch angle
\production constant for k in SST model
\kronecker delta
\dissipation
\diffusion coefficient
\production constant for ω in SST model
\node value
\normal vector
\molecular viscosity
\turbulent viscosity
\angular velocity propeller
\turbulent frequency
\angle between air and blade speed
\general variable
\approximate solution
\interpolation weight
\turbulent Prandtl number for ω equation
\turbulent Prandtl number for k equation
\shear stress
\wall shear stress
\distance vector
\drag force
\lift force
\normal vector
\mean velocity
\relative velocity acting on the propeller blade
\velocity vector
\area
\length scale limiter constant
\area of the propeller blade
\wing
\length of the wing
xvii
b
CD
Cf
CL
Cp
Di
e
Fa
Ft
F 1, F 2
L
grad
i, j, k
k
k
l
lk−ω
n
p
p
p
Pi
r
r̄
Si
Sij
S0
Si
t
ui
u0i
V
xi
\source term
\drag coefficient
\skin friction coefficient
\lift coefficient
\pressure coefficient
\dissipation ()
\error
\axial force on propeller blade
\tangential force on propeller blade
\Menter SST blending functions
\Differential operator
\gradient vector
\indices for index notation
\turbulent kinetic energy
\multi-grid level
\length scale
\dissipation length
\number iterations
\exponent for IDW
\pressure
\nodal point
\production ()
\residual
\average residual
\source term
\strain rate tensor
\receiver node
\donor node
\time
\instantaneous velocity
\fluctuation velocity
\volume
\position vector component
xviii
Chapter 1
Introduction
1.1
Aerial Spraying
Canada’s forests are of major economic importance and are exposed to persistent threats from insect outbreaks which are mitigated by pesticides (and
increasingly bio-pesticides) released from aircrafts. Aerial spraying has become popular due to its flexibility and ability to supply large areas with
pesticides in short periods of time. The air tractor AT802, as illustrated in
Figure 1.1, is commonly used for pesticide delivery in New Brunswick. The
spray droplets, released by the air tractor, have to be evenly spread over the
target area to maximize efficiency. The trajectories of the pesticide droplets
into a forest canopy are heavily influenced by aircraft generated and atmospheric turbulence leading to a potential for off-target drift. Off-target drifts
are subject to heavy environmental regulations due to potential hazard for
1
Figure 1.1: Air tractor AT802 [1].
human health, contamination of crops and livestock and endangerment of
ecological resources [2]. Advanced aerial operators, such as Forest Protection Limited (FPL) make use of spray drift models to predict the droplet
trajectories in advance to compensate drift.
FPL was founded in 1952 in order to protect New Brunswick’s forests
and that includes the service of aerial pest management, among others. FPL
uses the real-time computer software AGDISP [3] (described in the next section) to adjust their flight and spray parameters. AGDISP is a Lagrangian
computational spray drift model that uses simplified analytic approaches for
vortex swirling or atmospheric ground effects. The analytical models do not
adequately predict the spray distribution and deposition and so buffer zones
are required between the target and the off-target areas. A better evaluation
of the spray droplet transport can be obtained with a full-physics representation using Computational Fluid Dynamics (CFD). The CFD simulations
are not used as a real-time spray drift model due to their high computational
costs, but they can be used to create a cost-effective (relative to experiments)
2
and reliable database to validate and improve existing real-time spray drift
models.
1.2
Objectives
A full-physics CFD simulation capable of predicting the droplet transport
from the air tractor AT802 into the forest canopy requires several import
sub-models to be assembled. The objective of this thesis is to develop and
verify some of the sub-models, which will be part of the entire full-physics
CFD model. One sub-model will be the implementation of an overset mesh
strategy into the CFD software EXN/Aero. EXN/Aero is currently being
developed by a research team at UNB and its research partners, and its layout
and features are briefly discussed in Section 3.2. Due to the independent mesh
systems used in an overset mesh method, a communication method has to
be implemented so that the flow solution data between individual meshes
can be exchanged by interpolation at inner fringe points of overlapping CVs.
These inner boundary points can be located using a donor search algorithm,
which handles the communication between a minor background mesh and
major overset meshes. The connectivity algorithm should support structured,
unstructured and hybrid meshes. It should be designed in such a way that a
moving mesh capability can be added in the future (beyond the scope of this
work) allowing the aircraft to move relative to a fixed background mesh. The
implementation follows a comparison to published numerical CFD results.
3
Therefore, a simple sliding lid geometry should be used which provides many
specific well known flow features, such as corner vortices.
Another sub-model will be the modeling of the overset domain containing the air tractor geometry. The turbulence model used in this simulation
will be validated against experiments. Therefore, a flow over a backward
facing step is used due to its simple geometry, but complex flow features,
like the reattachment of turbulent shear flow, which are common to many
real flow situations. Also, to verify that all models used in the simulation
are implemented correctly, the same computational domain with identical
boundary conditions is simulated with a commercial CFD software (Ansys
CFX V14.0) and the results are compared against each other.
1.3
AGDISP System
The desire to optimize aerial spraying applications led to the development of a
simulation tool for aerial spraying applications. USDA Forest Service in cooperation with the U.S. Army, the U.S. Environmental Protection Agency and
agriculture research partners developed a Lagrangian computational spray
drift model called AGDISP [3]. AGDISP is used to estimate the spray dispersal under real-time conditions to attain a best possible spray distribution
and avoid spray drift to off-target areas. The AGDISP model uses simple analytical models to define vortex swirling, propeller effects, local wind speed,
gravity and atmospheric ground effects [2]. Ongoing improvements [4, 5, 6]
4
have been made to the AGDISP model over the last couple of decades that
include updated drift and evaporation models, the inclusion of further atmospheric effects, a new time-stepping algorithm and better representation
of droplet size distribution. The Spray Drift Task Force extended the original AGDISP model to a regulatory tool named AgDRIFT [4], in which
improvements are made to the accuracy of predictions of downwind drift and
deposition. Despite the improvements made to the AGDISP model, it shows
limitations in modeling turbulent flows, which are present in the atmosphere
and more so in the aircraft wake. A better evaluation of the spray droplet
transport can be obtained by making use of a full-physics representation of
the application using CFD. A computational study on the spray dispersal in
the wake of an aircraft was made by Ryan et al. [7].
For instance, Figure 1.2 shows the differences between the AGDISP
model and a full-physics CFD computation predicting the droplet distribution 200m behind the aircraft for 0.8, 22 and 55km/h crosswinds. The
AGDISP solution is illustrated as faded circles, with the center representing
the mean droplet position, the radius representing one standard deviation of
the droplet position probability distribution, and the color representing the
droplet size. Here, the AGDISP model uses nearly the same standard deviation for each droplet plume independent of the position of release, whereas
the CFD simulation considers local mean strain rates of the velocity field
stretching or compressing the droplet plume. [7]
Full-physics CFD modeling as shown in Figure 1.2 needs to be extended
5
Figure 1.2: Comparing full-physics CFD with low order modelling (faded
circles AGDISP) of droplet release and transport from an AT802 aircraft [7].
to predict both droplet distribution behind the aircraft and its subsequent
transport into the canopy itself. Only then would the full-physics approach
support full evaluation of AGDISP. To implement such a full-physics CFD
capability requires several sub-models to be assembled.
6
1.4
Physical Understanding and Research Motivation
Newtonian fluid flows can be described accurately with non-linear partial
differential equations which can rarely be solved analytically and hence a
discretization method is necessary. In the case of a finite volume discretization, the entire fluid domain is divided into small Control Volumes (CV).
Within these CVs, the flow equations can be approximated, which leads to
a system of algebraic equations that can be solved numerically. The result is
an entire numerical solution of the flow field composed of the discrete results
of each CV in space and time. [8]
In traditional CFD codes, the mesh type is determined by the shape
of the CV, which are subdivided into structured and unstructured types (excluding hexahedral CVs which can be both structured and unstructured).
As described by Ferziger [8], elements in structured meshes (as seen in Figure 1.3a) are easily addressed by three indices (in 3D), e.g. (i, j, k), and thus
the neighbors of an element can be located by varying the indices by ±1. The
addressing resembles a Cartesian mesh structure that simplifies programming
and accelerates the computation time due to a regular matrix structure of
the algebraic equation system. Structured meshes are easy to generate for
simple geometries but difficult for complex geometries. A further drawback
is initiated in some areas of the flow domain where a higher concentration
of CVs is necessary to obtain an accurate solution. These local mesh re7
finements are propagated over parts of the remaining domain where a coarse
resolution would be sufficient and thus the computation time is increased. An
unstructured mesh (as seen in Figure 1.3b) in contrast is suitable for complex
geometries and allows local mesh refinements. The disadvantage, however, is
the irregularity of the data structure, which increases the computation time.
Hybrid meshes (as seen in Figure 1.3c) are a combination of structured and
unstructured meshes and feature an option to take advantage of both mesh
types.
The mesh required for a full-physics representation of the aerial spraying domain faces difficulties, which can be best mitigated by use of structured
and unstructured meshes; however, it must also include the additional complexity of a moving object: the aircraft. Figure 1.4
1
shows the dimensions
and the configuration of the computational domain used for the aerial spraying process. The domain has a length of 1000m, a width of 800m and a
height of 50m. The canopy (defined by porosity and leaf area density distributions) within the domain is included as part of the full-physic atmospheric
model. If the aircraft is not taken into account, no solid objects (other than
ground) are placed in the domain and a structured axis-aligned mesh with
a CV length of ∼ 1m in all three Cartesian dimension would be the best
method of choice to model the atmospheric ground effects. However, the
aircraft AT802 flies approximately 30m above the canopy and creates a wake
including wingtip vortices that significantly influence the spray distribution
1
Figure dimensions do not match actual proportions for visual display
8
(a)
(b)
(c)
Figure 1.3: Structured, unstructured and hybrid meshes around an aircraft
airfoil. (a) Structured mesh; (b) Unstructured mesh; (c) Hybrid mesh; The
structured mesh around the airfoil is changing into an unstructured mesh
away from the airfoil.
9
of the droplets.
The turbulence generated by the aircraft cannot be resolved with the
coarse mesh used for the atmospheric turbulence; therfore, the aircraft’s complex geometry requires a hybrid mesh (combined structured and unstructured) for meshing simplicity and computational advantages. Since the wake
generated by the aircraft strongly depends on the correct prediction of the
boundary layers around the aircraft body, a much finer local mesh resolution
is necessary. Therefore, considering the needs of the atmospherical and the
near aircraft wake modelling a full-scale simulation with a single mesh is not
possible without a mesh regeneration or deformation at each time-step due
to the significant changes in scale (both geometrically and in terms of turbulent flow activity) as well as the motion of the aircraft relative to the canopy
(that in general is not a flat uniform terrain).
Figure 1.4: Sketch of the aerial spraying domain including the aircraft AT802.
10
A solution to the meshing difficulties is the use of an overset mesh
strategy where the computational domain consists of separate mesh systems
(each focused on resolving its own flow features of interest).
1.5
Overset Mesh Method
Essential to an overset method is the determination of mesh system overlap,
which for a dynamic simulation has to be undertaken at each timestep, along
with interpolation of solution variables between the mesh systems (exchange
of flow solution data at their boundaries). Usually, the overset mesh system consists of a major background mesh with superimposed minor meshes,
which enclose parts of body configurations or entire objects. Figure 1.5 shows
an overset mesh system for aerial spraying where the background mesh (major mesh) spans over the entire domain and the superimposed mesh (minor
mesh) encloses the solid aircraft body. A two-dimensional arrangement of
the aerial spraying domain is shown in Figure 1.6. The physical task of the
background mesh will be the prediction of atmospheric ground effects and
turbulence created by the canopy. The overset mesh enclosing the aircraft
is superimposed on to the background mesh and solves the near-body flow
around the aircraft. The superposition of both meshes allows the aircraft
to move relative to the background mesh and its orientation relative to the
background mesh to be changed for each simulation or each time step without the need of creating a new mesh. The geometrical independence of the
11
Figure 1.5: Major background mesh superimposed by a minor mesh enclosing
the aircraft body.
overlapped meshes allows to design each mesh individually and facilitates the
meshing of complex curvatures since their interfaces do not need to concur.
To help explain the overset mesh method, a simple two-dimensional
overset mesh is illustrated in Figure 1.7. The background mesh consists of
a rectangular structured mesh which is superimposed by a single cylindrical
curvilinear structured mesh with a solid rectangular body. Usually, the superimposed meshes are designed to solve near-body regions which require a
finer mesh resolution than off-body regions. Therefore, in regions where the
minor and background mesh overlap, the minor mesh is given the highest
solution priority and its mesh is preferred over the background mesh for sub-
12
Figure 1.6: Depicting arrangement of mesh systems for spray droplets released from an aircraft and a subsequent transport on to the forest canopy.
sequent computations for that physical location. This leads to the creation
of two inner fringe boundaries. The first inner fringe boundary is defined by
the outer boundary of the higher priority mesh. Both, background and minor
meshes are typically solved at a region that is three to four CVs deep to the
outer boundary. The adjacent points to that specific overlap region form the
second inner fringe boundary. All points of the lower priority background
mesh, which fall outside of the second inner fringe boundary are blanked
out and not solved. The process of locating points in the background mesh
which are excluded from the solution procedure is called hole cutting. Flow
solution data between the meshes is transferred via interpolation at these
shared inner fringe boundaries using a donor-receiver methodology.
This implies that in regions where both meshes are overlapped, the CVs
13
Figure 1.7: Rectangular background mesh with a superimposed curvilinear
cylindrical mesh enclosing a solid body.
with the higher priority are solved, and the CVs with the lower priority are
blanked out. Figure 1.8 shows the data transfer between the superimposed
meshes. For clarity, the cylindrical mesh is positioned beside the background
mesh and only its wireframe is superimposed to the background mesh. The
layer of CVs which comprise the outside boundaries of the cylindrical minor
mesh are flagged as receivers. These receivers obtain an interpolated value
from overlapping control volumes, flagged as donors, in the background mesh.
In this way, the forced receiver values are based on calculated donor values
(flow variables such as velocity, pressure etc.). This process is repeated for
the opposite direction where the receivers for the background mesh are the
CVs next to the blanked out region and their donors come from the minor
mesh. A buffer region exists between the donors and receivers of a particular
mesh such that no CV can be both a donor and receiver. This two-way cou-
14
Figure 1.8: Data transfer between overlapped meshes at their fringe points
and illustration of hole-points.
pling allows flow features to freely pass from the background to the minor
mesh and vice-versa.
Such domain connectivity algorithms for simple overset mesh methods in
CFD applications were first applied in the early eighties. One of the pioneers was Steger et al. [9] in 1983. For his work, he used 2D structured
meshes where a major mesh was overlapped by one or more minor airfoil
meshes. The closest receiver node for a donor node was found by comparing
the distance from the donor node to each receiver node. This search process
is computationally expensive and an improvement was obtained by using a
‘stencil walk’ procedure if the boundary curve was smooth, as illustrated in
Figure 1.9. For the stencil walk, the neighbors of the previous detected donor
15
Figure 1.9: Stencil walk from point T to point T 0 which is nearest to B 0 . [9]
node are used to find the next closest node to the new receiver node. This
process is repeated until the closest donor is found. Steger used a simple
Taylor expansion to interpolate the flow solution data between the meshes.
A more complex, fully-automated overset methodology was developed
by Wang et al. [10]. Wang simulated flows around a three-element airfoil, a
storage tank that separates from a wing and a three-dimensional missile fin
geometry using an Alternating Digital Tree (ADT) [11] data structure for the
donor search procedure. The structure of an ADT is shown in Figure 1.10
where [ai , bi ] are the minimum and maximum position vectors of the search
space covered by the tree-node i. A standard tree traversal limits the number
of candidate target elements. The nodes of the ADT in Wangs work contain
the Bounding Box (BB) coordinates of all CVs in each mesh. The BBes
are then be used to perform intersection checks between the receiver CV BB
16
Figure 1.10: Data structured of an Alternating Digital Tree [12].
and the target CV BBes in the leaf nodes of the trees. The tree traversal
BB intersection check narrows down the number of potential donor CVs and
further linear search determines the donor CV which contains the centroid
of the receiver CV. Wang et al. made use of a tri-linear interpolation to
exchange the flow solution data between the CVs of two different meshes.
Since CFD is compute intensive, attention also has to be given to parallelization of the additional steps introduced by overset solutions. Parallelization strategies including overset have been documented for traditional
multicore computing using MPI and OpenMP. In 2000, Prewitt et al. [13] investigated the algorithms and performances of different grid assembler (Beggar [14], PEGASUS [15], DCF3D [16] and CMPGRD [17]), which were implemented in a multicore computing environment by various researches. Prewitt
concluded that in comparison to the above mentioned codes, Beggar had overall superior capabilities. Beggar uses a Polygonal Mapping tree (PM) (see
Figure 1.11a) which is a combination of an octree and a Binary Space Partitioning (BSP) tree data structure to identify hole points and interpolation
17
stencils. The two-dimensional equivalent to the three-dimensional octree is a
quad tree as illustrated in Figure 1.11b. The leaf nodes (highest level) in the
BSP tree structure contain information about a point lying in- or outside of
a plane representing a segment or an entire facet of an overlapping boundary
grid surface. To quickly narrow down the search space and to identify the
leaf node of the BSP tree for a given point, the BSP tree is inserted into the
leaf nodes of the octree data structure. Thus, each leaf octant of the octree
is classified relative to the grid boundaries. A leaf octant can either be inside
or outside of a mesh block or contain a mesh boundary. The localization of
an octant containing a given point leads to an efficient way to determine if
a point lies inside or outside of a mesh block or if it is a boundary point. In
the latter case, a further step is necessary where the BSP tree stored in the
boundary octant is used to determine if the point lies inside or outside of the
boundary facet.
A prominent overset grid assembler called SUGGAR was developed by
Noack et al. [18][19][20][21] for structured and unstructured meshes. The
SUGGAR code uses an octree-based Cartesian approximation to the geometry for the donor search process. SUGGAR uses a solver neutral library
(DiRTlib [22]) which contains the operations required to implement the overset capability to a flow solver. The latest version of SUGGAR was designed
for moving body problems and simulations were performed for complex geometries like a C130 aircraft with a parachute. SUGGAR is a robust and
validated grid assembler but not designed for the use in a multicore-manycore
18
(a)
(b)
Figure 1.11: (a) Example quad tree mesh; (b) Example PM tree structure. [13]
computer environment. Load balancing deficiencies limit the scalability of
threads for parallel execution on shared memory machines. Another deficiency is large memory requirements caused by the octree data structure,
which also limits the automation of the hole cutting process [21]. SUGGAR++ [21] is a rewrite of the SUGGAR code in which the deficiencies
of SUGGAR are mostly eliminated. The octree-data structure is replaced
by an inverse map data structure, which is a Cartesian-like subdivision of
the BB enclosing the donor grid. The grid points are then assigned to the
coordinates of the Cartesian-like grid, which are closest to them. This data
structure is similar to that used by Sitaraman et al. [23] (as described below), which improves the donor search algorithm and reduces the amount
of memory for storage. SUGGAR++ also showed improvements of parallel
multicore performance characteristics relative to SUGGAR.
19
The CHIMPS [24] domain connectivity package was designed for multicore computing environments. The mesh is distributed over several processors where each of them receives a list of points for which the processor
has to find interpolation points in its local mesh. The interpolation points
are found based on an algorithm using the ADT data structure shown in
Figure 1.10, which is a less efficient search algorithm. For the interpolation
of flow variables at shared boundaries, the standard tri-linear interpolation
formula is used.
The PEGASUS code is one of the oldest grid assembler codes which
has gone through many updates. The donor-search process is based on an
ADT data structure to narrow down the number of potential donor CVs.
The CV containing the receiver centroid node is found by using a stenciljumping algorithm which is based on a tri-linear interpolation using a Newton
iteration. PEGASUS is robust and validated but some processes have to be
executed sequentially and can not be performed simultaneously.
Also Liu et al. [25] made use of an ADT searching procedure to locate
interpolation points in an unstructured tetrahedral mesh and simulated flows
of unsteady pitching airfoils, butterfly valves and a mono-cylinder IC engine
with piston movement.
In [23] Sitaraman et al. used a parallel multicore overset mesh domain
connectivity algorithm for rotorcraft analysis, which can also be used for
other types of unsteady, moving-body problems. His donor searching algorithm is based on meta data in terms of bounding boxes and a division of
20
the BBs into so called Vision Space Bins (VSB) facilitating the donor search
algorithm. The CV indices are reordered in a bin-wise fashion in order to
locate a VSB based on the coordinates of a given point in a one step process.
A VSB spiral search is performed until a VSB containing a candidate donor
node is found. The donor node closest to a given point is determined with a
line segment CV face intersection check. The multicore parallel programing
is achieved by allocating different cells of the domain to several processors so
that each processor only executes calculations associated to its own cell block.
The processors transfer information via communication tables so that each
processor, which needs to find donor nodes for its own receiver nodes, forms
a list of the receiver nodes and sends it to all potential processors whose cell
blocks might contain valid donor nodes. The information is returned, and
the requesting processor chooses the best donor nodes based on interpolation
criteria.
Parallelization strategies including overset has only recently being investigated for use on manycore devices such as the Graphics Processing Unit
(GPU). In [26] Soni et al. execute the same donor search algorithm as described above by Sitaraman (see [23]) on GPUs. The main task hereby is to
parallelize the donor search process, which is done by making use of as many
threads as there are grid nodes in the receiver mesh searching for donor nodes
in the donor mesh. The domain connectivity algorithm is verified by demonstrating the flow solutions of a two-dimensional NACA0012 airfoil in [26]. A
three-dimensional comparison of the drag coefficient of a static sphere to a
21
moving sphere at the same Reynolds number is presented in [27] and shows
that the moving overset solution only approaches the solution of the static
sphere.
The basis of the overset mesh methodology used for this research
project lies on a variant form of the meta-data used by Sitaraman et al. [23]
and is adapted for the development of a fast searching algorithm executed
on a hybrid, multicore-manycore computing architecture.
22
Chapter 2
Turbulent Flow Modeling
The atmospheric flow is governed by the Navier-Stokes (NS) equations. In
EXN/Aero, solutions of turbulent flow fields can either be obtained in Reynolds
averaged SST or LES formulations or combined in a DES formulation. For
the work done in this thesis, a two-equation k − ω model with stress and
production limiters is sufficient to obtain accurate results and thus this modified k − ω model is preferred to the LES or DES formulations, which are
more complex. The Reynolds-Averaged Navier-Stokes (RANS) equations for
an incompressible fluid are described in Section 2.1 and the SST-model is
discussed in Section 2.2.
23
2.1
Fluid Equations of Motion
The atmospheric flow around the aircraft is governed by the continuity equation and Newton’s second law of motion. In tensor notation, the incompressible continuity equation and Newton’s second law of motion are [28]
∂ui
=0
∂xi
(2.1)
∂ui
∂p
∂τji
∂ui
+ ρuj
=−
+
+ SM i ,
∂t
∂xj
∂xj
∂xj
(2.2)
and
ρ
where ui is the velocity, τij are the viscous stresses, p is the pressure and SM i
are other body forces such as gravity. Newton’s law of viscosity relates the
viscous stresses τji to the rate of deformation of fluid elements [28]:
∂ui ∂uj
τji = ρν
+
,
∂xj
∂xi
(2.3)
where ν is the kinematic viscosity. A combination of Equation 2.1 - 2.3 yield
the NS equations in non-conservative form [28]:
∂ui
∂ui
1 ∂p
+ uj
=−
+ν
∂t
∂xj
ρ ∂xi
∂ 2 ui
∂xj ∂xj
+ SM i .
(2.4)
The left hand side of Equation 2.4 represents the acceleration of a fluid
element in time and the convective acceleration in space. The first term on
the right hand side is the pressure gradient followed by the diffusion term.
24
The conservation equations show similarities and can be written as a general
transport equation in conservative form for all fluid properties by introducing
the general variable φ [29]:
∂(ρφ)
+ div(ρφu) = div(Γ grad φ) + Sφ ,
∂t
(2.5)
where u is the velocity vector, Γ is the diffusion coefficient and Sφ is a new
source term that contains terms like the pressure gradient in Equation 2.4.
An integration of Equation 2.5 over the CV, applying the divergence theorem
of Gauss for the convective and the diffusion term and a second integration
over time yield [29]:


Z


t+∆t
Z


t+∆t
Z

Z
δ
 n.(ρuφ)dA dt
(ρφ)dt dV + 
δt
t
t
CV
A
 t+∆t

t+∆t
Z
Z
Z Z




=
dt +
n.(Γ grad φ)dA
Sφ dV dt ,

t
t
A
(2.6)
CV
where n is the vector normal to the surface area dA. Equation 2.6 is used
for developing discretization methods in CFD codes using the finite-control
volume method.
Equation 2.4 is applicable to solve laminar flows and turbulent flows
directly (Direct Numerical Simulation (DNS)). However, a DNS requires an
extremely fine and tailored mesh to the wide range of turbulence scales. A
by far less computationally expensive treatment of turbulent flows can be
25
achieved using a turbulence model. Therefore, the instantaneous velocity ui
and pressure p are broken up into a mean Ui , P and a fluctuation u0i , p0 component, respectively. By replacing the instantaneous velocity in Equation 2.4
by its components and time (ensemble) averaging the equation, the RANS
equations in non-conservation form is obtained [30]:
ρ
∂Ui
∂Ui
∂P
∂
+ ρUj
=−
+
(2µSij − ρu0i u0j ) + SM i .
∂t
∂xj
∂xi ∂xj
(2.7)
The terms in Equation 2.8 are similar to those in Equation 2.4 with the
exception of the quantity u0i u0j , called the Reynold stress term arising from
the decomposition of the velocity which must be modeled. The term Sij is
the strain-rate tensor:
1
Sij =
2
∂Ui ∂Uj
+
∂xj
∂xi
.
(2.8)
A model for the Reynold stress term (SST turbulence model introduced by
Menter [31]) is described in the following chapter.
2.2
Turbulence SST-Model
Menter [31] originated the SST-turbulence model which is based on the baseline (BSL) model [31] to retain the robust and accurate formulation of the
original k − ω model in the near wall region and to avoid its freestream dependency by blending into the k − model towards the outer part of the
26
boundary layer. Here, the original k − ω model refers to the Wilcox (1988)
k − ω model given in [32] and [33]. The original k − ω model accurately
predicts flow separation near solid boundaries which leads to more accurate
results than the standard k − model, which is inadequate under adverse
pressure gradients close to the wall. Away from the wall, the original k − ω
model blends into the k − model, which is less sensitive to free stream values. The blending is achieved by transforming the k − model into a k − ω
formulation, multiplying the original k − ω model by a blending function F1
and the transformed model by a blending function (F1 −1), and a subsequent
addition of both models. [31]
Following, the transport equation for the turbulent kinetic energy k is
given by:
∂
∂k ∂uj k
+
=
∂t
∂xj
∂xj
νT ∂k
ν+
+ Pk − Dik ,
σk ∂xj
(2.9)
where νT is the turbulent viscosity, Pk is the turbulent production and Dik
is the turbulent dissipation. The transport equation for the turbulent frequency ω is:
∂ω ∂uj ω
∂
+
=
∂t ∂xj
∂xj
νT ∂ω
γ
β ω
2σω2 ∂k ∂ω
ν+
+ Pk − ∗ Dik +(1−F1 )
.
σω ∂xj
νT
β k
ω ∂xk ∂xk
(2.10)
The blending function F1 used for the blending of the original k − ω and the
transformed k − is also used to determine any model constant φSST for the
new model:
φSST = F1 φ1 + (1 − F1 )φ2
27
(2.11)
where the constants of the original k − ω model are represented by φ1 and
the constants of the transformed k − model are represented by φ2 . The
blending function is defined as:
where
F1 = tanh(arg14 ),
(2.12)
√
k 500ν
4ρk
arg1 = min max
;
;
,
0.09ωy y 2 ω
CDkω σω2 y 2
(2.13)
and y is the distance to the next surface and CDkω is the positive portion of
the cross-diffusion term in Equation 2.10 defined as:
CDkω
∂k ∂ω σω2
−20
; 10
.
= max 2ρ
∂xj ∂xj ω
(2.14)
An improvement of the SST-model is obtained through a stress limiter applied on the turbulent viscosity νT [34]:
νT =
a1 k
p
,
max{a1 ω, F2 Sij Sij }
(2.15)
so that νT does not strictly depend on ω, which avoids an over prediction of
τ in adverse pressure gradient flows where the turbulence production exceeds
its dissipation as found from experiment [35]. The function F2 :
F2 = tanh(arg22 ),
28
(2.16)
where
√
k 500ν
;
,
arg2 = max 2
0.09ωy y 2 ω
(2.17)
is one for boundary-layer flows and zero for free shear flows. The SST-model
also applies a production limiter to avoid excessive generation of turbulence
energy in the vicinity of a stagnation point [34]:
Pk = min{10β ∗ kω, 2νT Sij Sij }.
(2.18)
The turbulence dissipation rate per unit mass is defined as:
3
Dik = k 2 /lk−ω ,
(2.19)
where the dissipation length lk−ω is given by:
√
lk−ω =
k
β ∗ω
.
(2.20)
The model constants for the original k − ω model and transformed k − model are given in Table 2.1
Wilcox [30] stated, that only little improvements are achieved by using
the cross diffusion term and the blending functions as added in Equation 2.10.
However, the stress-limiter modification improves the predictive accuracy of
the k − ω model without cross diffusion and blending functions as shown by
Kandula et al. [36]. Also Huang [37] showed, that the stress-limiter limiter
29
Table 2.1: Closure coefficients for turbulence SST-model [31].
Original k − ω model
Transformed k − model
Coefficient
σk1
σω1
β1
β1∗
γ1
Coefficient
σk2
σω2
β2
β2∗
γ2
Value
2
2
0.075
0.09
5/9
Value
1
0.856
0.0828
0.09
0.44
greatly improves incompressible- and transonic- flow predictions. [30] For the
following studies, the blending function F1 is set to one, which eliminates the
cross-diffusion term and the blending of the closure coefficients so that only
the closure coefficients of the original k − ω model are used. This simplifies
the ω-transport equation to:
∂
∂ω ∂uj ω
+
=
∂t
∂xj
∂xj
β ω
νT ∂ω
γ
ν+
+ Pk − ∗ Dik .
σω ∂xj
νT
β k
30
(2.21)
Chapter 3
Numerical Methods
3.1
Computational Solution Procedure
The governing equations of fluid flow were described in Chapter 2 and this
section addresses the solution procedure followed by the EXN/Aero code.
The flow chart is shown in Figure 3.1. The right hand side of the diagram
illustrates problem specific input data and overset procedures whereas the
left hand side follows a usual program sequence of the EXN/Aero code. The
solution procedure starts with the initialization of initial conditions, fluid
properties and problem specific settings. After the initialization, the first
time loop is initiated for unsteady flow simulations and the overset algorithm
is executed in order to create the mesh connectivity information between the
overset meshes. At this point, all receiver and donor nodes are located and
the interpolation weights are calculated. The interpolation information is
31
stored and can be recalled at any time, which avoids a recalculation of interpolation weights at each coefficient iteration or time loop for stationary
meshes. The coefficient loop starts with the discretization of the governing
equations and the associated calculation of gradients and solution coefficients
at each nodal point. This leads to a system of linear algebraic equations,
which are solved using an additive correction multi-grid methodology as described in [38] and summarized in Section 3.2.3. The node values of receiver
CVs are constant during an iteration and updated at the beginning of each
fine-grid multi-grid iteration (see Section 3.2.3) based on the receiver-donor
information obtained at the beginning of each time loop.
32
Figure 3.1: Computational solution procedure including overset executions.
33
3.2
EXN/Aero Software Design
The overset mesh method is implemented in the CFD program EXN/Aero [39].
As described by Gerber et al [39], EXN/Aero is based on an object oriented Fortran 2003 code, and it is designed to take advantage of new hybrid
multicore-manycore computer architectures to improve the computational
performance.
3.2.1
EXN/Aero Features
EXN/Aero uses an Object Oriented Programming (OOP) style in higher levels. In lower levels, however, a procedure-based programming style is utilized
for all major (compute intensive) tasks to avoid the increased computational
overhead of an object-oriented implementation. EXN/Aero shares similar
features that are used in many commercial CFD packages. The finite volume
discretization method is used together with an upwind biased Total Variation
Diminishing (TVD) (Van Leer) scheme for second order advection behavior.
The discretized equations are solved using an additive correction multi-grid
(see Section 3.2.3) along with a red-black Gauss-Seidel iterative method. For
the pressure-velocity coupling, the iterative solution algorithm SIMPLEC is
applied, as described in [29]. Turbulent solutions can either be obtained
in Reynolds averaged SST or filtered Large-Eddy Simulation (LES) formulations and, if required, combined in a Detached Eddy Simulation (DES)
formulation. The in- and output to EXN/Aero is managed with the CFD
34
General Notation System (CGNS) [40], which was first used in the aerospace
industry before it was opened to the public under the administration of the
CGNS Steering Committee. The CGNS standard is wide spread in CFD and
enables a standardized communication between CFD-solvers and pre- and
post-processing software.
3.2.2
EXN/Aero Domain Decomposition
R
A pre-processing software such as Pointwise
is used to generate the mesh
for the computational domain, which is recorded in a CGNS-file and read by
the EXN/Aero software. If required, the computational domain is divided
into several sub-domains. The sub-domains are a collection of adjacent CVs
and are called ‘cells’ in EXN/Aero. Adjacent cells have common boundaries,
called ‘interfaces’, that are of the ‘inter-cell’ type. Cell boundaries which
are located at the edge of a domain are of the type ‘boundary’. The initial
number of cells is predefined by the mesh-generation software and recorded
in the CGNS-file. For the parallel programming implementation, however,
EXN/Aero uses a cell based mapping module (CBMM), which detects available compute resources (CPUs and GPUs) and calculates the optimal number of cells and interfaces based on a computationally efficient load balance.
CBMM also manages the assignment of cells to available processing units so
that a maximum throughput can be obtained. Figure 3.2 shows an example
load balancing of a 2D problem and how it is broken up into cell and interface
objects. In this case, cell 1 is assigned to GPU-1, cell 2, 3 and 4 are assigned
35
to GPU-2 and cell 5 and 6 are assigned to the host CPU. In contrast to the
Figure 3.2: Cell and interfaces of a 2D mesh with 6 cells and 20 interfaces.
cell tasks, interface tasks might have to access common memory that is not
shared between the processing units. Thus, one task of an interface object
is to transfer boundary data (cell data that is on either side of an interface)
to a common processing unit. There, the data is processed and transferred
back to the original processing unit. These tasks are executed in parallel,
meaning that an interface task is launched as soon as the two cells corresponding to an interface are processed. Thereby, attention is paid to keeping
36
the data transfer at a minimum by selecting the optimum processing units.
An example of four interfaces is given in Figure 3.2. Interface 1/2 is shared
by cell 1 and 2 and thus can be processed either on GPU-1, 2 or the CPU. In
such a case, the optimal assignment is made based on a performance analysis.
This also applies to interface 2/5, which is either processed on GPU-2 or the
CPU. Interface 3/4 and 5/6 do not depend on memory from different units
and thus are processed on GPU-2 and the CPU, respectively. [41]
As mentioned in Section 3.2, EXN/Aero has been specifically designed
for manycore computing environment [39]. The overset mesh technique described in Section 4 is implemented in EXN/Aero. In the case of EXN/Aero,
to accommodate the improved performance when processing data on GPUs,
its data structures distinguish structured/unstructured and single/double
precision regions of the mesh.
This hybrid approach provides consider-
able flexibility in deploying CFD task execution in heterogeneous environments. [39]
Figure 3.3 shows how cells and interfaces are deployed in the context
of overset mesh systems. The interfaces have the role of connecting different
cells (and any associated data transformations) that can have tasks to be
executed on different devices. The scenario in Figure 3.3a shows a cylindrical structured overset mesh made up of three different cells and a single
structured background mesh. Additional to the ’inter-cell’ interfaces shown
here, EXN/Aero creates overset interfaces from the type ’interpolate’ connecting each cell of the background mesh with each cell of the overset mesh.
37
(a)
(b)
(c)
Figure 3.3: Simplified background and overset mesh system. Each mesh
system can be divided in cells and interfaces with cells using structured or
unstructured data, and single or double precision. (a) shows two structured
mesh systems, cell, and interface use; (b) shows use of structured and unstructured cells; (c) shows use of multiple cells of mixed structured and unstructured data.
38
In this manner, the scenario in Figure 3.3a has three overset ’interpolate’
interfaces. The scenario in Figure 3.3b has one overset ’interpolate’ interface
connecting a structured background mesh to an unstructured overset mesh.
In the scenario in Figure 3.3c, the background mesh system is a hybrid mesh
(a combination of a structured and an unstructured mesh) connected by an
interface. The overset mesh is constructed of three different structured cells,
which results in six overset ’interpolate’ interfaces. Results shown later are
obtained with the top and middle scenario, but many combinations could be
employed for testing.
3.2.3
Additive Correction Multi-grid Methodology
The spatial discretized governing equations of fluid flow, as shown in Chapter 2, have the form:
Lφ = b
(3.1)
where vector φ is the true solution of the system, L is a differential operator
(coefficient matrix) and b is a known vector. These equations are solved
using an iterative Gauss-Seidel or Jacobi method at each time step. Iterative
methods are favored over direct methods because of lower memory requirements. However, the convergence rate of iterative solvers is reduced if the
mesh is refined due to a slower propagation of boundary values across the
domain. Thus, EXN/Aero is equipped with an additive correction multi-grid
methodology (see [38]) to account for the convergence issues. This section
39
gives an overview of the multi-grid methodology. A more detailed description
can be found in [41].
The multi-grid methodology is best described by means of the flow
chart provided in Figure 3.4. In addition to solving Equation 3.1 at the
Figure 3.4: Multi-grid methodology V-cycle.
initial fine grid (level 0), error correction equations are solved at multiple
40
grid levels (the grids become gradually coarser with each level). After n
iterations are performed on the fine grid using the Gauss-Seidel method, low
frequency error components have smoothed out and the approximate solution
φ̃ after n iterations is obtained. This requires only a few number of iterations,
which typically show a rapid convergence. Following, the error of φ̃ can be
described as:
e = φ − φ̃
(3.2)
where e is the error after n iterations. However, the convergence rate might
decrease vastly after a few iterations since the Gauss-Seidel method is inefficient in solving low-frequency errors. At this point, a grid level switch
(from fine to coarse) takes place so that the low-frequency errors from the
fine mesh appear as high-frequency errors in the coarser mesh and can be
efficiently smoothed out by applying the Gauss-Seidel method. Instead of
solving the original Equation 3.1 with a coarse grid, an error correction
equation is solved, which is derived by first defining the residual r at any
multi-grid level k as:
rk = bk − Lk φ̃k
(3.3)
Substituting Equation 3.1 into 3.3 yields, after some rearrangement, the following correction equation:
Lk ek = rk
(3.4)
whereas the differential operator Lk and the residual vector rk are constructed
from the previous finer grid k − 1. This transformation from fine-to-coarse
41
is called restriction. Equation 3.4 is solved with the Gauss-Seidel method,
and the solution of this equation with a coarse grid at level k + 1 is used
to correct the intermediate solution of the previous finer grid k so that the
convergence rate of the finer grid is improved:
φk = φ̃k + ek+1
(3.5)
The transformation of the error vector from coarse-to-fine is called prolongation. The coefficients of the differential operator Lk only depend on the
coefficients of the original Equation 3.1 and thus only need to be constructed
when the multi-grid method is initiated. The residual rk depends only on the
residual from the previous iteration at the same or previous grid level and
has to be updated at each iteration. EXN/Aero constructs the coefficient
matrices for the coarser grid algebraically from the previous finer grid level
using an additive correction method. Algebraic multi-grid methods obtain
the coefficients for the coarser grid by agglomerating elements of the finer
grid level. This prevents any computationally expensive interpolations between grid levels. More details of the agglomeration strategy of structured
and unstructured grids and the coefficient construction are given in [41].
The sequence of the multi-grid logic can be summarized with the flow
chart as shown in Figure 3.4. Before a fine-mesh iteration is started, the
receiver values (the flow variable that is currently processed) are interpolated.
42
An average residual r̄ per CV is calculated after each fine grid iteration:
N0
P
rp0
p=1
r̄ =
N0
(3.6)
where N 0 is the number of nodes and rp0 is the residual of a CV at the fine
grid level 0. The convergence rate α:
α=
r̄n
r̄n−1
(3.7)
is evaluated and used to trigger a multi-grid V-cycle if the reduction rate is
greater than a certain threshold. The iteration will end when a fixed number
of fine grid iterations is exceeded or when the current residual is smaller than
O orders of magnitude of the residual r̄0 after the first fine grid iteration. In
the case that a multi-grid V-cycle is triggered, a fixed number of iterations
is performed at each multi-grid level during the restriction process (e.g. two
iterations as seen in Figure 3.4). After arriving at the coarsest grid level,
the prolongation process is initiated. Here, a fixed number of iterations is
performed (e.g. eight iterations as seen in Figure 3.4) at each multi-grid level
k after the additive correction of ek+1 is applied before the first iteration.
Back at the fine grid level 0 the residual is calculated after each fine grid
iteration, compared to the threshold and, if applicable, another multi-grid
V-cycle is initiated.
43
3.3
Design for Manycore Computing
Traditionally, the majority of software applications follow a sequential program flow and are constrained to the performance of a single CPU. Until
around 2003, the performance of microprocessors had continuously improved
by increasing their clock frequency, and thus, software applications speeded
up with each new generation of microprocessors. Associated increasing energy consumptions and heat-dissipation issues have slowed such performance
gains and further significant speed improvements for a single CPU were not
expected. Consequently, the semi-conductor industry enhanced the performance of their microprocessors by moving towards multicore CPUs, where
one chip is equipped with multiple processing units. The switch to multicore CPUs forced software developers to redesign their programs (which
are based on a sequential execution) and to build new programs based on
a parallel program execution in order to utilize the improved performance
of new multicore microprocessors. As multicore microprocessors will remain
in place in the future, manycore GPUs promise further advancement in improving computer performances. This can be seen in Figure 3.5 where the
theoretical performance between CPUs and GPUs is compared over the last
years. The increasing gap between the CPU and GPU performances is attributed to the special design of the GPUs for compute-intensive, highly
parallel computations [42].
Figure 3.6 shows the basic design of a CPU and a GPU. Multicore CPUs
44
Figure 3.5: Performance gap between CPUs and GPUs.[43]
aim to maintain execution speeds of sequential programs using multiple cores
and are designed to handle heavy and complex instructions. Therefore, the
CPU must lower operation latencies within the same thread to consequently
reduce the total execution latency of each individual thread. This requires
low-latency Arithmetic Logic Units (ALU), sophisticated operand data delivery logic, and large cache memories, which increase chip area and power.
In contrast to the coarse grained parallelism of the CPUs, GPUs focus on
a fine grained parallelism, which place less value on the low-latency memory access, and thus provide more hardware space for arithmetic execution
45
units and memory access channels. The GPUs rely on large number of much
smaller cores, which share the same simple instruction that are processed on
a large amount of data. This significantly increases the execution throughput
of parallel applications and turns GPUs into excellent numeric computing engines, which can solve large systems of algebraic equation (such as arise in
CFD solvers) in parallel on many different simple cores. [42]
Figure 3.6: Design differences between CPUs and GPUs. [42]
46
Chapter 4
Overset Mesh Technique
As mentioned in Section 1.4, the overlapped meshes need to exchange their
flow solution data via interpolation at their boundaries and, hence, a mesh
connectivity algorithm is necessary to identify appropriate inner-boundary
fringe points. In addition to the general interfaces as first introduced in
Section 3.2, overset mesh systems have the interface type ‘interpolate’, which
is used to establish a connection between separate cell blocks. In the case
of dynamic meshes, the donor-search algorithm must be called at each time
step to locate the donors at the new mesh positions and to calculate the
interpolation coefficients. The implementation of an overset mesh technique
in a CFD-software like EXN/Aero requires further computational efforts in
addition to solving the governing flow equations. An efficient donor-search
algorithm must be applied to minimize the solution time.
Meta-data in the form of BB is used as a foundation to develop a
47
fast domain connectivity algorithm. The necessary steps are best illustrated
with a simple composite mesh system as shown in Figure 4.1. The mesh
Figure 4.1: The left side shows two independent meshes, a structured cylindrical minor mesh (overset), and Cartesian structured major mesh (background) which are superimposed to an overset mesh system on the right
side.
system consists of a Cartesian structured background mesh (mesh A) and
a structured curvilinear cylindrical mesh (mesh B), which is superimposed
onto the background mesh. The steps involved in developing a connectivity
between the overlapped meshes are as follows:
1. Creating bounding boxes
The first step is to create Axis-Aligned Bounding Boxes (AABB) around
each cell block, as seen in Figure 4.2. The BBs are defined by the minimum
48
and maximum mesh coordinates ({xmin , ymin , ymin }, {xmax , ymax , zmax }) of
each cell block, respectively. As mentioned in Section 3.2, one domain
Figure 4.2: Creation of individual BBs for each cell block; One BB enclosing
the background cell and three BBs enclosing the three cells from the overset
mesh.
might consist of several sub-domains (cells) or is divided in several cells
by the CBMM. In our case, the background mesh consists of a single cell
whereas the superimposed cylindrical mesh is a composition of three cells.
Each BB is further divided into VSB (see Figure 4.3) that are numbered
consecutively. All CVs are assigned to the VSB that contains its centroid
coordinates. The size of the VSBs depends on the average volume of the
CVs within one cell block and can be adjusted depending on how much
49
CVs the average VSB should contain. The bin-wise reordering allows a
quick access to the CVs inside a VSB through the VSB index. The VSB
Figure 4.3: Each BB is divided in smaller VSBs.
indexing also allows from the beginning to exclude regions that are not of
interest for further tasks such as areas that do not contain any overlapping
CVs. This is illustrated in Figure 4.4, which only shows VSBs of mesh B
that contain CVs and only a few VSBs of mesh A for illustrative purposes.
2. Receiver identification
When the BB and VSB initialization is completed, the outer fringe nodes
of the superimposed meshes are flagged as receiver nodes. Figure 4.5
50
Figure 4.4: Hiding of VSBs that do not contain any CV centroids.
shows the superimposed mesh B where the boundary nodes are flagged
as receivers (orange CVs). The slice through the center illustrates that
one layer of receiver CVs is present. It is an easy task to identify receiver
nodes of mesh B since they are adjacent to overset interfaces, which are
already defined in the pre-processing.
3. Donor search procedure
The donor search procedure is computationally expensive and a search
refinement is used to reduce the number of calculations. Again, all cell
blocks are connected through an overset interface that associates each cell
of mesh A with each cell of mesh B. To find donors for the receiver nodes
51
Figure 4.5: The fringe nodes of the overset mesh are flagged as receivers
(orange) are shown.
in mesh B, a loop over all overset interfaces is conducted, and the BBs of
the current cell pair are checked for an intersection. VSBs and thus CVs
inside non-intersecting BBs do not need to be considered in further search
processes, which reduces the searching time significantly.
The VSBs of mesh B have stored the information whether they contain a
receiver CV or not. Instead of looping over all CVs in mesh B, only CVs
in VSBs that contain at least one receiver CV must be considered in the
following search. In order to find a first candidate donor CV in mesh A for
a particular receiver CV in mesh B, the search space in mesh A is reduced
by locating the VSB in mesh A, which contains the centroid of the receiver
CV of mesh B. Figure 4.6 only shows one receiver CV of mesh B (orange
CV) and the corresponding VSB of mesh A (red VSB) that contains its
52
centroid. This VSB localization is an easy and computationally inexpensive task due to the Cartesian structure of the VSBs. Also neighboring
VSBs might embody donor CVs, which could contribute to the interpolation and, thus, adjacent VSBs are included in the following donor search
as well. At this point, the donor search for a particular receiver has been
reduced from all VSBs and their corresponding CVs to a handful of CVs
in mesh A.
Figure 4.6: VSB of the donor mesh (red outline) containing the CV centroid
coordinates of the receiver CV (orange).
From now on it is to distinguish between donor CVs, which will be used
for the final interpolation, and pseudo donor CVs. The latter ones are
only used to obtain a continuous fringe of donor CVs in mesh A and will
not contribute to the interpolation. The identification of those donors is
initiated by looping over all CVs in the preselected VSBs. Approximated
axis-aligned Control Volume Bounding Boxes (CVBB) are built around
the receiver CV and each of the candidate donor CVs as seen in Figure 4.7.
53
The receiver CVBB is checked for intersections with each of the candidate
donor CVBBs and if an intersection exists, the donor CV is flagged as
a pseudo donor CV intersecting the receiver CV in space. Referring to
(a)
(b)
Figure 4.7: CV intersection check: (a) Intersecting receiver and donor CV;
(b) Intersecting receiver and donor CVBBs.
Figure 4.7, the CVBBs are defined by two extreme points amin and amax ,
where amin
≤ amax
, ∀i ∈ x, y, z. The CVBB intersect if they overlap in x
i
i
or y or z and, thus, if the following inequality is satisfied:
amin
> bmax
i
i
or
bmin
> amax
i
i
f or each i ∈ x, y, z.
(4.1)
Simultaneously the donor CV that contains the receiver centroid is identified by conducting a dot-product between each face normal vector ~n and
the distance vector ~c (see Figure 4.8). The centroid of the receiver CV lies
54
(a)
(b)
Figure 4.8: Check if CV encloses centroid: (a) Intersecting receiver with
centroid and donor CV; (b) Dot product between face normal vector ~n and
distance vector ~c .
inside the donor CV if the following inequality is satisfied for each face i:
n~i · ~c < 0.
(4.2)
To assure that each donor CV physically qualifies for the interpolation,
only the donor CV containing the receiver CV centroid and its adjacent
neighbors are further considered as possible interpolation donors. The
final interpolation donors are chosen based on a dot-product check between
the vector ~rD and the vectors ~rni , respectively. As seen in Figure 4.9,
the vector ~rD gives the direction from the receiver centroid to the donor
CV centroid containing the receiver centroid and the vectors ~rni give the
direction from the receiver centroid to the adjacent centroids of the donor
55
CV containing the receiver centroid. The angle between vector, ~rD , and
Figure 4.9: Identification of potential donors adjacent to the initial donor
node containing the receiver center point coordinates.
each neighbor vector, ~rni , is calculated according to Equation 4.3. Nodes
that are outside of a specified angle (90◦ in Figure 4.9) are flagged as
interpolation donors.
cos ^(~rni , ~rD ) =
~rni · ~rD
.
|~ni ||~rD |
(4.3)
Donor nodes that are validated by the dot-product check are most qualified
for the interpolation because only donor nodes close to the receiver CV
are chosen to maintain donor quality. Figure 4.10 shows a slice through
the center of mesh A. One layer receiver CVs from mesh B (circular CVs
in orange) are superimposed on mesh A. Its corresponding donor CVs are
56
Figure 4.10: Slice through the center of mesh A with superimposed receiver
CVs of mesh B.
emphasized in red. Figure 4.10 also shows receiver CVs of mesh A three
layers distant from the donor CVs. A two-way coupling is necessary so
that the background mesh also obtains flow solution data from the overset
mesh to account for its own flow solution. The region between the donor
and receiver CVs of mesh B is a buffer layer, such that no CV can be both
a donor and receiver. CVs of the background mesh that are overlapped by
a particular mesh with a higher priority and are not tagged as a receiver
node or located within the buffer layer are ’blanked‘ out as hole points.
The donor search for the receiver CVs in mesh A has to be repeated for
the opposite direction. The results can be seen in Figure 4.11, which
57
shows a slice through the center of mesh B. One layer of receiver CVs of
mesh A is superimposed on mesh B and its corresponding donor CVs are
emphasized in red.
Figure 4.11: Slice through the center of mesh B with superimposed receiver
CVs of mesh A.
A quarter segment of mesh A and a superimposed segment of the receiver
CVs of mesh B are illustrated in Figure 4.12. Figure 4.13 shows half of
the domain of the entire overset system. To better illustrate the receiverdonor relationship, parts of the CVs are made transparent.
The same procedure described above is also used to create a mesh connectivity between unstructured cells or a mix of unstructured and structured
58
Figure 4.12: A segment of a structured background and overset mesh showing
donors, receivers, buffer layer and, hole points.
cells. Figure 4.14 shows a segment of an unstructured background mesh,
which is superimposed by an unstructured overset mesh.
4. Interpolation
For interpolation, the Inverse Distance Weighting (IDW) method is used
due to its easy implementation in computer codes and cheap computational costs. In the IDW method, the weight of the donors decreases with
the distance from the receiver node. The IDW interpolation is defined
as [44]:
λ(S0 ) =
n
X
ψ λ(S )
Pin i ,
j=1 ψj
i=1
59
(4.4)
Figure 4.13: Cross section of the three dimensional domain showing donors,
receivers, and calculated CVs of both meshes.
where
ψi =
1
.
d(S0 , Si )p
(4.5)
The value λ at a node S0 (receiver node) is calculated by summing up the
weighted values of all donor nodes λ(Si ) and dividing them by the sum
of all interpolation weights. The weights ψi are calculated as the inverse
of the distance d(S0 , Si ) between the receiver and donor nodes with an
exponent p defining the influence of a donor node based on its distance
to the receiver nodes. Greater values of p assign higher weights to the
nearest points to the receiver node, whereas smaller values of p assign
higher values to the points far away from the receiver node. [44]
60
Figure 4.14: A segment of an unstructured background and overset mesh
showing donors, receivers, buffer layer, and calculated CVs.
61
Chapter 5
Validation of EXN/Aero
A flow over a backward facing step is a widely used configuration for the
validation of turbulence models. The computational domain and applied
boundary conditions are presented in Section 5.1. In Section 5.2 follows a
validation of the flow results against experimental and computational data.
5.1
Fluid Domain and Boundary Conditions
The backward step as seen in Figure 5.1 resembles the sharp edge at the
aircraft wing tip and thus serves as a well understood test case to validate
the turbulence model used in the aircraft simulation presented in Chapter 6.
Data of the tunnel geometry and boundary conditions are given in Table 5.1
and 5.2. At the inlet, a velocity inlet profile is applied which leads to a
reference velocity Uref = 44.2m/s at the center of the channel near x/H =
62
−4. The skin friction coefficient and pressure coefficient are calculated with
τw
1
2
ρUref
2
(5.1)
pw − pref
1
2
ρUref
2
(5.2)
Cf =
and
Cp =
where reference values are taken near the location x/H = −4. Studies by
Lien et al. [45] showed that a minimum entrance length of 130Y0 is required
for the flow to be fully developed. In the current case an entrance length
of approximately 148Y0 is used, which corresponds to the recommended entrance length of 150Y0 [45].
Figure 5.1: Schematic of the backward facing step.
Figure 5.2 shows the mesh topology at the vicinity of the step. The
63
Table 5.1: Flow geometry of the backward-facing step problem.
Step height
Channel height
Tunnel span
Entrance length
Exit length
H = 0.0127m
Y0 = 8H
z = 12H
xinl = 147.6H
xexit = 25H
Table 5.2: Boundary conditions of the backward facing step problem.
ρ = 1.185kg/m3 ; µ = 1.831 · 10−5
u ≡ inlet profile ;v = w = 0
k ≈ 13m2 /s2 ; ≈ 9795m2 /s3 )
Outlet (east)
zero pressure p = 0
Wall (north, south)
u=v=w=0
Symmetry (top, bottom) zero normal velocity and pressure
∂f /∂n = 0)
Boundary layer thickness δBL = 0.019m
Reynolds number
ReH ≈ 36, 000
Fluid properties
Inlet (west)
mesh topology resembles the same mesh structure, which is also used for
the simulation of the air tractor, especially in the region where the wing tip
vortices are predicted (see Figure 6.8 for a comparison of the meshes). The
boundary layer flow is predicted with a prism inflation layer, which smoothly
transitions into a tetrahedral mesh moving away from the boundary. The y +
values are similar to those obtained at the wing surfaces of the air tractor
simulation in Chapter 6 and vary at around 30.
64
Figure 5.2: Prism inflation layer along the wall, which is transitioning
smoothly into the isotropic tetrahedral mesh away from the wall.
5.2
Flow Result, Verification and Validation
Figure 5.3 shows the turbulent kinetic energy contours and velocity vectors
downstream of the step. A flow separation occurs after the step, leading to a
recirculating flow, which in turn generates a smaller eddy in the corner of the
step. The velocity vectors also show the point of reattachment further downstream of the step. The reattachment point as well as the pressure coefficient
Cp and the skin friction coefficient Cf are used in the following to validate
the implementation of the k − ω model. Figure 5.4 shows a comparison of
the skin friction coefficient between the measured data of Driver [35] and the
numerical data obtained with EXN/Aero. The data is in good agreement
before the step and is underpredicted straight after the step. In the region
of the reattachment of the flow (x/H ≈ 6.3), the skin friction is in excellent
agreement with the experimental data and slightly underpredicted further
downstream until the flow starts to recover and to develop its typically flat
65
Figure 5.3: Turbulent kinetic energy contours and velocity vectors in the
region after the step.
parabolic u-velocity profile for turbulent channel flows. The results are in
good agreement with numerical results obtained with the original Wilcox
(1988) k − ω model given in Wilcox [46]. Figure 5.5 shows a comparison of
the pressure coefficient near the step between the measured data [35] and the
numerical results from EXN/Aero. Note, that the data is shifted so that Cp
is 0 near the position x/H ≈ 40. The experimental data is in good agreement
with the numerical results. The underprediction of Cp straight after the step
is consistent with results obtained with the original Wilcox (1988) k − ω
model in Wilcox [46]. An even better prediction of Cp has been obtained
further downstream of the step (x/H > 15) in comparison to the numerical
results provided in Wilcox [46].
Figure 5.6 shows a close-up of the near wall region downstream of the
step where the reattachment takes place. The vectors show a scaled velocity field and the reattachment point is emphasized where the skin friction
66
Figure 5.4: Skin friction coefficient Cf as a function of the channel length
x/H.
coefficient has a value of 0. The k − ω model predicts the reattachment at
6.22H which is in good agreement with the measured value of 6.26H [35]
which corresponds to a difference of 0.64%.
Figure 5.7 shows a comparison of the normalized u-velocity profile
across the channel height at the upstream location x/H = −4. It should
be noted that the channel flow obtained from experiment was not fully developed at the given reference location. This might cause smaller deviations
between the numerical and experimental results such as noticeable for the
u-velocity between 1.5H and 4H. The underprediction of the upstream uvelocity profile also impinges the u-velocity profile above y/H > 1 at different
locations downstream of the step as seen in Figure 5.8. The u-velocity is also
underpredicted at x/H = 4, 6 and 10 at the area of recirculation. The same
deviations in this region were also obtained in Reference [47] with the Wilcox
67
Figure 5.5: Pressure coefficient Cp as a function of the channel length x/H.
2006 k −ω model. Discrepancies are noticeable at x/H = 1 at the area where
the recirculating flow interacts with the corner as seen in Figure 5.3. The
profiles indicate that the corner eddy is slightly underpredicted in its length.
68
Figure 5.6: Reattachment at 6.22H downstream of the step.
Figure 5.7: Normalized u-velocity profile over the channel height y/H at
x/H = −4 upstream of the step.
69
Figure 5.8: Normalized u-velocity profile over the channel height y/H at
different locations downstream of the step; x/H = 1, 4, 6 and 10.
70
Chapter 6
Single Mesh AT802 Air Tractor
Study
A sketch of the aerial spraying domain and the depicted arrangement of
the overset mesh system was shown in Figure 1.4 and 1.6. In this chapter,
the near-field mesh enclosing the air tractor is evaluated. The air tractor
geometry, the computational domain, boundary conditions and solutions are
demonstrated. The single mesh simulation should confirm the model’s ability
to reproduce physics and thus its assignment as a moving overset mesh at
later date. The flow results obtained with EXN/Aero are verified against
solutions obtained from the commercial CFD-solver Ansys CFX.
71
6.1
Air Tractor Geometry
Figure 6.1 shows a comparison between the real airtractor AT802 and the
corresponding CAD-model. The dimensions of the model are shown in Fig-
(a)
(b)
Figure 6.1: (a) Air tractor AT802 [1]; (b) CAD-model of the air tractor
AT802.
ure 6.2 and 6.3. The model includes the fuselage, cockpit, wings, and horizontal and vertical stabilizers. Parts of the aircraft geometry which do not
have a significant influence on its aerodynamic, such as the landing gear or
exhaust, are not included in the model to simplify the geometry. For the
current study, the effects of the aircraft’s propeller on the fluid flow are not
considered in the simulation. The propulsion created by the propeller is
much less influential on the flow features behind the aircraft than the large
influence of the wing and fuselage geometry. If needed, linear and angular
momentum sources can be added to the domain to account for the propulsion
created by the propeller. Adding momentum sources reduces the computational costs in comparison to modeling the moving blades. A simplified blade
element momentum theory can be used to calculate the momentum source
terms as described in Appendix A.1.
72
Figure 6.2: Air Tractor AT802 geometry (side view). Reproduced from [48].
The wings have a NACA4415 profile with a chord length of 2.08m and
a span of 9.03m measured from the center of the aircraft. The horizontal
stabilizer have a NACA0010 profile with a chord length of 1.07m and a span
of 2.495m measured from the center of the aircraft.
6.2
Fluid Domain and Boundary Conditions
The outline of the computational domain, including the air tractor, is shown
in Figure 6.4. The domain is a rectangular box dividing the aircraft’s body
into two symmetrical halves. External boundary conditions will be applied
on the faces of the box. The box spans three aircraft lengths L ≈ 11m in front
of the aircraft and 21L behind the aircraft. It spans approx. 2.2L above,
approx. 1.8L below and 4L on the left side of the aircraft. The coordinate
system is placed at the centroid of the fuselage (x, y, y) where the x − axis
points to the trail of the aircraft, the y −axis points to the roof of the cockpit
and z − axis points to the port of the aircraft.
The domain has six external boundary conditions and one internal
73
Figure 6.3: Air Tractor AT802 geometry (top and front view ). Reproduced
from [48].
boundary condition, which is the aircraft’s body. The six external boundary
conditions are the faces of the external box and are named relative to the
axis of the coordinate system. The face intersecting the positive direction of
the x − axis is named +xf and its opposite face −xf . The same notation is
applied for the y− and z−axes, which gives the faces +yf , −yf , +zf and −zf .
The corresponding boundary conditions are given in Table 6.1. The external
face −xf is given a velocity equal to the aircraft speed in a direction parallel
to the x − axis. Since there are no cross-winds applied and the geometry of
the aircraft is symmetric about the x − y plane, a symmetric solution can
74
Figure 6.4: Air Tractor AT802 wireframe view. The aircraft length L ≈ is
approximately 11m.
be assumed about the x − y plane. Following, a symmetry plane is applied
at the −zf boundary, which significantly reduces the number of calculation
per iteration. The boundary xf is defined as an outlet and the remaining
boundaries are defined as symmetry boundaries.
Table 6.1: Boundary conditions of the computational domain.
Fluid properties
ρ = 1.185kg/m3 ; µ = 1.831 · 10−5 P a · s
Boundary surface
Boundary Condition
Internal aircraft surface
−xf
Smooth surfaces (u = v = w = 0)
Inlet (u = 69.44m/s; v = w = 0
k = 0.0001; = 0.0003)
Outlet (zero pressure p = 0)
Symmetry plane (zero normal velocity and pressure
∂f /∂n = 0)
xf
yf , −yf , zf , −zf
75
6.2.1
Mesh Sensitivity Study
A mesh sensitivity study for a similar computational domain and boundary
conditions was performed by Ryan et al. [7]. Differences between Ryan’s
computational domain and the current study are an extended far-field mesh
(6L) on the right side of the air tractor, a full-domain simulation and the use
of solely unstructured CVs. Ryan et al. concluded that a mesh containing
31.67 million CVs is sufficient to make the solution independent of the mesh
size. This corresponds to approximately 15.8 million CVs for half of the domain size. Ryan used a prism inflation layer, containing 4.4 million elements
(full domain), which yield y + values in the range of around 200 − 600 for
the wings and stabilizer of the air tractor. For the current study, the y +
values were reduced by increasing the number of CVs within the boundary
layer. Following, a simulation was performed using maximal y + values for
the wings of 90. This led to a mesh refinement within the inflation layer
yielding 7.8 million prism elements based on a full-domain simulation. The
mesh topology is shown in the following section.
6.2.2
Mesh Topology
R
For the simulations a hybrid mesh (created with Pointwise
) is used. A
summary of the types and numbers of elements used is given in Table 6.2.
A plane located at the centerline of the air tractor’s fuselage normal to the
z −axis (see Figure 6.5) shows the unstructured near-field mesh enclosing the
76
air tractor and the structured far-field mesh. The reason for this mesh-type
Figure 6.5: Plane at the centerline of the air tractor’s fuselage normal to the
z − axis showing the hybrid mesh structure.
switch is to gain solution efficiency. Structured meshes increase computational efficiency on parallel computing resources and thus are a better choice
in regions where no near-body meshing is required and the flow has stabilized
into some regular regime (such as wingtip vortices). The surface of the solid
air tractor body is entirely represented by an unstructured mesh as illustrated in Figure 6.6. An anisotropic mesh structure is used to avoid faceting
at the leading and trailing edges of the wing and stabilizer geometry. Boundary layer flows in the near-field mesh around aircraft wing and stabilizer are
77
Figure 6.6: Air Tractor AT802 surface mesh. Unstructured surface mesh with
anisotropic extrusion at the wing and stabilizer leading and trailing edge.
solved using an inflation layer - an unstructured, prism mesh that provides
good shear stress and separation prediction. Detailed understanding of the
airflow around the wings is paramount for these simulations because the wing
geometry has a strong effect on the dispersion of spray drops in the wake of
the aircraft. Figure 6.7 shows a section of the inflation layer on the wing
of the aircraft. The prism elements grow with the distance away from the
surface and transition smoothly into the isotropic tetrahedral far-field mesh
as shown in Figure 6.8.
78
Figure 6.7: Anisotropic surface mesh at the trailing edge of the wing with a
section showing the prism inflation layer.
Table 6.2: Number and types of elements of the air tractor mesh.
Tetrahedral
Hexahedral
Pyramid
Prism
Total CVs
Total Points
79
6,195,022
12,259,900
146,638
7,837,622
26,439,182
8,925,029
Figure 6.8: Prism inflation layer around the wing smoothly transitioning into
the isotropic tetrahedral far-field mesh.
80
6.3
Flow Results and Verification
The air tractor AT802 creates a wake including wingtip vortices, which significantly influence the spray distribution of spray droplets. As described by
Green [49], the generation of wing-tip vortices can be explained in various
ways. A descriptive way focuses on the pressure difference above and below
the wing, which occurs when a lifting area such as a wing causes a net deflection or turning of the oncoming flow. In that case, air accelerates around
the wing tip due to the pressure difference between the upper and lower wing
surfaces initiating the creation of a wing tip vortex. Figure 6.9 shows the
velocity streamlines and the pressure contours. The upstream streamlines in
Figure 6.9: Velocity streamlines showing the upward movement before and
the downward movement behind the wing.
the vicinity of the leading edge experience an upward movement as a result
of the wing shape. The shape of the wing forces the flow to deflect and turns
it into a downward movement on its way over the surface. The evolution
81
of a wingtip vortex at different locations downstream of the leading edge is
shown in Figure 6.10 and the roll-up process further downstream is illustrated in Figure 6.11. In Figure 6.11 the color of velocity streamlines show
Figure 6.10: Velocity vectors showing the wake vortex evolution in the vicinity of the wing. The color contours show the turbulent kinetic energy magnitude; a) x/c = 0.7 b) x/c = 0.95 c) x/c = 1.19 d) x/c = 1.44
the vorticity magnitude. It can be seen how the vorticity is generated within
the turbulent boundary layer and rolls up into a single vortex further downstream. The vorticity is highest at the tip of the wing where a separation
of the boundary layer takes place. The streamlines traversing the wingtip in
span-wise direction will build the core of the vortex and are responsible for
the high amount of vorticity in the vortex center straight behind the trailing
edge. Figure 6.10 also shows the high amount of turbulent kinetic energy at
the vortex core, which relaminarizes further downstream of the trailing edge.
The generated rotation of the fluid around the initial vortex center produces
82
Figure 6.11: Velocity streamlines showing the wake vortex evolution and the
the roll-up process. The color contours show the vorticity magnitude.
a lower pressure around the core forcing the fluid to swirl around the core.
The low pressure cores at different locations at and after the wing tip area
are shown in Figure 6.12 as well as the streamlines building the vortex core
straight after the wing region. Figure 6.13 shows the beginning of the vortex
Figure 6.12: Pressure distribution at different locations downstream of the
leading edge at x/c = 0.7, 1.09, 1.43 and 1.92.
formation and the related boundary layer separation. The picture on the
right hand side shows the velocity streamlines at the wingtip with the color
83
contours indicating the magnitude of the z-component of the velocity. The
red contours of the streamlines at the wingtip surface indicate a fluid flow
from the inside of the wing towards the wingtip, which occurs after a flow
separation perpendicular to the axial velocity. The starting point of boundary layer separation can also be located due to the lower surface pressure as
seen in the left picture of Figure 6.13. The appearance of flow separation is
evident when the axial vorticity (ωx ) is plotted on a plane cutting through
the wing normal to flow direction at x/c = 0.95 as shown in Figure 6.14.
The negative vorticity layer (blue contours) generated in the boundary layer
of the high pressure side (lower surface) smoothly travels over the tip and
thickens on its pass towards the top of the tip. The thickening is caused by a
decrease of the driving pressure gradient. This boundary layer vorticity sheet
acts as a feeding sheet of the wingtip vortex. Simultaneously, the tip vortex
induces a velocity in span-wise direction to the boundary layer attached to
upper wing surface in the vicinity of the tip. This creates a secondary vortex
counter-rotating with the tip vortex as indicated by the red vorticity contours. The same appearance of a secondary vortex has also been observed
by others, including Devenport et al. [50].
Some of the results are verified via a comparison to the results from
the commercial CFD-software Ansys CFX V.14.5. Figure 6.15 shows Cp
contours on the wing surface of the EXN/Aero solution and a comparison of
Cp profiles and different locations along the wing in span-wise direction. The
x-values are shifted so that x/c = 0 represents a point at the leading edge and
84
Figure 6.13: Velocity streamlines showing the vortex evolution and boundary
layer separation. The color contours show the pressure distribution at the
left and the z-component of the velocity at the right picture.
x/c = 1 represents a point at the trailing edge of the wing. Also, the spanwise y position of the planes intersecting the wing are shifted so that y/b = 0
represents a point at the surface of the fuselage and y/b = 1 is at the tip of
the wing. Solutions of all plane locations as indicated in Figure 6.15 are given
in the Appendix A.2. At the stagnation point at the leading edge at x/c = 0,
the pressure is equivalent to dynamic pressure at the free-stream area, which
leads to a Cp value of 1. Following a path from the stagnation point along
the upper surface of the wing, a steep decrease of Cp can be noticed due to
the decreasing pressure reaching a minimum at the lowest surface pressure
at the first quarter of the wing. From this point on, Cp increases until the
upper surface pressure reaches the pressure value from the high pressure side
(lower wing surface) at the trailing edge. Also a pressure drop along the
wing surface, starting from the fuselage and traveling towards the wing tip,
can be observed due to the pressure compensation at the wing tip. Excellent
agreement of Cp and thus the pressure distribution can be noted between the
85
Figure 6.14: Axial view of the vortex evolution and boundary layer separation
at the chord wise location x/c = 0.95. The color contours show the axial
vorticity indicating the evolution of the tip vortex.
two solutions. A comparison of the tangential velocity vectors and contours of
the vorticity at planes located 10m, 50m, 100m and 200m downstream of the
aircraft are prepared in Figure 6.16 and 6.17. Both solutions are in excellent
agreement. The same plane locations are also used to compare the turbulent
kinetic energy between the two CFD-solver (see Figure 6.18 and 6.19). The
turbulent kinetic energy of the EXN/Aero solution is in good agreement
with the CFX solution but slightly larger indicating the EXN/Aero code to
be slightly less dissipative.
The drag and lift force of the aircraft is also compared between the
two CFD-solutions. A lift force of 61.48kN was obtained with EXN/Aero
which shows a discrepancy of 3.6% when compared to the lift force (59.32kN )
86
Figure 6.15: The wing surface is showing the Cp contours and the figures show
a comparison of the Cp values between the EXN/Aero and CFX solutions at
different span-wise positions (y/b = 0.15, y/b = 0.49 and y/b = 0.88).
obtained with Ansys CFX. Less well conformity is obtained for the drag of the
aircraft, which deviates by 9.3% between the EXN/Aero solution (3.61kN )
and the Ansys CFX solution (3.3kN ).
87
Figure 6.16: Vorticity contours and mean velocity vectors at 10 and 50 meters
planes downstream of the air tractor.
88
Figure 6.17: Vorticity contours and mean velocity vectors at 100 and 200
meters planes downstream of the air tractor.
89
Figure 6.18: Turbulence kinetic energy contours and mean velocity vectors
at 10 and 50 meters planes downstream of the air tractor.
90
Figure 6.19: Turbulence kinetic energy contours and mean velocity vectors
at 100 and 200 meters planes downstream of the air tractor.
91
Chapter 7
Testing the Overset Meshing
Algorithm
Another commonly used problem for the validation of CFD-codes is the sliding lid cavity problem. In the following, three different mesh configurations
are used to evaluate the overset mesh connectivity algorithm. The mesh
topology of each individual case is illustrated in Section 7.1 and their boundary conditions are described in Section 7.1.1. For one of the cases a mesh
sensitivity study is performed (Section 7.3) and results for all three cases are
shown in Section 7.2. A validation against experiment is done in the last
Section.
92
7.1
Fluid Domain and Boundary Conditions
In the following, three individual mesh systems are applied. The shape of
the background and superimposed overset meshes are unaltered, however, the
mesh types and resolutions of each individual case are altered. The sliding
lid problem in this case is a three-dimensional box that has a moving wall at
the north face (n), stationary no-slip walls at the west, east and south faces
(w, e and s), and symmetry planes on the top and bottom faces (t and b)
as illustrated in Figure 7.1 and summarized in Table 7.1. The side lengths
Figure 7.1: Sliding lid fluid domain and boundary condition.
L = 1m of the background mesh and the lid velocity u = 1m/s are kept
constant for all conducted simulations. The superimposed overset mesh has
the form of a cylinder and is placed in the center of the background mesh
and does not touch any of the end walls. The Reynolds number is altered by
93
modifying the properties of the fluid.
Table 7.1: Boundary conditions of the computational domain.
Boundary surface
Boundary Condition
Fluid properties
µ = 0.1P a s
Re = 100: ρ = 10kg/m3
Re = 400: ρ = 40kg/m3
Re = 1000: ρ = 100kg/m3
Smooth surfaces (u = v = w = 0m/s)
Moving wall (u = 1m/s; v = w = 0m/s)
Symmetry plane (zero normal velocity and pressure
∂f /∂n = 0)
w, s, e
n
b, t
7.1.1
Mesh Topology
The first mesh system Sim 1 is an entirely structured mesh composition.
The background mesh consists of uniform Cartesian hex-elements and the
superimposed overset mesh has a cylindrical shape consisting of curvilinear
hex-elements. The second mesh Sim 2 has a structured background mesh
equivalent to Sim 1 and a cylindrical shaped superimposed overset mesh
consisting of unstructured tet-elements. The last mesh Sim 3 is equivalent to
that of Sim 1 but has a solid core in the overset mesh center. The individual
mesh systems are shown in Figure 7.2.
94
Figure 7.2: Sliding lid overset mesh systems; structured overset mesh (Sim1),
unstructured overset mesh (Sim2) and structured overset mesh with solid
core (Sim3).
7.1.2
Mesh Sensitivity Study
A mesh sensitivity study was performed using the structured background
mesh at a Reynolds number of 400. Alternations of the primary vortex
center and the size of the secondary vortex in the lower right corner were
compared between the meshes counting 64, 100 and 150 CVs in each of the
three coordinate directions, respectively. Table 7.2 and 7.3 show the position
of the primary vortex center and the length of the secondary vortex in the
lower right corner. The discrepancies between the coarsest and the medium
mesh are in good agreement and there only infinitesimal differences noticeable
in the solution between the medium mesh and finest mesh. This leads to the
conclusion that a mesh with 100 CVs in each coordinate direction is sufficient
to obtain solutions independent of the mesh size. In the following discussion,
three-dimensional results are shown in a two-dimensional plane normal to the
y-axis at y = 0.5m cutting through the geometric center of the domain. For
95
Table 7.2: Alternations of the primary vortex center location between different mesh sizes.
Mesh size (CVs per dimension)
64
100
150
x
y
z
0.539 0.5 0.601
0.545 0.5 0.603
0.544 0.5 0.603
Table 7.3: Alternations of the secondary vortex length (vertical attachment
length) between different mesh sizes.
Mesh size (CVs per dimension)
64
100
150
length in m
0.328
0.331
0.332
reasons of clarity, the top picture of Figure 7.3 shows a cut through the
geometric center of the domain (x − z plane) and the bottom picture shows
typical velocity streamlines at the same plane. The moving lid creates a
primary vortex with a center that is offset towards the top right corner and
recirculating secondary vortices in the lower left and right corner and as well
to some extent in the upper left corner. A comparison of the size and center
location of the vortices provide a good validation and thus these features are
used for the validation of the overset implementation.
96
Figure 7.3: Parameters and conventions used for the validation of the sliding
lid problem. Three dimensional results are shown on a plane normal to the
y-axis at y = 0.5m (at the center of the domain).
7.2
Flow Results
The spanwise invariant steady state velocity field (Sim 1) for a laminar flow
with a Reynolds number of Re = 400 is shown in Figure 7.4. The left side
shows the overset mesh positioned beside the background mesh and the right
side shows a composition of both meshes. The solutions shown in Figure 7.5
are identical to the ones in Figure 7.4 due to the same boundary conditions;
however, the overset mesh is unstructured (Sim 2). It is clearly demonstrated
97
Figure 7.4: Three-dimensional sliding lid (Sim 1) velocity field at a plane
normal to the y-axis at y = 0.5m. Showing the overset mesh positioned
beside the background mesh (left side) and the composite mesh (right side);
Re = 400.
that in both cases the flow features are able to seamlessly pass between the
background and minor meshes. Sim 3 differs from the previous solutions
due to its solid core in the overset mesh. The shape of the solid obstacle
is chosen arbitrarily but could have any form such as that of the aircraft
shown in Chapter 6. As seen in Figure 7.6, the flow passes freely between
the mesh systems and the no-slip wall boundary condition of the core surface
effects the flow field around it. Another representation of the velocity field of
Sim 3 is shown Figure 7.7. Here, a section of the overset mesh (red) and the
coarser background mesh (black) are shown at a plane normal to the z-axis
at z = 0.5m.
98
Figure 7.5: Three-dimensional sliding lid (Sim 2) velocity field at a plane
normal to the y-axis at y = 0.5m. Showing the overset mesh positioned
beside the background mesh (left side) and the composite mesh (right side);
Re = 400.
Figure 7.6: Three-dimensional sliding lid velocity field (Sim 3) at a plane
normal to the y-axis at y = 0.5m including a solid core. Showing the overset
mesh positioned beside the background mesh (left side) and the composite
mesh (right side); Re = 400.
99
Figure 7.7: Three-dimensional sliding lid velocity field (Sim 3) at a plane
normal to the y-axis at y = 0.5m including a part of the overset mesh (red)
and the coarser background mesh (black).
100
7.3
Verification and Validation
Results of the u and v velocity profiles along a vertical and horizontal line
passing through the geometric center of the cavity under different levels of
mesh refinement are shown in Figure 7.8 and 7.9, respectively. The level
of mesh refinement can be taken from the figure legend, which refers to the
number of CVs in a two-dimensional plane. The mesh resolution of the
overset mesh is adjusted based on the resolution of the background mesh so
that it remains finer and increases with the background mesh resolution.
Figure 7.8: v-velocity results along horizontal line through geometric center
of cavity.
Figure 7.8 shows that the solution strongly depends on the resolution of
the mesh system, which was also observed by Sousa et al. [51]. It can be noted
that there are only minor differences in the solutions between the 64×64 mesh
and the solutions obtained by Ghia et al. [52]. However, the velocity peaks of
101
Figure 7.9: u-velocity results along a vertical line through geometric center
of cavity.
the EXN/Aero solutions increase when the mesh is further refined. There is
no noticeable difference between the two fine meshes (100×100 and 150×150)
which leads to the conclusion that the EXN/Aero solution is independent of
the grid size for meshes with a finer resolution than 100 × 100. The same
result was also observed in Section 7.1.2 for single non-overset meshes.
A closer look at the velocity profiles at the distances x ≈ 0.3 and 0.7
discloses the area of the mesh system where both meshes are overlapped
and solved parallel. The transitions between the two different solutions sets
are smooth and are in very good agreement with the single mesh solutions
of Sousa [51] and Ghia [52]. Figure 7.11 shows a comparison between the
overset meshes Sim1, Sim2, a non-overset mesh and a two-dimensional mesh
with the same mesh size. There are no discrepancies recognizable between
the different mesh types. The same findings are obtained when examining
102
Figure 7.10: v-velocity results along a horizontal line through geometric center of cavity.
Figure 7.9 and 7.11. The meshes used here are identical to the one used in
Figure 7.8 and 7.9, though, the results for the u-velocity along a horizontal
line through the geometric center of the cavity are shown.
As mentioned before, one way to validate numerical sliding lid results
against experiments is the comparison of the size of the upstream corner vortex at different Reynold numbers. A direct comparison to the experimental
data from Pan et al. [53] where vortex reattachment lengths (along the right
vertical boundary) are provided are shown in Figure 7.12. The upstream vortex height d is normalized by the total side height z and plotted as a function
of the Reynols number. The results show an increasing of the recirculating
corner vortex with an increasing Reynolds number up to Re = 500 and a following weakening of the vortices, which is consistent with the experimental
results obtained by Pan et al. [53] and confirmed by Koseff et al. [54] in later
103
Figure 7.11: u-velocity results along a horizontal line through geometric center of cavity.
experiments.
The viscous effects on the primary vortex center are observed by varying the Reynolds number from Re=100 to 1000. As illustrated in Figure 7.13,
the vortex center moves towards the center of the domain as the Reynolds
number increases, which is an expected result and in good agreement with
computational results presented in other publications [51, 52].
104
Figure 7.12: Ratio of the upstream vortex height d to the total side height
z as a function of the Reynolds number. Experimental data from Pan et
al. [53] (blue circles).
Figure 7.13: Location of the primary vortex center as a function of the
Reynolds number. Numerical data from Theodossiou et al. [51] (blue circles).
105
Chapter 8
Conclusion and Future Work
8.1
Conclusion
The major objective of this work was the implementation of an overset capability into the CFD-code EXN/Aero as illustrated in Section 4 and Chapter 7. Overset results from a sliding lid example obtained with EXN/Aero
were validated against experimental and numerical solutions from other publications. The sliding lid example showed, that the flow features are able to
seamlessly pass between the individual meshes. A more precise comparison
was obtained by observing the u− and v−velocity profiles along a vertical
and horizontal line through the geometric center of the cavity. The results
showed a dependence on the mesh size, but were independent of the mesh
type including overset or non-overset mesh systems. Also the location of the
primary vortex center and the size of the upstream vortex height were in good
106
agreement to results from others publications. In conclusion, the overset implementation handles the communication between structured, unstructured
and hybrid static overset mesh systems.
A further substep and objective of this thesis was the validation of the
computational domain used to simulate the flow over the airtractor. This
included a validation of the turbulence model showing its ability to predict
real flow solutions. Therefore, a flow over a backward facing step was examined, which showed a good agreement of the pressure and friction coefficients
between the numerical and experimental data within the bounds of possibility of a two-equation turbulence model. An underprediction of the friction
coefficient within the first 4 step heights downstream of the step, and after
7 step heights until the flow recovers, is a common error of numerical results
obtained with two-equation turbulence models in comparison to experimental data. An underprediction of the pressure coefficient was also observed
at the region of recirculation within the first 3 step heights downstream of
the step. Also, an underprediction of the pressure coefficient after 6 step
heights can be noted, but shows a better agreement with experimental data
in comparison to the numerical results obtained by another CFD-solver. An
excellent agreement could be obtained for the reattachment point at 6.264
step heights downstream of the step.
The last step towards completion of this work, was the verification of
the airtractor domain by comparing the EXN/Aero results with that from
the commercial CFD-software Ansys CFX V.14.5. The pressure distribution
107
over the wing surface was evaluated by comparing the pressure coefficients
at different regions along the span-wise direction of the wing. An excellent
agreement of the pressure coefficient Cp could be noted between the two
solutions at all span-wise positions. Also, the tangential velocity vectors
and contours of the vorticity at planes located 10m, 50m, 100m and 200m
downstream of the airtractor were compared. Both solutions are in excellent
agreement. The same locations were also used to compare the turbulent kinetic energy, which is in good agreement with the CFX solution but slightly
larger, indicating that the EXN/Aero code is slightly less dissipative. The
drag and lift force of the airtractor was also compared between the two CFDsolutions. A lift force of 61.48kN was obtained with EXN/Aero, which shows
a discrepancy of 3.6% when compared to the lift force (59.32kN ) obtained
with Ansys CFX. There is a less desirable correlation for the drag of the aircraft which has a deviation of 9.3% between the EXN/Aero solution (3.61kN )
and the Ansys CFX solution (3.3kN ).
8.2
Future Work
Both, the implementation of an overset methodology in EXN/Aero and the
demonstration of an aircraft simulation contribute to the goal of the research
program. With this foundation laid, the next step will be the usage of the
overset methodology in combination with the aircraft simulation. In order
for the aircraft’s near-body mesh to move relative to a background mesh, the
108
overset mesh methodology has to be extended so that moving meshes are
supported. Further steps should focus on a more realistic representation of
the aerial spraying domain, which requires the implementation of additional
sub-models and adjusted boundary conditions.
One of these sub-models should represent the complex ground topography with real forest canopies. The influence of the canopy model on the
fluid flow can be defined by porosity and leaf area density distribution. Another sub-model must account for the propulsion created by the propeller.
Momentum sources for such a model can be obtained with the blade element
theory as described in Appendix A.1.
The aircraft simulation in this thesis did not account for a true representation of atmospheric ground effects as found in nature. This can be
improved by adjusting the inlet conditions of the fluid domain by using a
velocity profile and realistic turbulence inlet conditions at the inlet domain.
Although the aircraft’s fuselage has a rather minor influence on the flow
features behind the aircraft in comparison to the wings, a mesh refinement at
the fuselage’s surface in terms of a prism inflation layer can help to improve
the prediction of the boundary layer, and thus its effect on the fluid flow.
109
Bibliography
[1] Air Tractor Inc. Air tractor. olney. /www.airtractor.com/sites/
default/files/wallpapers/1024/Air-Tractor-1024x768-6.jpg,
2012. retrieved 01 Jan. 2013.
[2] M. E. Teske, S. L. Bird, D. M. Esterly, T. B. Curbishley, S. L. Ray,
and S. G. Perry. Agdrift: A model for estimating near-field spray
drift from aerial applications. Environmental Toxicology and Chemistry,
21(3):659–671, 2002.
[3] A. J. Bilanin, M. E. Teske, J. W. Barry, and R. B. Ekblad. Agdisp:
The aircraft spray dispersion model, code development and experimental
validation. Trans. ASABE, 32(1):327–334, 1989.
[4] M. E. Teske, H. W. Thistle, and G. G. Ice. Technical advances in modeling aerially applied sprays. Trans. ASABE, 46(4):985–996, 2003.
[5] M. E. Teske, H. W. Thistle, and R. J. Londergan. Modification of droplet
evaporation in the simulation of fine droplet motion using agdisp. Trans.
ASABE, 54(2):7417–421, 2011.
110
[6] M. E. Teske, H. W. Thistle, W. C. Schou, P. C. H. Miller, J. M. Strager,
B. Richardson, M. C. Butler Ellis, J. W. Barry, D. B. Twardus, and
D. G. Thompson. A review of computer models for pesticide deposition
prediction. Trans. ASABE, 54(3):789–801, 2011.
[7] S. D. Ryan, A. G. Gerber, and G. L. Holloway. A computational study
on spray dispersal in the wake of an aircraft. Trans. ASABE, 56:847–868,
2012.
[8] J. H. Ferziger and Peric M. Computational Methods for Fluid Dynamics.
Springer, Berlin, 3rd, rev. edition, 2002.
[9] J. L. Steger, F .C. Dougherty, and J. A. Benek. Chimera grid scheme.
volume 5, pages 59–69, 1983.
[10] Z. J. Wang and V. Parthasarathy. A fully automated chimera methodology for multiple moving body problems. Int. J. Numer. Meth. Fluids,
33:919–938, 2000.
[11] J. Bonet and J. Peraire. An alternating digital tree (adt) algorithm for
3d geometric searching and intersection problems. International Journal
for Numerical Methods in Engineering, 31:1–17, 1991.
[12] M. Aftosmis. Solutions adaptive cartesian grid methods for aerodynamic flows with complex geometries. von Karman Institute for Fluid
Dynamics Lecture Series 1997-02, 28th Computational Fluid Dynamics,
1997.
111
[13] N. C Prewitt, D. M. Belk, and W. Shyy. Parallel computing of overset grids for aerodynamic problems with moving objects. Progress in
Aerospace Sciences, 32:117–172, 2000.
[14] R. C. Maple and D. M. Belk. Automated set up of blocked, patched, and
embedded grids in beggar flow solver. N. P. Weatherill et al.,editors.
Numerical Grid Generation in CFD and Related Fields., pages 605–314,
1994.
[15] Sush, N. E. and Tramel, R. W. Pegasus 4.0 users’s manual, 1991.
[16] R. L. Meakin. A new method for establishing intergrid communication
among systems of overset grids. In 10th AIAA CFD Conference, pages
662–671, 1991.
[17] G. Chesshire and W. D. Henshaw. Composite overlapping meshes for
the solution of partial differntial equations. J Comput Phys, 90(1), 1990.
[18] R. W. Noack. An octree based overset grid hole cutting method. In Proceedings of 8th International Conference On Numerical Grid Generation
in Computational Field Simulations, pages 783–792, 2003.
[19] R. W. Noack. Resolution appropriate overset grid assembly for structured and unstructured grids. In 16th AIAA CFD Conference, 2003.
[20] R. W. Noack. Suggar: a general capability for moving body overset grid
assembly. In 17th AIAA CFD Conference, 2005.
112
[21] R. W. Noack and D. A. Boger. Improvements to suggar and dirtlib for
overset store separation simulations. In 47th AIAA Aerospace Sciences
Meeting, 2009.
[22] R. W. Noack. Dirtlib: Aa library to add an overset capability to your
flow solver. In 17th AIAA CFD Conference, 2005.
[23] J. Sitaraman, M. Floros, A. Wissink, and M. Potsdam. Parallel domain
connectivity algorithm for unsteady flow computations using overlapping and adaptive grids. Journal of Computational Physics, 229:4703–
4723, 2010.
[24] J. J. Alonso, S. Hahn, F. Ham, M. Herrmann, G. Iaccarino, G. Kalitzin,
P. LeGresley, K. Mattsson, G. Medic, P. Moin, H. Pitsch, J. Schlter,
M. Svrd, E. Van der Weide, D. You, and X. Wu. A high-performance
scalable module for multi-physics simulations.
In 42nd AIAA/AS-
ME/SAE/ASEE Joint Propulsion Conference & Exhibit, 2006.
[25] J. Liu, A. U. Akay, A. Ecer, and R. U. Payli. Flows around moving
bodies using a dynamc unstructured overset-grid method. International
Journal of Computational Fluid Dynamics, 24(6):187–200, 2010.
[26] K. Soni, D. D. J. Chandar, and J. Sitaraman. Development of an overset
grid computational fluid dynamics solver on graphical processing units.
Computer and Fluids, 58:1–14, 2012.
113
[27] D. D. J. Chandar, J. Sitaraman, and D. Mavriplis. A gpu-based incrompressible navier-stokes solver on moving overset grids. Internationala Journal of CFD, 27(6-7):268–282, 2013.
[28] P. A. Davidson. Turbulence - An Introduction for Scientists and Engineers. Oxford University Press, New York, 2004.
[29] H. K. Versteeg and W. Malalasekera. An introduction to computational
fluid dynamics: the finite volume method. Pearson, Prentice Hal, Harlow, 2007.
[30] D. C. Wilcox. Turbulence Modeling for CFD. DCW Industries, Inc., La
Cañada, 1994.
[31] F. R. Menter. Two-equation eddy-viscosity turbulence models for engineering applications. AIAA JOURNAL, 32(8):1598–1605, 1994.
[32] D. C. Wilcox. Reassessment of the scale-determining equation for advanced turbulence models. AIAA Journal., 26(11), 1995.
[33] D. C. Wilcox. Turbulence modeling for CFD, 1st edition. DCW Industries, La Cañada, 1993.
[34] ANSYS Canada Ltd. ANSYS CFX-Solver, Release 14.1: ANSYS CFXSolver Theory Guide. Technical Report.
[35] D. M. Driver. Reynolds shear stress measurements in a seperated boundary layer. AIAA Paper., 91(1787), 1991.
114
[36] M. Kandula and D. C. Wilcox. An examination of k − ω turbulence
model for boundary layers, free shear layers and separated flows. AIAA
Journal., 95-2317:1299–1310, 1995.
[37] P. G. Huang. Physics and computations of flows with adverse pressure
gradients. Modeling Complex Turbulent Flows., pages 245–258, 1999.
[38] B. R. Hutchinson and G. D. Raithby. A multigrid method based on the
additive correction strategy. Num. Heat Transfer, 9:511–537, 1986.
[39] G. A. Gerber, K. W. Wilcox, and J. T. Zhang. Benchmarking of a
massively parallel hybrid cfd solver for ocean applications. In Proceedings
of the ASME 2013 32nd International Conference on Ocean, Offshore
and Arctic Engineering, 2013.
[40] C. L. Rumsey, D. M. A. Poirier, R. H. Bush, and C. E. Towne. A user’s
guide to cgns. 2001.
[41] A. Eghbal, A. G. Gerber, and E. Aubanel. Algebraic multigrid employing mixed structured-unstructured data on manycore hardware. Int. J.
Numer. Meth. Fluids, pages 1–23, 2014.
[42] D. B. Kirk and W. W. Hwu. Programming massively parallel processors:
a hands-on approach. Morgan Kaufmann, Burlington (USA), 2010.
[43] nvidia. Cuda c programming guide, 2015.
115
[44] G.Y. Lu and D. W. Wong. An adaptive inverse-distance weighting spatial interpolation technique. Computer & Geoscience, 34:1044–1055,
2007.
[45] K. Lien, J. P. Monty, M. S. Chong, and A. Ooi. The entrance length
for fully developed turbulent channel flow. In 15th Australasian Fluid
Mechanics Conference, 2004.
[46] D. C. Wilcox. Turbulence Modeling for CFD. DCW Industries, Inc., La
Cañada, 1994.
[47] NASA Langley Research Center. Turbulence modeling resource, 2d
backward facing step validation case. http://turbmodels.larc.nasa.
gov/backstep_val_w06.html, 2014. retrieved 18 Jan. 2015.
[48] Air Tractor Inc. (ed.). Air tractor. olney. /http://www.airtractor.
com/sites/default/files/dimensional-drawings/AT_802A_
dimensional_drawings.pdf, 2012. retrieved 01 Jan. 2013.
[49] S.I. Green. Fluid vortices - Fluid Mechanics and its Applications, volume 30. Kluwer Acadamic Publisher, Dordrecht, 1995.
[50] W. J. Devenport, M. C. Rife, S. I. Liapis, and G. J. Follin. The structure
and development of a wing-tip vortex. J. Fluid Mech., 312:67–106, 1996.
[51] V. M. Theodossiou and A. C. M. Sousa. An efficient algorithm for
solving the incompressible fluid flow equations. International Journal
for Numerical Methods in Fluids, 6:557–572, 1986.
116
[52] V. Ghia, K. N. Ghia, and C. T. Shin. High-re solutions for incompressible
flow using navier-stokes equations and a multigrid method. J. Comp.
Phys., 48:387–411, 1982.
[53] F. Pan and A Acrivos. Steady flows in rectangular cavities. J. Fluid
Mech., 28(4):643–655, 1967.
[54] J. R. Koseff and R. L. Street. Visualization studies of a shear driven
three-dimensional recirculating flow. Journal of Fluids Engineering,
106(21), 1984.
117
Appendix A
Blade Element Theory
A.1
Propeller Sub-domain
The moving blades of the propeller are not modeled to reduce computational
costs. Instead, a propeller blade disk is created (see Figure A.1) where linear
and angular momentum sources (SM t and SM a ) are added to the air that
moves through the propeller blade disk, to account for the propulsion effects
of the propeller. The momentum sources are added to the Momentum Equation (Equation 2.8) as described in Section 2.1. The propulsion created by
the propeller is less influential on the flow features behind the aircraft than
the wing and fuselage geometry and consequently a simplified blade element
momentum theory is used to approximate the momentum source terms. Figure A.2 shows a cross-section of a single propeller blade where the relative
#”
#”
velocity acting on the propeller blade is UR , the aircraft speed is U and the
118
Figure A.1: Propeller blade disk.
#”
#”
#” F
rotational speed of the propeller is ωr.
a and Ft are the axial and tangential
#”
aerodynamic forces. The blade pitch angle is β , the angle between the air
Figure A.2: Propeller blade cross-section with velocities and forces.
#”. The
speed and the blade speed is φ and the effective angle of attack is α
e
#”
#”
lift L and drag D forces acting on the propeller are:
#” 2
#” 1
#”
L = ρCL U R Ap i n
2
119
(A.1)
and
#” 2
#” 1
#”
D = ρCD U R Ap i p
2
(A.2)
#”
#”
where i n and i p are the unit vectors normal and parallel to the relative
velocity, Ap is the planform area of one blade and CL and CD are lift and
drag coefficients. As mentioned above, the propulsion of the propeller has a
relative small influence on the flow featured behind the aircraft and hence the
lift and drag coefficients are approximated, the propeller blades are assumed
to be straight without a twist and the planform area is assumed to be constant
along the propeller blade radius. The lift and drag forces are used to calculate
the total axial and tangential forces acting on the total number of blades by
rotating the axis of interest an angle of β − αe :
SM a =
#” F a VBS
Nblades =
#”
#”
D cos(β − αe ) + L sin(β − αe )
VBS
Nblades
(A.3)
Nblades
(A.4)
and
SM t =
#” F t VBS
Nblades =
#”
#”
L cos(β − αe ) − D sin(β − αe )
VBS
120
A.2
Cp values at the Wing Surface
Figure A.3: Comparison of the Cp values between the EXN/Aero and CFX
solution at different span-wise positions (y/b = 0.15 and y/b = 0.49).
121
Figure A.4: Comparison of the Cp values between the EXN/Aero and CFX
solution at different span-wise positions (y/b = 0.63 and y/b = 0.88).
122
Figure A.5: Comparison of the Cp values between the EXN/Aero and CFX
solution at span-wise position y/b = 0.63.
123
Curriculum Vitae
Daniel Fieger
Education:
• MScEng Student, Department of Mechanical Engineering, University
of New Brunswick, Canada. Sept. 2012 - present
• Bachelor of Science in Mechanical Engineering, Karlsruhe University
of Applied Science, Germany, Sept. 2012
Conference/Technical Presentations:
1. D. Fieger, K. Wilcox, A. Gerber. “Design of an Overset Mesh Methodology for Forest Protection Aircraft Droplet Release”, CFD Society of
Canada 22nd Annual Conference, Toronto, June 2014.
2. D. Fieger. “An Overset Mesh Methodology used for Forest Protection”,
In Ninth Mechanical Engineering Graduate Students Conference Proc.,
Fredericton, October 2013.