Experimental and Computational Investigation of a Turbofan Inlet Duct
by
Zachary Mitchel Hall
A thesis submitted to the Graduate Faculty of
Auburn University
in partial fulfillment of the
requirements for the Degree of
Master of Science
Auburn, Alabama
December 18, 2009
Approved by
Anwar Ahmed, Chair, Professor of Aerospace Engineering
Roy Hartfield, Professor of Aerospace Engineering
Andrew Shelton, Assistant Professor of Aerospace Engineering
ii
Abstract
The flow field of an axisymmetric turbofan inlet was investigated experimentally
and computationally. Flow visualization results were obtained using LIF, hydrogen
bubbles, and PIV. Incidence angle was determined to be a primary factor in the variation
of pressure coefficients near the leading edge of the inlet geometry. Formation of an inlet
vortex was observed when the inlet was in the proximity of the ground.
An optimization study for a non-axisymmetric turbofan inlet duct using Genetic
Algorithms and Computational Fluid dynamics was also conducted. The CFD model
included flow conditions of the CFM56-5B turbofan inlet duct geometry to provide
baseline results for comparison with the optimized geometry. A grid refinement study
was conducted to ensure accuracy of results. This grid generation and computational
model was used in the optimization study.
iii
Acknowledgements
The author would like to thank Dr. Anwar Ahmed for instilling an interest in
aerodynamics and for guidance and support throughout the course of this effort. The
author would also like to thank his committee: Dr. Roy Hartfield for his guidance in
aerospace system optimization methods and Dr. Andrew Shelton for his support in
computational aerodynamics. Thanks are also due to Vivek Ahuja for his help with the
development of the optimization code used in this effort and Hamza Ahmed for his
training in experimental methods. The author would especially like to thank his fianc? for
her enduring support and patience during this effort.
iv
Table of Contents
List of Figures ................................................................................................................... vii
List of Tables ..................................................................................................................... xi
Nomenclature .................................................................................................................... xii
Introduction ......................................................................................................................... 1
Methodology ..................................................................................................................... 19
1 Experimental ...................................................................................................... 19
1.1 Model Geometry ............................................................................... 19
2 Experimental Data Acquisition .......................................................................... 22
2.1 Test Facilities .................................................................................... 22
2.2 Experimental Setup ........................................................................... 22
2.3 Tests Performed ................................................................................ 24
2.3.1 Flow Visualization ........................................................................... 24
2.3.2 Particle Image Velocimetry (PIV) ................................................... 25
3 Computational Fluid Dynamics ......................................................................... 28
3.1 Grid Generation ................................................................................ 28
3.2 CFD Solver Model ............................................................................ 32
3.3 Boundary Layer Resolution: Near ? Wall Treatment ...................... 35
3.4 Flight Conditions .............................................................................. 37
v
3.5 Grid Refinement................................................................................ 38
3.5.1 y + Sensitivity Study ......................................................................... 38
3.5.2 Far-Field Boundary Refinement ...................................................... 47
3.5.3 Grid Spacing Refinement ................................................................ 51
4 Inlet Optimization .............................................................................................. 56
4.1 Genetic Algorithms ........................................................................... 56
4.1.1 Tournament Selection ...................................................................... 56
4.2 Integrated CFD and GA Networks ................................................... 58
4.3 Optimization Goals ........................................................................... 60
4.4 Design Space ..................................................................................... 63
Results & Discussion ........................................................................................................ 66
5 Experimental Results.......................................................................................... 66
5.1 Effect of Reynolds Number .............................................................. 70
5.2 Effect of Angle of Incidence ............................................................. 74
5.3 Formation of an Inlet Vortex ............................................................ 78
6 Computational Fluid Dynamic Simulations ....................................................... 82
6.1 Simulation of CFM56-5B ................................................................. 82
6.2 Optimized Geometry ......................................................................... 85
Conclusions ....................................................................................................................... 89
References ......................................................................................................................... 90
Appendices ........................................................................................................................ 93
1 CST Transformation & Bernstein Polynomials ................................................. 93
vi
2 Example GA Curve Fitting Design Space.......................................................... 99
3 Example Curve Fitting of Bernstein Polynomials to CFM56-5B Cowl .......... 100
4 PIV Uncertainty Analysis................................................................................. 103
vii
List of Figures
Figure 1. Inlet Locations ? Integrated engines [1] .............................................................. 2
Figure 2. Inlet Locations ?Podded engines [1] ................................................................... 3
Figure 3. Thin lip inlet auxiliary devices at low speed [5] ................................................. 4
Figure 4. Subsonic Inlet Nomenclature [1] ......................................................................... 5
Figure 5. Typical Streamline Patterns for Subsonic Inlets [4] ............................................ 7
Figure 6. Possible locations of boundary layer separation [4] ............................................ 8
Figure 7. Example Total-pressure distortion contour plot [5] .......................................... 10
Figure 8. Sources of distortion [5] .................................................................................... 12
Figure 9. Ground vortex visualization [16]....................................................................... 13
Figure 10. Inlet vortex flow model (inlet vortex source) .................................................. 14
Figure 11. Potential flow streamlines a) quiescent b) low speed c) high speed [13] ........ 16
Figure 12. Axisymmetric Model Geometry (inches) ........................................................ 20
Figure 13. CFM56-5B Duct and Engine Layout .............................................................. 21
Figure 14. Water tunnel experimental flow visualization diagram ................................... 23
Figure 15. Water tunnel flow visualization setup ............................................................. 24
Figure 16: CFM56-5B mounted on wing.......................................................................... 29
Figure 17: 3-D geometry generation using circular revolution of 2-D CFM56-5B ......... 30
Figure 18. CFM-56-5B CFD grid ..................................................................................... 34
viii
Figure 19: Universal wall law plot for turbulent boundary layers on smooth, solid
surfaces [23] .................................................................................................... 36
Figure 20: Grid comparison of area-weighted y+ solutions on inner duct surface ........... 40
Figure 21: Grid comparison of area-weighted y+ solutions on outer duct surface ........... 40
Figure 22: Comparison of coarse and fine mesh for y+ sensitivity study ........................ 42
Figure 23: y+ grid comparison of non-dimensionalized total drag on inner duct surface 44
Figure 24: y+ grid comparison of non-dimensionalized total drag on nose cone surface 45
Figure 25: y+ grid comparison of non-dimensionalized fan-face total pressure .............. 46
Figure 26: y+ grid comparison of non-dimensionalized fan-face mass flow rate ............ 46
Figure 27: Comparison of coarse and coarser mesh for far-field boundary study............ 48
Figure 28: Far-field grid comparison of non-dimensionalized total drag on inner duct
surface ............................................................................................................. 48
Figure 29: Far-field grid comparison of non-dimensionalized total drag on nose cone
surface ............................................................................................................. 49
Figure 30: Far-field grid comparison of non-dimensionalized fan-face total pressure .... 49
Figure 31: Far-field grid comparison of non-dimensionalized fan-face mass flow rate ... 50
Figure 32: Comparison of coarse and fine mesh for grid spacing study .......................... 51
Figure 33: Grid spacing comparison of percent total drag on inner duct surface ............. 54
Figure 34: Grid spacing comparison of percent total drag on inner duct surface ............. 54
Figure 35: Grid spacing comparison of non-dimensionalized fan-face total pressure ..... 55
Figure 36: Grid spacing comparison of non-dimensionalized fan-face mass flow rate ... 55
Figure 37: Example tournament selection and creation of new generations .................... 58
ix
Figure 39. Generalized concept of operations for a given generation GA run [34] ......... 59
Figure 40. Network structure of GAMBIT and FLUENT [34] ........................................ 60
Figure 41: Design space for optimization study ............................................................... 63
Figure 42: Maximum and minimum input geometry variables for GA design space ...... 65
Figure 43. Example LIF Data ........................................................................................... 67
Figure 44. Example PIV Data ........................................................................................... 68
Figure 45. Re? = 3700 4.5 hz a) LIF b) PIV ..................................................................... 69
Figure 46. Sub-critical operating condition Re? = 3700 4.5 hz a) LIF b) PIV ................ 70
Figure 47. Critical operating condition Re? = 11000 13.4 hz a) LIF b) PIV ................... 71
Figure 48. Super-critical operating condition Re? = 15000 17.9 hz a) LIF b) PIV .......... 72
Figure 49. Super-critical operating condition Re? = 18000 a) LIF b) PIV ....................... 73
Figure 50. Super-critical operating condition Re? = 22000 a) LIF b) PIV ....................... 73
Figure 51: PIV Results Re? = 3700 Incidence Angle = a. -10? b. 0? c. 10? ..................... 77
Figure 52 PIV Results Re? = 15000 Incidence Angle = a. -10? b. 0? c. 10? .................... 77
Figure 53. Quiescent flow PIV measurements Re? = 0 .................................................... 79
Figure 54. Inlet Vortex Formation Re? = 0, dt = 20/32 seconds ..................................... 80
Figure 55. Inlet Vortex Stagnation Region, Re? = 0 ....................................................... 81
Figure 56. Vector Flow Field of CFM56-5B at an Angle of Attack of two degrees ........ 82
Figure 57. Flow field pressure coefficient contour plots for the CFM-56-5B .................. 83
Figure 58. Flow field Mach number contour plots for the CFM-56-5B ........................... 84
Figure 59. Boundary Layer Growth of CFM56-5B AoA: 2? ........................................... 84
Figure 60. Flow uniformity: best & worst performers vs. GA Generations ..................... 86
x
Figure 61. Total pressure ratio: best & worst performers vs. GA generations ................. 87
Figure 62. Comparison of the original and the optimized CFM-56-5B Geometry .......... 88
Figure 63. General equation representation for a round LE, sharp TE airfoil [32] ......... 93
Figure 64. Class Function 2D Design Space .................................................................... 94
Figure 65. CFM56-5B Duct Geometry to Equation Fit .................................................... 97
Figure 66. GA Design Space ............................................................................................ 99
Figure 67. GA Equation Fitting after 50 Generations..................................................... 100
Figure 68. GA Equation Fitting after 200,000 Generations ........................................... 101
Figure 69. Equation Fitness with Increasing Generations of GA Run ........................... 102
Figure 70. Example standard deviation, Re? = 22000 .................................................... 103
Figure 71: PIV Standard deviation: Variation in angle of incidence and Re.................. 104
xi
List of Tables
Table 1: Initial boundary layer aspect ratio comparison for y+ sensitivity study ............. 39
Table 2: Mesh sizes used for y+ sensitivity study ............................................................ 42
Table 3: Solution comparison for y+ sensitivity study ..................................................... 43
Table 4: Solution comparison for Far-Field sensitivity study .......................................... 47
Table 5: Grid comparison of initial and maximum grid spacing ...................................... 51
Table 6: Grid comparison of y+ solutions for grid refinement study ............................... 52
Table 7: Solution comparison for grid refinement study .................................................. 52
Table 8. Fitness Ratio Data of Increased Generations .................................................... 102
xii
Nomenclature
A shaping function variable
( )iA Cell area at ?ith? location on grid surface
AoA Angle of attack
REFa? Reference speed of sound of the fluid
BP Bernstein Polynomials
C Class function
c chord length
CFD Computational Fluid Dynamics
pC Pressure coefficient
CST Class-Shape-Transformation
d Fan-blade diameter
dt Time step
GA Genetic Algorithm
i Variable counter
k Total number of velocity values
lbs Pounds
LE leading edge of an airfoil
M Mach number
xiii
( )iM x x-axis component of Mach number at ?ith? location on grid surface
N Class function variable
N? Total number of grid points on a grid surface
n Order of Bernstein polynomial
p Local pressure
PIV Particle image velocimetry
( )iPS Static pressure at ?ith? location on grid surface
?p Freestream pressure
R Universal gas constant
RANS Reynold?s Averaged Navier Stokes
r Variable counter
R Radius
Re Reynolds number
Re? Reynolds number
S Wing area
Sr,n(x) Shape function
T? Average total temperature for a grid surface
TE Trailing edge of an airfoil
U Freestream velocity
u Velocity
? Averaged mean velocity
ui Velocity at the ith location
xiv
u* Friction velocity
V Local velocity
?V Freestream velocity
v Kinematic viscosity
?x Velocity component in the x-axis direction
( )ivx Velocity component at grid point ?i? in the x-axis direction
x Variable location on x-axis
y Variable location on y-axis
y+ Dimensionless distance from wall
z Variable location on z-axis
? Boatail angle
? Change in
? Index of flow uniformity
? Specific heat ratio
? Symbolic variable
? Courant number
? Ratio of x-axis location to chord length
? Ratio of y-axis location to chord length
S? Static density for a grid surface
?? Average total density for a grid surface
? Degrees
? Freestream
1
Introduction
Efficient inlets are an integral part of a propulsion system because the performance
of an engine depends greatly on the characteristics of flow provided by the inlet. The
purpose of an engine inlet or diffuser is to match the mass flow requirements of the
compressor for efficient operation at a given flight condition. In doing so, a diffuser
slows down the flow to a lower Mach number with the best pressure recovery so as to
provide the highest stagnation pressure upstream of the compressor face for improved
thrust generation. Diffusion of flow is accomplished by decelerating the flow such that
the steep stream wise pressure gradient does not result in boundary layer separation
rapidly and flow unsteadiness and consequently the distortions in the velocity profiles at
the compressor inlet that can lead to compressor stall and surge.
Inlets are categorized as either integrated or podded based upon where they are
located on the aircraft. Integrated inlets are a part of the body of the aircraft, commonly
on the fuselage and are also known as buried inlets. Common locations include on the
nose of the fuselage (chin), above or below the fuselage (chin or over-fuselage),
underneath the wings (armpit), on the fuselage before the tail (tail root), or on the wing
leading edge, Figure 1.
2
Figure 1. Inlet Locations ? Integrated engines [1]
Integrated inlets are commonly used in military applications for their improved
aerodynamic characteristics in transonic and supersonic flight. However, efficient and
stable supersonic diffusion for a wide range of supersonic Mach numbers is difficult to
achieve. Supersonic integrated inlets must capture the engines required mass flow rate
while managing shocks in the inlet. To ensure this, variable inlet geometry may be
required to minimize inlet loss and drag [2]. Integrated inlets are more constrained by
internal aerodynamics due to engine placement and therefore require longer ducts that
bend and turn the flow. Therefore, internal flow separation and secondary flow are the
primary design concerns [3].
Unlike integrated inlet, podded inlets are placed at a distance from the aircraft and
are commonly used in subsonic commercial applications due to two important
3
considerations: 1) the engines are farther from the fuselage, therefore, the engines radiate
less noise to the cabin, and 2) maintenance is generally easier. Common locations include
under and below the wings, on the tail, and even on the wingtips, Figure 2 .
Figure 2. Inlet Locations ?Podded engines [1]
Since podded inlets are placed away from the aircraft, the engine ingests
undisturbed freestream flow. They also have short inlet ducts and therefore have the most
direct route possible from freestream flow conditions to the engine [3][4] and a near-
isentropic internal diffusion can be achieved [2]. Variable inlet geometries are used to
adjust the inlet for optimal flow conditions at multiple operating conditions. Variable
inlet lip geometry is not required but is commonly used to improve performance at low
speeds, such as during takeoff [5]. A few examples of variable inlet geometry devices are
shown for reference in Figure 3.
4
Figure 3. Thin lip inlet auxiliary devices at low speed [5]
The primary aerodynamic considerations for a podded inlet design are the distance
air travels from freestream conditions to the fan-face, the shape of the inlet, and the type
of attachment to the wing. A subsonic, podded inlet was chosen for this investigation;
therefore further literature on podded inlet aerodynamics is presented here.
Podded inlets consist of a nacelle or duct that surrounds the engine. The cross
section of a typical subsonic inlet nacelle and its major geometry parameters is presented
in Figure 4. The inlet area, Al, sometimes referred to as the inlet highlight, is the area of
the forward most cross section of the duct. The maximum internal area of the duct is at
the fan-face. The main purpose of the inlet, to increase the pressure by decelerating the
flow through subsonic diffusion, is achieved by an increase in area from the inlet to the
fan-face, Af.
5
Figure 4. Subsonic Inlet Nomenclature [1]
The area of flow that is ingested into the engine, at a given condition, is known as
the capture area. This area is normally non-dimensionalized by the inlet area, and is
referred to as the capture area ratio. The magnitude of the capture area ratio is dependent
on the freestream flow conditions and the mass flow requirements of the engine.
To understand how capture area ratios may be greater or less than one, Seddon?s
[3] conclusions analysis of incompressible flow through an inlet is presented here.
( )( ) peefe CqqAAk ?=+ ? 11 2qe (6)
Using the definition of dynamic pressure:
( ) 21
21
22
?
?
?
? =???
?
???
?==
?
qqqqVVAA e
e
e
ee ?? (7)
Substituting Equation 6 in Equation 7 obtains:
6
( )21
1
fe
pe
e AAk
CAA
+
?=
? (8)
For a real world engine, the area at the fan-face is the exit area:
k
CAA pf
f +
?=
? 1
1
(9)
The final result, Equation 9, shows that, assuming incompressible flow, that the
capture area is determined primarily by the area at the fan face. The inlet area was
simplified out of the equation; this proves that the capture area is independent of the inlet
area. Therefore, the flow at the entry to the inlet adapts to the required mass flow value
set by the fan-face area whether or not the inlet area is large or small.
Equation 9 was obtained by assuming incompressible, subsonic flow, but Seddon
asserted that this conclusion may be applied to compressible subsonic flow as well.
Qualitative results for compressible and incompressible subsonic flow are the same,
though quantitative results differ. Therefore a qualitative understanding of compressible
flow through an inlet can be gained from incompressible flow.
During low-speed high-thrust operations (take-off and climb) the inlet may be at a
sub-critical operating condition, and not initially ingest enough air to meet the mass flow
requirement. If this occurs, the engine will attempt to ingest the air required [1]. A
streamline pattern of additional suction is presented in Figure 5a. The inlet area is less
than the freestream area and flow accelerates into the inlet.
During level-flight at cruise velocities, the inlet may be at a super-critical
operating condition, and ingest more air than is required. During this condition inlet must
7
spill the excess flow out the front lip of the inlet; referred to as spillage [1] [4]. A
streamline pattern of spillage is presented in Figure 5b. When spillage occurs, the inlet
area is greater than the freestream area, and flow decelerates into the inlet.
Figure 5. Typical Streamline Patterns for Subsonic Inlets [4]
The freestream capture area is commonly non-dimensionalized by the area of the
inlet and referred to as the capture area ratio. The capture area ratio is greater than one
during sub-critical operating conditions, less than one at super-critical conditions. The
critical condition is when the capture area ratio is equal to one, and is commonly referred
to as full flow.
For all capture area ratio values, the flow bifurcates at the duct leading edge of the
inlet and either is ingested into the engine or flows externally around the duct. Freestream
flow that is not ingested accelerates externally over the surface of the duct and causes a
region of lower pressure near the external surface of the duct lip. At high-speed
conditions, the flow may accelerate and become supersonic, resulting in the formation of
shock waves. The ingested flow decelerates in the diffuser and, depending on the rate of
the pressure rise, can be a source of local flow separation. Flow separation also occurs on
8
the external and internal surfaces of the inlet: (1) on the exterior surface, on the (2)
interior lip, (3) or nose cone, Figure 6.
Figure 6. Possible locations of boundary layer separation [4]
During high alpha operations, the likelihood of local flow separation and formation
of separation bubbles increase [6][7]. This possibility is manifested in cases of nacelles
with sharp lips. Sharp lips are designed to have optimal flow for a specific flight
condition, at the cost of performance at off-design conditions. Rounded lips are
commonly used to ensure well behaved internal flow characteristics at most flight
conditions. Internal flow separation may occur if the area of the inlet increases too
quickly. Limits exist on the radii of curvature of the leading edge and internal diffuser
section of the duct which maximize the pressure recovery with minimal to no flow
separation [9]. Internal flow separation has large adverse effects on engine performance.
Many research efforts have focused on inlet design to predict and ultimately prevent flow
separation through the use of wind tunnel testing, empirical models, and numerical
analysis [8][10].
The purpose of the inlet is to increase the pressure of the flow by lowering the
Mach number. Because of this, during compressible flow, an inlet is a form of a
compressor. Like a compressor, the inlet ingests free stream flow, at a high Mach number
and low pressure, and increases the local pressure by lowering the Mach number of the
9
flow as it passes through the inlet. (The inlet?s ability to increase the pressure is known
as the pressure recovery and is considered the best gauge of inlet efficiency.) The
pressure recovery is the ratio of the work done in compression to the total available
kinetic energy of the flow. In high freestream flows, this ratio is equivalent to the total
pressure ratio, or the ratio of the total pressure at the exit of the diffuser to the freestream
pressure.
As previously stated, diffusion in podded inlets is near isentropic, and therefore are
quite efficient, commonly having pressure recovery values over 90%. The pressure
recovery is critical to engine performance because approximately a 1% reduction in inlet
pressure recovery will reduce thrust by about 1.3% [1].
Reductions in pressure recovery can be caused by turbulence due to flow
separation, losses due to boundary layers on the diffuser walls, and external and internal
shock waves. The total effect of these disturbances on pressure recovery is known as
distortion. Distortion is used to describe the magnitude of how non-uniform and non-
ideal a flow is across the face of the engine: at the aerodynamic interface plane (AIP)
between the inlet and the engine [5]. Distortion refers to an adverse distribution of flow at
the API and is described in terms of the variation of total pressure across the engine face
[3].
Distortion levels are traditionally visualized by plotting total-pressure contours in
polar coordinate form at the AIP [5]. The data is plotted as if looking upstream, to view
how the engine sees the oncoming flow. A typical total-pressure distortion plot
comparing experimental and analytical data is presented in Figure 7.
10
Figure 7. Example Total-pressure distortion contour plot [5]
A certain level of radial non-uniformity will always exist, even without flow
separation, due to the boundary layer growth on the inlet walls, that can cause major
engine aerodynamic failures [11],[12]. The most severe malfunctions caused by distortion
are compressor stall and engine surge. Compressor stall is when airflow separates from
the airfoils in the compressor, decreasing engine performance. Flow separation, if severe
enough, may cause engine surge. Flow separation can prevent the compressor from
increasing the local pressure inside the engine, causing the pressure inside of the engine
to be higher than the pressure in the compressor and inlet. If this occurs, the high-
pressure flow from the combustor surges back through the front of the inlet and can cause
severe structural damage.
Malfunctions due to distortion can not be completely prevented through careful
design, but inlets can be designed to limit their occurrences to a minimum that can be
considered negligible. This is accomplished by maintaining a tolerable amount of
11
distortion. This tolerance limit is the amount of distortion an engine can experience
without surge occurring.
12
Distortion can be caused by a number of sources, depending on the type of inlet
and location on the aircraft. Presented here is an overview of common aerodynamic
effects that increase distortion, depicted in Figure 8 [5]. Distortion can be caused by: (a)
Flow separation due to the interaction between the inlet shock and the compression
surface boundary layer; (b) Spillage of the boundary layer from the front of the fuselage
that can be ingested into the inlet; (c) Vortices formed upstream of the aircraft can be
ingested: vortices formed by the aircraft or vortices generated by other aircraft if the
aircraft crosses the path of another aircraft before the vortices have dissipated; (d)
Separated flow in a curved or S-duct diffuser; (e) Separation at the duct lip due to sideslip
or high incidence angle.
Figure 8. Sources of distortion [5]
13
Other types of ingestion induced distortion include ingestion of weapon exhaust,
re-ingestion of hot-exhaust during vertical and short take-off and landing (VSTOL) flight
and use of thrust reversers due to, and the ingestion of inlet vortices near the ground.
Inlet vortices are vortices that form between the inlet and the ground; and are also
known as ground vortices [13]. They form when the engine is operating at high power
near the ground while at low speeds or stopped [14]. Normally the vortex core cannot be
seen with the naked eye, but condensation can cause the vortex core to become visible
[15].
Figure 9. Ground vortex visualization [16]
In the absence of the ground, inlet vortices do not occur. In freestream flight,
streamlines of ingested flow are axisymmetric .At low speeds, the capture area is near
infinite and freestream flow may be ingested from a considerable distance away from the
engine centerline. In the presence of the ground, the ground impedes these streamlines
below the inlet and the flow lines become asymmetric; causing a stagnation point to form
on the ground [17].
14
However, inlet vortices do not occur solely from an inlet being near the ground.
Inlet vortices require a non-ideal flow field to form; therefore only in the presence of
flow disturbances will inlet vortices form. A common misconception is that the vortex is
formed by the gas turbine rotor, but this is incorrect [13].
Disturbances such as wake vortices from other aircraft and cross winds cause
horizontal flow to be introduced to the vertical up-flow of air from the ground to the inlet.
A vortex immediately forms when this occurs [14]. High axial velocities in the vortex
core occur and cause a large drop in pressure [18]. A cartoon of the vortex core flow
field is presented in Figure 10.
Figure 10. Inlet vortex flow model (inlet vortex source)
Inlet vortices are a problem to the aerospace industry because of the drop in
pressure in the vortex core. This pressure drop causes the vortex to become like a
?vacuum? and to pick up rocks, sticks, dust, etc. and create foreign object debris [14][19].
15
The vortices are not strong enough to carry debris the entire distance into the
engine, however, the vortices can be strong enough to toss objects upward, and the inlet
flow field ingests the object. In the absence of an inlet vortex, the ingested flow field is
not strong enough to suck objects on the ground into the engine [17]. Therefore if the
formation of inlet vortices can be prevented, damage due to FOD will be prevented.
Inlets can be designed to minimize the formation of inlet vortices but they can
never be wholly prevented. Some novel concepts have been developed to periodically
break up the inlet vortex. However these have been found to stir up as much debris as the
inlet vortices that they prevent [14][19]. A common method implemented by the
aerospace industry to minimize ingestion of objects into the engine is to keep the runways
clean by sweeping and or vacuuming the runways on a regular basis [13].
Inlet vortex suppression through design requires a strong understanding of the
characteristics of their formation. The main characteristics of the vortex are its stagnation
location on the ground relative to the engine and its strength. The strength of the vortex
and location of the stagnation point depend on the cross wind conditions and are not fixed
[17]. To gain a better understanding of this, Colehour?s analytical flow model is
presented here [13]. Colehour divided the flow into inviscid potential flow and viscous
flow. He concluded that the potential flow model allows the deduction of a fairly
complete flow model in the region of the ground plane. He asserted that the complete
three-dimensional flow field can be studied using the method of Rubbert by assuming the
flow is inviscid and incompressible [20]. With these assumptions, his potential flow field
results are shown here.
16
A simple sink flow near a ground plane was used to model flow with quiescent
ambient conditions, Figure 11a. With the addition of tangential flow to the sink flow, a
model of flow with some ambient wind condition is obtained, Figure 11b. It was found
that the addition of a head-wind caused the stagnation point to move in the ambient flow
direction. A large enough addition of a tangential flow was found to remove the
stagnation point from the ground, Figure 11c. His results support the assertion that the
stagnation point location is variable and dependent on the ambient flow conditions.
Figure 11. Potential flow streamlines a) quiescent b) low speed c) high speed [13]
a b
c
17
Genetic Algorithms (GA) and Motion Adjoint methods have been used in the past to
optimize aerodynamic shapes for freight trucks [25], gas turbine engines [26], missiles
[27][28], and aircraft wings and airfoils [29], [30].An efficient tool used for optimization
of aerodynamic shapes is the Class-Shape-Transformation (CST) method with Bernstein
Polynomials (BP) [31],[32]. This method has been successfully used with the GA to
create equations for and to optimize airfoil and propeller [33] geometries.
Optimization of an inlet duct can be used to increase pressure recovery and ensure
flow uniformity at the inlet to an engine, resulting in better performing and efficient
engine inlet geometries. However, little research has been done on optimization of engine
inlet geometries using Bernstein Polynomials and GA.
The CFM56-5B turbofan inlet duct was used as the baseline geometry for this effort.
It was chosen because it is widely used around the world. It is the primary engine for the
A320 family of aircraft, and any implemented improvements to the inlet geometry would
have a significant economic impact on the airline industry. The CFM56 engine is a single
stage, high-bypass ratio turbofan engine designed for commercial and military use. The
CFM56-5B has the highest fan pressure ratio of all CFM56 engines, providing between
22,000 and 33,000 lbs of thrust, and is the first commercial engine to use an ultra-low
emission combustor.
A binary encoded GA was used to drive Computational Fluid Dynamics (CFD) that
ran three dimensional flow simulations with the aim of optimizing engine geometry. The
inlet geometry was defined as multiple Bernstein Polynomials whose coefficients were
varied using a binary encoded GA over a wide design space to optimize the inlet
18
geometry for cruise conditions. The system created for this optimization effort was thus
both versatile and modular and allowed for designs that, in future, could enable further
modular additions including engine pylons and wing interfaces.
19
Methodology
1 Experimental
1.1 Model Geometry
The axisymmetric model?s geometry was determined from available two-
dimensional CFM56-5B specifications using a genetic algorithm and the Class Shape
Transformation method (CST) [31]. Exact data points were obtained for each of the duct
surfaces (two internal and two external duct surfaces) using AUTOCAD. This was done
to obtain equations to represent each surface by curve fitting the data point. Bernstein
polynomials have been proven accurately to represent airfoils and nacelles [31].
Therefore, a real-coded genetic algorithm was used to randomize these Bernstein
polynomials to match the twenty points obtained from the figure for each curve. This
method is presented in detail in the appendices. Using this method four equations were
found, with a maximum percent difference from the data points of less than 0.1 %. This
was assumed to be a negligible error.
A 3-Dimensional model was created from these 2-D equations with circular swept
revolution from the upper surfaces to the lower. Ideally, a non-axisymmetric model
would have been used for experimental tests. However an axisymmetric model was
chosen over the real world non-axisymmetric CFM56-5B geometry due to machining
limitations using a CNC lathe. The axisymmetric geometry was obtained by revolving the
20
equations representing the real world duct upper surfaces 360? about the engine
centerlines.
The lower portion of the duct is blunt, which was assumed to minimize the
formation of inlet vortices when near the ground. The upper airfoil has a larger camber
and a shape that matches more conventional duct geometry. The upper duct surfaces were
chosen to create the model because it was assumed that they were more critical to cruise
condition design. A comparison of the model geometry used and the CFM56-5B is
presented in Figure 12 and Figure 13.
Figure 12. Axisymmetric Model Geometry (inches)
21
Figure 13. CFM56-5B Duct and Engine Layout
Photos courtesy of CFM International, a 50/50 joint company between Snecma and
General Electric
The model was cut from a solid block of acrylic using a CNC lathe from a STEP
file created in SOLIDEDGE. Acrylic was chosen to be able to permit light to shine
through the model to illuminate clearly the flow field inside the model. This was
necessary to be able to conduct flow visualization inside the model cavity. The nose cone
was painted black to reduce reflections that would adversely affect the captured images.
Initially after machining, the model had a turned finish and was opaque. The model
was polished using NOVUS polish remover level 2 and then level 1 to obtain a clear
finish.
22
2 Experimental Data Acquisition
Flow visualization was conducted on scale model geometry of a high-bypass
turbofan inlet duct.
2.1 Test Facilities
All tests were conducted in the Auburn University Aerospace Engineering 45 cm x
45 cm cross-section test section water tunnel. The test section was 2 m long and
transparent, which allowed for flow visualization and quantitative measurements. The
water tunnel was capable of maximum velocity of 1.1 m/s and had a turbulence intensity
of 1% at maximum velocity.
2.2 Experimental Setup
Tests were conducted in the water tunnel and the model was sting mounted on a
specially designed support system. The model was connected to a constant volumetric
flow rate water pump to achieve a favorable pressure gradient in the cavity of the model.
The extracted flow was deposited back into the water tunnel through a hose, at
approximately thirty times the body diameter downstream of the model support system,
which was assumed to have a negligible effect on the flow field. The vertical support was
attached to the sting mount at approximately four body diameters behind the trailing edge
of the model. The entire support assembly rested on the top of the tunnel walls. This
distance was chosen to limit the moment arm caused by the model on the support system,
while also minimizing disturbance caused by the cylindrical vertical support strut. The
mass flow rate was determined from the measured volumetric flow rate using a Fill-RITE
digital flow meter attached directly after the rate water pump. A laser light sheet was
23
created using an argon laser and reflected using a mirror to illuminate regions of interest,
as can be seen in Figure 14.
Figure 14. Water tunnel experimental flow visualization diagram
The laser sheet was set at an obtuse angle to prevent shadows caused by refraction
in the leading edge of the lower surface from being present in the PIV images. A dark
colored material was placed on the opposite side of the water tunnel from the camera to
absorb reflected light that would interfere with flow visualization results, as can be seen
in Figure 15. Note that the inlet model is not attached to the mounting system in the
image shown.
24
Figure 15. Water tunnel flow visualization setup
2.3 Tests Performed
The tunnel was run at Reynolds numbers of 3700, 7000, 11000, 15000, 18000, and
22000 based on the diameter of the inlet near the fan-face (2 inches).
2.3.1 Flow Visualization
Two flow visualization methods were used in this effort: hydrogen bubbles and
laser induced fluorescence (LIF); simultaneously and alone. Hydrogen bubbles were
produced through electrolysis by applying voltage across a platinum wire and anode
placed in the water tunnel. The electrolysis caused the hydrogen and oxygen in the water
to separate and form visible hydrogen bubbles that followed accurately the path of the
flow. A constant voltage of 34 V was applied through the probe for all tests to create
optimum size and amount of bubbles for flow visualization. A bubble wire probe that
created bubbles vertically on the X-Y plane was used to obtain data on the vertical
25
symmetry plane of the model. The probe consisted of three equally spaced 32 Swg
platinum wires. The probe was mounted onto a traversing system that rested on the tunnel
side walls. A 2 mm thick laser light sheet was placed in the plane of symmetry to
illuminate the hydrogen bubbles.
For the LIF tests, a solution of sodium flourescein salt and water was injected into
the freestream flow at approximately two model body diameters away from the leading
edge of the model. An airfoil shroud was placed onto the dye injection tube to minimize
interference caused by the introduction of the dye injection system to the flow. Flow
visualization results were recorded using a high speed CCD camera.
2.3.2 Particle Image Velocimetry (PIV)
Particle Image Velocimetry is a non-intrusive technique that tracks the motion of
seeding particles in the flow. The particles are illuminated by a dual-pulsed laser light
sheet in the plane of interest. The laser light is reflected off of the particles during the
duration of the laser pulse. A CCD camera is positioned perpendicular to the plane of
interest to capture a series of still images from the light reflected from seeding particles.
The camera is synchronized with the dual-pulse laser to obtain pairs of images with a
known time difference between the images of each pair. Each seeding particle
displacement distance is determined by calculating the change in location of individual
seeding particles between the first and second image of each pair. The time between each
dual pulse laser is set according to the freestream velocity of the flow field for each
experiment and the cross-correlation camera is synchronized with the dual-pulse laser.
Therefore the time and displacement of the seeding particles between each image is
26
known. From each pair, the velocity vector magnitude and direction of the seeding
particles can be obtained from the known displacements of the seeding particles between
each image.
Measurements were statistically averaged from 200 pairs of images to remove any
outlying disturbances in the flow as well as obtain the major trends of the flow. Each pair
of images may have not caught every intricacy of the flow with the same fidelity.
Averaging multiple pairs of images ensures that vector data of high fidelity is obtained
for the entire flow field. Increasing the total number of images increases quality of the
averaged data, however a limit exists after which increasing total pairs of images gives
diminishing returns. The number of pairs of images was chosen to obtain a well defined
flow field, while not requiring an unreasonable amount of time to compute the statistical
average of the pairs. Rifki determined that ?the dual-pulsed laser and cross-correlation
camera allow the system to significantly reduce images acquisition rate between a pair of
consecutive images in the illuminated observation plane [34].? An increased acquisition
rate decreases the time required for each series of image capturing, thus allowing for a
larger number of total image pairs to be taken and statistically averaged in the same
amount of time.
A Dantec Dynamics PIV system, consisting of a Highsense 1k x 1k cross-
correlation CCD camera and a PIV 2100 processor, and New Wave Research 50 mJ dual-
pulse ND: YAG laser were used to acquire PIV images that were processed using Dantec
Flow Manager Software. The interrogation window used for cross-corexhaurelation
computation was 32x32 pixels with 50% overlap. PIV data was post-processed using
27
Tecplot 360. The flow was seeded with silver coated hollow glass spheres with an
average diameter of 20 microns. These were chosen because they are highly reflective,
with specific gravity approximately equal to one, and follow the streamlines of the flow
closely.
28
3 Computational Fluid Dynamics
The CFM56-5B geometry used in the experimental investigation was also used for
the CFD solution.
3.1 Grid Generation
One of the major requirements of the automated optimization discussed later in
this effort was the need for fully autonomous and computerized grid generations driven
by a GA. Such an automated grid generation program was created for the CFM56-5B
engine geometry. The program created a journal file based on the geometry of the inner
and outer surfaces of the duct. The journal file was run by the grid generator code.
The commercial code GAMBIT was used to develop an unstructured mesh from
the journal file defined in one zone. The input to the grid generation code included values
for the constants in the Bernstein Polynomials as well as the chord lengths of the 2D duct
geometry on the vertical X-Y plane
A 3D grid was also generated based on the CFM56-5B engine duct. Assumptions
were made about the engine geometry to obtain a 3D grid from available 2D data of the
duct. It was assumed that the upper surface of the duct CFM56-5B is revolved over a
circular path to the lower surface. As can be seen in Figure 16, the CFM56-5B duct is
nearly circular. Therefore this assumption was deemed to be reasonable.
29
Figure 16. CFM56-5B mounted on wing
Photo courtesy of Gary Brossett via the Aircraft Engine Historical Society
A geometric representation of the circular revolution used to model the engine is
shown in Figure 17. The image on the left is the circular revolution of the interior surface
points and the image on the right is the circular revolution of the exterior surface points.
The concentrated blue regions near the leading edge are representative of the clustering
of points near the leading edge as previously mentioned.
30
Figure 17. 3-D geometry generation using circular revolution of 2-D CFM56-5B
In the figure, the vertical lines that connect the upper and lower surfaces are the
circular revolutions, while the vertices on the symmetry plane, representative of the 2-D
data for the CFM56-5B, are shown as vertices. Center points for each pair of upper and
lower surface points were obtained and the distances from the center to the surface were
determined. This distance was set as the radius of the circular revolution.
The vertices where the radii are extended on the Y-Z plane are shown as black
vertices. The virtual line that connects these points does not appear ?flat? because y-axis
location of the center points between the upper and the lower surface points was not
constant as the upper and lower surfaces varied differently from each other along the
chord.
The assumption of a circular revolution introduced a known discrepancy in design
between the optimized geometry and the real world engine because the CFM56-5B duct
is not a perfect circle. However, this assumption was required for computational
efficiency..
31
The fuselage, wings, and pylon were not modeled in this effort. The engine
exhaust was not an area of interest for this work and CFD modeling of the exhaust would
have greatly increased the complexity of the investigation. Therefore the exhaust volume
was replaced by a sting of five fan-face diameters in length.
The engine was assumed to be symmetric about the X-Y plane to reduce
computational time and allow for a finer mesh in areas of high gradients. A cylindrical
shaped grid was used instead of a rectangular grid, with the engine centerline placed
along the centerline of the cylinder to further reduce the computational time.
The grid was generated with a sufficient number of nodal points to resolve the
flow field around the CFM56-5B geometry accurately. A successive ratio was applied to
the growth of the mesh relative to defined edges and surfaces. The ratio was chosen to
place the smallest x-axis vertex spacing closest to the leading edge and increase this
spacing as the vertices were placed further along the chord length. This successive ratio
was applied to the inner and outer surfaces of the duct as well as to the tip of the nose
cone.
The primary region of interest was near the cowling and inside the duct inlet
before the fan face. The mesh was refined to model accurately the pressure gradients in
this region and is discussed later. The nodal points were carefully developed to create a
well-defined mesh that adequately modeled the flow while not requiring excessive
computational times.
32
3.2 CFD Solver Model
The CFD solver used for this effort was the commercially available Reynold?s
Averaged Navier Stokes (RANS) code, FLUENT. An implicit pressure-based solver was
used for this effort. The pressure-based solver was chosen because it maintained accuracy
and robustness of the solution model given a large number of geometries prescribed by
the GA.
Convergence was defined to be when all of the residuals dropped below a 10-6 in
magnitude. A Mach number ramp-up was used to ensure the stability of the solution
during initial solution convergence. A first-order accuracy solver was used until the
solution converged. To increase the accuracy of the solution, the converged first-order
solution was used in a second-order accuracy solver.
The Spalart-Allmartas (SA) turbulence model was used because it was designed
specifically for aerospace applications involving wall-bounded flows [21]. The SA model
is a one-equation turbulence model and was chosen over more complex two-equation
turbulence models (ie. k-epsilon, k-omega) or Reynolds stress models due to reduced
computational times.
Turbulence models are accurate only for attached flows. The flow field around the
CFM56-5B was assumed to remain attached during cruise. Detached flow would be
avoided during the original design process of the engine. However, for the optimization
study, if the GA generated a geometry that caused flow separation to occur, the
inaccurate separation modeling would not affect the optimization study. The turbulence
model would inaccurately model the flow separation, however the incorrect solution
33
would accurately solve for increased losses in total pressure, compared to geometries
with no detached flow. The separated flow solution would not be chosen as a ?best
geometry? by the GA using the tournament selection method, explained later, and
therefore would be ignored. Therefore an attached flow solver was deemed to be
adequate.
The boundary conditions for the solution were set as far-field pressure, pressure
outflows, or no-slip walls. The surfaces of the inner and outer duct, sting and nose cone
were set as no-slip walls. The entry plane upstream of the engine and curved plane of the
cylindrical grid were defined as pressure far-field boundaries to model the flow coming
into the control volume. A pressure outflow boundary was used for the fan-face to model
air ingestion. The exit plane of the grid downstream of the engine was set as a pressure
outflow. For the pressure outflow boundaries, the mass flow rate was not enforced, and
therefore was allowed to change during convergence. The grid used is presented in Figure
18 below.
34
Figure 18. CFM-56-5B CFD grid
35
3.3 Boundary Layer Resolution: Near ? Wall Treatment
Boundary layer growth on the interior surfaces of the duct and nose cone causes
losses in total pressure. To better understand this growth, and to ensure that the grids used
in the y+ sensitivity study accurately resolved the boundary layer, a brief overview of
boundary layer profiles by Frank White is presented below [22].
The velocity profile of a boundary layer consists of three regions: the viscous sub-
layer (y+ < 5), the outer region (350 ? y+ > 30), and the overlap region (5 ? y+ ? 30). In
the viscous sub-layer, viscous shear is dominant and the velocity profile is linear.
However, in the outer region, turbulent shear is dominant and the velocity profile is
logarithmic. In the blending region, both viscosity and turbulence are important in
resolving the boundary layer, and the velocity profile is represented by a blending of the
linear and logarithmic profiles. Presented in Figure 19 is the experimental turbulent
modeled in wall coordinates. As can be seen in the figure, the law of the wall fits the
experimental data. The law of the wall however for y+ > 1000, the data departs the wall
law due to an adverse pressure gradient.
36
Figure 19. Universal wall law plot for turbulent boundary layers on smooth, solid
surfaces [23]
To accurately model the boundary layer and near-wall region, multiple approaches
can be used. Given here is a description of the two near-wall treatments predominantly
used: near-wall models or wall functions [21].
For near-wall modeling, a mesh is developed to resolve the viscosity-dominated
region completely to the wall, which includes the viscous sub-layer and overlap region.
However, to properly resolve this region a considerably fine mesh is required.
Wall-functions do not resolve the viscous region near the wall. Instead, semi-
empirical ?wall functions? are used to model, as opposed to fully resolve, the near-wall
region. Because wall functions do not require a fine mesh all the way to the wall,
turbulence models that use wall functions do not require grids to be as fine, compare to
near-wall models. Therefore, solutions using wall functions are faster and therefore more
37
practical. This is true only for high-Reynolds-number flows because of the thin boundary
layer.
As previously stated, the turbulence model used was the SA model. The SA model
uses an enhanced wall function. Instead of modeling the near-wall region as three
separate wall laws (viscous sub-layer, outer layer, and overlap layer), enhanced wall
functions formulate the law-of-the-wall as a single wall law for the entire near-wall
region.
Because of the lack of universally accepted models in the overlap region, grid
solutions with y+ values in the blending region were avoided for the optimization study.
3.4 Flight Conditions
The goal of the optimization study was to demonstrate a methodology for
optimizing a turbofan inlet for cruise conditions. Exact flow parameters for the CFM56-
5B engine duct during cruise are proprietary information of GE and Snecma, and had to
be approximated for this effort. The engine is the primary engine for the A320 family of
aircraft. Therefore the far-field conditions were based upon the A320 cruise conditions at
a Mach number of 0.8 at 38,000 ft altitude. A static pressure was estimated at the fan-face
by assuming a face Mach number of 0.4 and assuming a stagnation pressure at the
constant freestream value. This is the proper boundary condition for inlet modeling. The
static pressure was set, while the total pressure at the fan-face was free to vary due to
loses in the boundary layer.
38
3.5 Grid Refinement
A grid refinement study was conducted on the CFM56-5B geometry to ensure that
variation in solutions of different sized meshes based on y+ solutions and grid spacing
were negligible.
3.5.1 y + Sensitivity Study
Before conducting the grid mesh size refinement study, a grid sensitivity study of
the aspect ratio of the first boundary layer mesh was conducted to verify that variations in
y+ did not affect the solution.
The goal of the optimization was primarily concerned with the interior of the duct.
Therefore conditions at the fan-face and on the interior walls of the duct and nose cone
versus number of grid cells are presented to compare results.
Initial y+ estimations were based on a boundary layer on a flat plate for freestream
and fan-face Reynolds numbers to determine approximate heights of the first layer of the
boundary layer mesh.
The initial height of a boundary layer mesh is commonly non-dimensionalized by
the tangential grid spacing and given as a percentage; this is referred to as the boundary
layer aspect ratio. The first boundary layer mesh aspect ratio was varied to generate
coarse and fine grids to determine the aspect ratios ranges that corresponded to each
boundary layer region. As can be seen in Table 1, aspect ratios of 200% and higher
corresponded to y+ values in the outer region (y+ > 30). Aspect ratios between 25% and
200% corresponded to y+ values in the blended region (5 ? y+ ? 30). Aspect ratios of
12.5% and below corresponded to y+ values in the viscous sub-layer (y+ < 5).
39
Table 1. Initial boundary layer aspect ratio comparison for y+ sensitivity study
Area-Weighted y+
Initial BL Aspect
Ratio
Grid
Points
Inner Duct
Surface
Outer Duct
Surface
300% 911097 61.70 122.03
200% 996064 40.44 79.46
100% 1164641 19.16 37.98
50% 1328332 9.03 17.94
25% 1450240 4.81 8.70
12.5% 1616464 2.46 4.47
The y+ solutions of the inner duct and outer duct surface for each grid are presented
in Figure 20 and Figure 21. Horizontal lines are overlain onto the figures to show the
boundaries between the three regions of the boundary layer. As can be seen in the figures,
the majority solutions of the grids generated were in the blending region, which is known
to be the least accurate.
40
1
10
100
0.9 1.1 1.3 1.5 1.7A
rea
-W
eig
hte
d y
+ I
nn
er
Du
ct
Su
rfa
ce
# of Cells x 106
Figure 20. Grid comparison of area-weighted y+ solutions on inner duct surface
1
10
100
0.9 1.1 1.3 1.5 1.7
Ar
ea-
We
igh
t y
+ O
ute
rr
Su
rfa
ce
# of Cells x 106
Figure 21. Grid comparison of area-weighted y+ solutions on outer duct surface
(Outer Region)
(Blending Region)
(Viscous Sub-layer)
(Outer Region)
(Blending Region)
(Viscous Sub-layer)
41
For comparison of solutions, a course mesh and fine mesh were chosen from the
grids generated based on their solutions of the area-weighted y+ values on the interior and
exterior surface of the duct. The aspect ratio for the course mesh was chosen such that the
solution y+ values were in the outer region of the boundary layer while the aspect ratio for
the fine mesh was chosen such that the solution y+ values were in the laminar sub-layer of
the boundary layer. The mesh sizes and y+ solutions of both grids are shown in Table 2.
Shown in Figure 22 below is a comparison of the symmetry plane mesh near the upper
surface duct leading edge also for both grids.
42
Table 2. Mesh sizes used for y+ sensitivity study
Initial BL
Aspect Ratio
Area-Weighted
Interior Duct Surface
y+
Area-Weighted
Exterior Duct Surface
y+
Number of
Cells
Course Mesh 200% 40.44 79.46 996064
Fine Mesh 12.5% 2.46 4.47 1616464
Figure 22. Comparison of coarse and fine mesh for y+ sensitivity study
Table 3, the total drag values for the coarsest grid, for an aspect ratio of 300 %,
were significantly less than the solutions using the less coarse grids. This was assumed to
be because the boundary layer mesh was too coarse to properly resolve the boundary
layer on the duct surface.
As previously stated, Sparta-Allmartas solutions in the blending region are less
accurate. However, the solutions presented in the table below, which includes solutions in
all three regions of the boundary layer, can be seen to be nearly identical, excluding the
coarsest grid. Therefore it was concluded that that the solutions were insensitive to
changes in y+.
43
Table 3. Solution comparison for y+ sensitivity study
Total Drag
Initial BL
Aspect
Ratio
Grid
Points
Inner Duct
Surface (N)
Nose
Surface
(N)
Fan-Face Area-
Weighted Total
Pressure (N/m2)
Mass Flow
Rate (kg/s)
300% 911097 162.87 314.41 12407.02 51.2436
200% 996064 2205.30 1370.14 12426.50 51.3746
100% 1164641 2208.58 1369.00 12405.34 51.2235
50% 1328332 2199.96 1369.43 12424.21 51.3647
25% 1450240 2191.46 1371.70 12402.54 51.1904
12.5% 1616464 2204.07 1370.36 12400.2 51.1800
Plots of the interior solution values are presented below to see more easily the
negligible differences between the solutions. The plotted data is non-dimensionalized and
presented as percentages of the coarse mesh solution. Solution data of the coarsest grid,
aspect ratio of 300%, is not presented.
Figure 20 and Figure 21 present the total drag of the inner duct surface and nose
cone. The solutions for drag on these surfaces are presented because drag prediction is
sensitive to the boundary layer resolution. Therefore, if the differences in drag between
each grid were small, it could be concluded that the boundary layer for each grid was
properly resolved.
44
Figure 23. y+ grid comparison of non-dimensionalized total drag on inner duct
surface
45
Figure 24. y+ grid comparison of non-dimensionalized total drag on nose cone
surface
The goals of the optimization study were to maximize flow uniformity and total
pressure ratio at the fan-face. The area-weighted total pressure and the mass flow rate at
the fan-face are presented in Figure 25 and Figure 26 to prove that the solutions of the
grid chosen for the optimization study were insensitive to changes in y+ and valid.
46
Figure 25. y+ grid comparison of non-dimensionalized fan-face total pressure
Figure 26. y+ grid comparison of non-dimensionalized fan-face mass flow rate
47
As can be seen in the figures, the differences between solutions were minimal, and
therefore were considered to be negligible. It was concluded that the solutions were
insensitive to the values of y+.
3.5.2 Far-Field Boundary Refinement
A study was conducted on the sensitivity of the solutions to the minimum distance
from the edge of the finite grid to the engine model, in terms of fan-face diameters. The
coarse mesh chosen for the y+ sensitivity study was chosen as the baseline for comparison
for this study. The minimum distances of the grids generated are shown in Table 4.
Shown in Figure 27 below is a comparison of the mesh on the symmetry plane seen from
afar.
Table 4. Solution comparison for Far-Field sensitivity study
Total Drag
Distance
(# Fan
Diameters)
Grid
Points
Inner Duct
Surface
(N)
Nose
Surface
(N)
Fan-Face Area-
Weighted Total
Pressure (N/m2)
Mass Flow Rate
(kg/s)
40 752591 2201.01 1369.57 12394.30 51.131
20 745101 2198.62 1369.72 12379.59 51.0293
10 737694 2198.92 1370.41 12425.34 51.3697
48
Figure 27. Comparison of coarse and coarser mesh for far-field boundary study
Figure 28. Far-field grid comparison of non-dimensionalized total drag on inner
duct surface
49
Figure 29. Far-field grid comparison of non-dimensionalized total drag on nose cone
surface
Figure 30. Far-field grid comparison of non-dimensionalized fan-face total pressure
50
Figure 31. Far-field grid comparison of non-dimensionalized fan-face mass flow rate
As can be seen in the figures, the differences between solutions were minimal, and
therefore were considered to be negligible. It was concluded that the solutions were
insensitive to the far-field boundary, on the range of distances investigated in the far-field
sensitivity study. The far-field distance of forty times the fan-face diameter was chosen
for the optimization study due to increased solution accuracy at little cost due to the small
increase in total grid size. This slight increase in total grid cells was due to the cells
furthest from the geometry were considerably large.
51
3.5.3 Grid Spacing Refinement
The coarse mesh chosen for the y+ sensitivity study was chosen as the baseline for
comparison for the grid spacing refinement study. The initial and maximum mesh sizes
were varied to obtain a more coarse mesh and fine mesh. The initial and maximum grid
spacing, dictated by the size function starting at the leading edge of the duct and affecting
the inner and outer duct surfaces, of the grids generated are shown in Table 5. Shown in
Figure 32 below is a comparison of the symmetry plane mesh near the upper surface duct
leading edge also for both grids.
Table 5. Grid comparison of initial and maximum grid spacing
Interior Duct
Surface
Initial % Fan-
Diameter
Maximum %
Fan-Diameter Number of Cells
200.00% 0.290 14.496 510045
Coarse Mesh 100.00% 0.145 7.248 996064
66.66% 0.096 4.832 1511458
Fine Mesh 50.00% 0.072 3.624 2048880
Figure 32. Comparison of coarse and fine mesh for grid spacing study
52
The solutions were found to be insensitive to variations in y+, however y+ solutions
are presented in
Table 6 to determine which region of the boundary layer each mesh solved. The
data shows that the y+ solutions of all grids were above 30, and therefore were in the
outer region of the boundary layer.
Table 6. Grid comparison of y+ solutions for grid refinement study
Area-Weighted y+
Grid Spacing Grid Points Inner Duct Surface Outer Duct Surface
200% 510045 47.96 172.67
Coarse Mesh 100% 996064 40.43 79.46
66.66% 1511458 36.08 56.39
Fine Mesh 50% 2048880 31.90 46.46
The solutions of the y+ sensitivity study were chosen again compared but between
solutions of the grids generated in the grid refinement study. Presented in Table 7 are
these solutions. As can be seen in the table, the solutions of all of the grids were close to
each other. The coarsest mesh, which had nearly four times less number of cells than the
fine grid, had almost the same values.
Table 7. Solution comparison for grid refinement study
Total Drag
Grid
Spacing
Grid
Points
Inner Duct
Surface (N)
Nose
Surface (N)
Fan-Face Area-Weighted
Total Pressure (N/m2)
Mass Flow
Rate (kg/s)
200% 510045 2210.35 1363.07 12412.92 51.2248
100% 996064 2205.30 1370.14 12426.50 51.3746
66.66% 1511458 2203.17 1370.63 12408.47 51.2698
50% 2048880 2199.88 1371.38 12399.50 51.2117
53
The data in Table 7 is plotted in the following figures. The plotted data is again
non-dimensionalized and presented as percentages of the coarse mesh solution, which
had a grid spacing of 100%.
As can be seen in the figures, the differences between the solutions are negligible.
It was therefore concluded that the solutions were insensitive to variations in grid
spacing.
54
Figure 33. Grid spacing comparison of percent total drag on inner duct surface
Figure 34. Grid spacing comparison of percent total drag on inner duct surface
55
Figure 35. Grid spacing comparison of non-dimensionalized fan-face total pressure
Figure 36. Grid spacing comparison of non-dimensionalized fan-face mass flow rate
56
4 Inlet Optimization
4.1 Genetic Algorithms
A genetic algorithm is an optimization technique that is based upon the biological
process natural selection through successive reproduction generations of an evolving
population. A member of a population is a sample design for the system of interest.
Members with beneficial genetic traits survive and pass on these traits to their children.
Members without these positive traits generally do not survive as often to reproduce and
pass on their genes, and genes that are not beneficial are gradually removed, or naturally
selected out, from the population. After multiple generations, the result is a population
that is better suited to their design goals than the original population.
4.1.1 Tournament Selection
The genetic algorithm employed in this investigation is modeled after natural
selection through the use of a tournament selection. Selection is based on a designated
fitness to the desired qualities, representative of a natural environment, developed by
Murray Anderson. Initially a population is created from a range of traits, representative of
genetic chromosomes. New populations are created from parents chosen randomly from
the population.
As previously mentioned, the main goals of the optimization study were to
maximize flow uniformity and total pressure ratio at the fan-face. To do this, the GA used
a best performer selection method known as tournament selection. The tournament
selection method picks, at random, two pairs of members in the total population of each
generation. The ?better? member of each pair is chosen based on the quality value
57
calculated from the weight single representative values for each optimization goal. The
next generation is created from the two ?better? members by ?mating? the two
geometries. Each member of the new generation is created by randomly splicing the
codes of each of the ?better? members.
A flow chart of an example GA run including the tournament selection process for
three generations of an eight member population is shown in Figure 37. The roman
numerals above the flow chart represent the steps of the process. For the first generation,
generation a, the GA randomly creates eight members based upon input parameters given
to the GA. Two pairs of members are randomly chosen from the total population for the
tournament selection process, [I]. The first step of the tournament selection process is the
fitness calculation and determination of the ?best? fitness member for each pair, [II]. A
member?s fitness is a measure of a desired characteristic of the member. The ?best?
member of each pair is then mated by randomly splicing their characteristics to a member
of the next generation b, [III]. This step is repeated until the entire population of the new
generation is created. The entire process, steps [I] [II] and [II] are repeated to create the
third generation, generation c.
58
Figure 37. Example tournament selection and creation of new generations
The process is not limited to only eight members and three generations; these
values were chosen only as an example. This process can be used for any combination of
total members in each generation and number of generations.
4.2 Integrated CFD and GA Networks
The network of integrated computers set up to allow multi-node parallel CFD case
ran under the direction of the GA had the capability to drive up to four simultaneous CFD
case runs with one smaller network of computers to allow fully automated, rapid three
dimensional grid development under the direction of the GA. This computer network
consisted of a maximum of sixty available processors for CFD runs on thirty computer
59
nodes. All processes were initiated on a central node referred to as the head node. In
addition, a total of four CFD solvers were run simultaneously on the above cluster.
All CFD simulations were run with the FLUENT software, whereas grid generation
requirements were met using the GAMBIT based grid generator as discussed previously
with both being remotely initiated and controlled in a non-GUI environment by the GA.
The current network uses the FLUENT V6.2 version software as the CFD solver and was
upgraded to use the latest FLUENT V6.3 version software that served as the basis for the
CFD runs conducted for this optimization effort. A brief overview of the networked
environment is presented in Figure 38.
The relationship between single nodes in the computer cluster with the head node
that drove the entire networking operation along with the GA is presented in Figure 39.
The file structure shown here was used for each of the processors running in parallel for
each of the CFD cases being run.
Figure 38. Generalized concept of operations for a given generation GA run [34]
60
Figure 39. Network structure of GAMBIT and FLUENT [34]
4.3 Optimization Goals
The main optimization goals for the engine cowling were identified as maximizing
the total pressure ratio and flow uniformity at the engine fan face. The goal emphasis for
the first run was on maintaining the total pressure ratio while improving the flow
uniformity. This was achieved by adding weighting factors on the two goals to ensure
that one goal acted as the primary goal (flow uniformity) while the other acted as the
secondary goal (total pressure ratio). Improvements in the primary goal had precedence
over the secondary goal but still were not set so dominant as to improve at the cost of the
secondary goal.
The method for quantification of the two goals is important. For both the total
pressure ratio and flow uniformity, the calculations must be averaged for the entire fan
61
inlet grid surface so that net goal values are sent back to the GA for evaluation. This
averaging process, however, must take into account the validity of the governing
equations of the flow. This constraint was met by using a modified version of the Stewart
Mixing Analysis designed for gridded surfaces [34], which is applicable to CFD grids.
The flow uniformity was quantified as the standard distribution of the velocities at
all the cells of the grid about the mean value of the flow velocity as calculated by the
modified Stewart Mixing Analysis. Equation 10 presents the resulting form of the mean
velocity of the flow along the axial direction of the engine at the fan inlet surface.
111
2
???
?
?
???
?
+
???
???
?
???
?
+
??=
? ?
?
?
?
REF
x
a
v (10)
Where,
( ) ( ) ( )[ ] ( ) ( )[ ]
( ) ( )( ) ( )?
?
?
=
=
=
?
?
?
?
?
?
?
?
???
?
???
?
???
?
???
?
??
?
????
?
???
? ++
???
?
???
?
??
?
=?
N
i x
x
S
REFREF
REF
N
i
SN
i
xS
REFREF
iAiv iMiPaP TR
P
iAiP
iAiMiPaP TR
?
1
2
?
1
?
1
2
2 2
1
?
?
??
(11)
The flow uniformity is therefore defined as:
( )( )?
=
?= N
i
xx
N
viv?
1
2
?flow ofDeviation Standard (12)
The average total pressure is similarly defined using the mixing analysis as:
62
( ) ( )( ) ( )
Aav
iAiv iMiPaRT
P
REF
xS
N
i x
x
S
REF
REF
??
?
?
?
?
?
?
?
?
???
?
???
?
???
?
???
?
?
=?
?
=
?
?
? ?
1
2
(13)
The total pressure ratio is then evaluated by dividing the pressure obtained from
Equation 13 by the free stream total pressure value.
63
4.4 Design Space
A constrained design space for a limited scope optimization study was used to
demonstrate the optimization abilities of the genetic algorithm. Variations of two-
dimensional geometric parameters of the three-dimensional duct were used to create the
limited design space.
The geometry of the duct was allowed to vary by changing the coefficients of the
Bernstein Polynomials, representing the interior and exterior duct surfaces, about the
baseline CFM56-5B geometry. For the optimization study, the representative curves of
the CFM56-5B that were varied can be seen below in Figure 40 as dashed lines, while the
geometries that were held constant can be seen as solid lines.
Figure 40. Design space for optimization study
64
The upper and lower leading edges were varied by varying the exterior chord
lengths of the inlet. The exterior chord lengths were set as independent input, designed by
the GA, with a variation of 10% about the CFM-56-5B values. The range of the possible
leading edges can be seen in brackets in Figure 40.
The interior chord lengths were set to be dependent on the exterior chord lengths.
This was accomplished by the trailing edge locations being held constant; as the CFM56-
5B trailing edge locations, seen as black circles in Figure 40.
The varied quantities created a design space comprised of a total of twelve
variables. The two optimization goals plus the twelve variables constituted the overall
input and output quantifications for the GA runs. A matrix of possible geometries at the
maxima and minima of the design space is presented in Figure 41. The CFM56-5B
geometry is represented by thin lines, while the geometries created by the GA are
represented by thick lines.
65
Figure 41. Maximum and minimum input geometry variables for GA design space
In the figure, the upper plots have larger Bernstein Polynomial coefficients, and
therefore have thicker chords, while the lower plots have smaller Bernstein Polynomial
coefficients. The plots on the right have longer chord lengths, while the plots on the left
have shorter chord lengths.
66
Results & Discussion
5 Experimental Results
PIV was found to be a more efficient for external flow field investigation compared
to dye injection and bubble wire because of entrainment. Streamlines for the entire flow
field were obtained simultaneously using PIV. However, only one streamline was
obtained at a time using LIF. Bubble wire was able to obtain streamlines for the entire
flow field simultaneously as well, but an image of a single frame did not convey the flow
field as clearly. However, it was found that LIF and bubble wire were better flow
visualization techniques for obtaining the internal flow field due to limitations in PIV
data acquisitions.
PIV data is not presented above the upper geometry surface or inside of the
geometry due to these limitations. Data in regions where the laser passed through the
model was unreliable due to the light having been internally reflected and refracted off of
the acrylic model geometry.
In the flow visualization images, a second streamline was observed that had less
intensity than the main streamline, Figure 42. This second streamline was found to be a
reflection of the laser used to illuminate the flow field and was ignored.
67
Figure 42. Example LIF Data
PIV measurements are presented using streamlines of the flow field superimposed
onto pressure coefficient contour plots, as can be seen in Figure 43 below. Pressure
coefficients were calculated from PIV velocity vector field measurements using the
incompressible pressure coefficient equation:
2
1 ???????=
?V
VCp (14)
The freestream pressure coefficient, where the pressure coefficient is equal to zero,
is seen as orange or green in the figures.
Regions of lower pressure coefficients, where the local flow velocities are greater
than the freestream velocity, are seen as colder colors in the figures and conversely, the
regions of higher-pressure coefficients, where the local flow velocities are less than the
freestream velocity, are seen as warmer colors in the figures.
Reflection
68
Figure 43. Example PIV Data
Contour plots reveal that the pressure coefficient contours in the vicinity of the inlet
were circular in trend. Multiple contour levels can be seen near the model inlet area. The
contour level spacing closest to the inlet area is relatively small, and moving further
upstream and away from the inlet, the spacing becomes larger, until the contour level
values are equal to freestream. The small contour spacing is indicative of a high pressure
gradient, representative of the simulated ingestion of flow into the inlet.
Higher pressure coefficients were measured near the upper and lower leading edges
of the duct due to stagnation. However, the contour level spacing was greater than the
contour level spacing of ingestion. Therefore the pressure gradient due to stagnation was
concluded to be less than the pressure gradient due to suction. At a distance further from
the duct surface, and further from the engine center line, the contour level values return to
freestream values.
A close investigation of the external flow field upstream of the model centerline
revealed that the freestream flow was at a slight positive angle from the horizontal. This
69
was due to the upper boundary of the water being a free surface, instead of bounded by a
wall. Therefore the water level height was free to rise and fall due to the water displaced
by the model obstructing the flow.
Dye injected upstream and outside of the external surface of the model was
ingested into the inlet at a freestream Reynolds number of 3700, as can be seen in Figure
44a. The dye streamline can be seen continuing to the porous screen, representative of the
engine fan face. Because the capture area was greater than one, it was concluded that the
test was analogous to a sub-critical operating condition.
PIV results corroborated the flow visualization findings. Streamlines obtained by
PIV closely match streamlines of flourescein dye used for flow visualization, Figure 44b.
The streamlines allow one to visualize the capture stream tube decreasing in area, normal
to the plane of view.
Figure 44. Re? = 3700 4.5 hz a) LIF b) PIV
a b
70
5.1 Effect of Reynolds Number
As an aircraft goes through its flight envelope, the engine inlet encounters multiple
flow fields, with varying freestream flow Reynolds numbers and angles of attack. The
most common of these flight conditions are take-off, climb-out, cruise, and approach. The
effect of varying the freestream Reynolds number, while the incidence angle was held
constant, on the external flow field around the model geometry is presented in this
section. This was done to determine the effect of Reynolds number on the flow field
separately from changes in incidence angle.
It was determined that at a Reynolds number of 3700, the capture area was larger
than the inlet area, therefore the capture area ratio was greater than one, Figure 45. The
capture area can be seen as the two opposite streamlines furthest from the engine
centerline that are ingested into the inlet. The distance between these streamlines
converge as they are ingested indicative of a sub-critical operating condition.
Figure 45. Sub-critical operating condition Re? = 3700 4.5 hz a) LIF b) PIV
a b
71
Regions of pressure gradients were observed to be approximately elliptical. The
ellipses of pressure gradients all had the same semi-major axes: fixed as the distance
between the upper and lower inlet leading edges. The size of regions of constant pressure
gradients increased further from the inlet leading edges. The elliptical regions also
increased in eccentricity further from the leading edge.
As the freestream Reynolds number was increased, the streamline of the ingested
dye moved closer to the internal surface of the duct geometry. At a critical freestream
Reynolds number of 11000, the streamline of the injected dye stagnated at the leading
edge of the duct, as can be seen in Figure 46a. After stagnation, the streamline of the
bifurcated and a fraction of the streamline was ingested into the engine while the rest of
the streamline spilled over the duct surface and flowed externally around the model,
Figure 46a. The capture area was found to be approximately equal to one, indicative of a
nearly critical operating condition.
Figure 46. Critical operating condition Re? = 11000 13.4 hz a) LIF b) PIV
a b
72
Pressure coefficient contours revealed that external flow near the surface of the
duct had lower pressure coefficients. This was due to the flow accelerating over the
surface of the duct. Higher pressure coefficients were measured near the duct leading
edges, due to stagnation. The pressure coefficient contours near the model inlet were only
slightly higher than the freestream.
As the freestream Reynolds number was increased past the critical number,
spillage occurred. At a Reynolds number of 15000, dye injected at a height inside of the
duct, closer to the model centerline, was found to flow externally around the duct, as can
be seen in Figure 47a, indicative of a super-critical operating condition. The external flow
near the duct was found to have even greater decreased pressure coefficient contours,
Figure 47b. The pressure coefficient contours near the model inlet had a significant
increase compared to the freestream.
Figure 47. Super-critical operating condition Re? = 15000 17.9 hz a) LIF b) PIV
a b
73
Further increasing the freestream Reynolds number further increased the
differences in local and freestream pressure coefficients. This can easily be seen by
comparing Figure 47b, Figure 48b, and Figure 49b below.
Figure 48. Super-critical operating condition Re? = 18000 a) LIF b) PIV
Figure 49. Super-critical operating condition Re? = 22000 a) LIF b) PIV
External flow was found to accelerate and cause lower pressure coefficients.
Ingested flow decelerated and caused increased pressure coefficients. Increasing the
Reynolds number was found to amplify these trends.
a b
a b
74
It was therefore concluded that the capture area of the inlet is sensitive to the
freestream Reynolds number. This corroborated Seddon?s assumptions of flow through a
duct, as described earlier.
5.2 Effect of Angle of Incidence
A quantitative analysis, using PIV, of the effect of varying the incidence angle of
the model on the external flow field around the model geometry is presented in this
section. The incidence angle was varied while the Reynolds number was held constant.
The geometry was set at positive ten degrees, and zero degrees incidence angle.
These angles were chosen because they represent approximately angles of attack
experienced during take-off and cruise conditions. PIV measurements were not obtained
for the flow field above the model due to refraction of the laser sheet inside of the
geometry. The duct was also set at negative ten degrees. The model geometry was
axisymmetric; therefore the flow field below the model, when set at a negative incidence
angle, was equivalent to the flow above the model, when set at a positive incidence angle.
It was determined earlier that there were differences between the flow fields, due to the
presence of the vertical support in the experimental setup, however the flow fields were
observed to be comparable, and Figure 51 below.
Pressure gradients were observed to be closest together near the inlet duct leading
edge, indicative of a strong potential. The regions of pressure gradient variations for each
angle of incidence were observed to be similar.
Elliptical regions of pressure gradients were observed for all angles of incidence.
As previously seen, the ellipses semi-major axes were fixed at the upper and lower inlet
75
leading edges. Therefore the angle of the external regions of pressure coefficient was
found to be equal to the incidence angle of the model. However, increasing the incidence
angle was found to not increase the eccentricity of the elliptical distributions.
Compared to an incidence angle of zero, the region near the forward most duct
leading edge, when at a non-zero incidence angle, experienced increased pressure
coefficient values. Simultaneously, the region near the rearward most duct leading edge
experienced decreased pressure coefficient values.
For the sub-critical operating condition, an increase in incidence angle was found to
increase the pressure coefficient near the stagnation region, Figure 50. However, for the
super-critical operating condition, an increase in the incidence angle further decreased the
pressure coefficient of the flow field near the external surface of the inlet. This decrease
in pressure coefficient is indicative of higher velocities, assumed to be caused by the flow
accelerating over the external inlet surface.
The region of variation to the external flow field varied with changes to angle of
incidence. Streamlines near the lower lip, at negative angles of incidence, would be
ingested into the inlet. However, the same streamlines, when the model was placed at
positive angles of incidence, flowed externally around the geometry.
The streamlines near the external surface of the duct were affected by the duct
impeding their flow when the model was at an incidence angle. However, external
streamlines followed closely the curvature of the external surface for all angles of
incidence.
76
The freestream streamlines were found to be not significantly affected by variations
in the incidence angle, and therefore capture area did not change as well.
The ingestion or spillage of flow streamlines of the external flow field was found to
be dependent on angle of incidence. However, the major trends were concluded to be
independent of the incidence angle of the model. It was therefore concluded that the
capture area of the inlet is independent of the incidence angle.
77
Figure 50. PIV Results Re? = 3700
Incidence Angle = a. -10? b. 0? c. 10?
Figure 51. PIV Results Re? = 15000
Incidence Angle = a. -10? b. 0? c. 10?
a
b
c
a
b
c
78
5.3 Formation of an Inlet Vortex
An interesting phenomenon known as an inlet vortex was captured during the
course of the experiment. The vortex formed when the model was placed two diameters
from the bottom wall the water tunnel, which served as the ground plane. The camera
was placed 45 degrees to the tunnel wall to obtain a cross-planar view of the inlet.
Previous studies used a similar setup to capture the formation of an inlet vortex [13]. The
mass flow rate was held constant for all tests.
To gain an understanding of quiescent flow, PIV measurements were taken with the
model placed within two body diameters from the bottom surface of the water tunnel. As
can be seen in Figure 52, the magnitude of the velocity increased as the radial distance
from the inlet decreased. The streamlines can be seen to be ingested from both tangential
directions from the inlet leading edge. Away from ground plane, the streamlines would
be axisymmetric. However, the ground plane impeded the streamlines below the model
and caused the flow to be asymmetric. This caused a stagnation region to form below the
inlet; the approximate stagnation streamline can be seen in Figure 52 directly below the
model leading edge.
Pressure coefficients could not be calculated because the freestream velocity was
zero. This would cause a division by zero in the pressure coefficient equation. Instead, to
gain a quantitative understanding of the flow field, the velocity magnitude was calculated
and superimposed onto streamlines in Figure 52 using the following equation:
22 vuv ?= (15)
79
Figure 52. Quiescent flow PIV measurements Re? = 0
Inlet vortices were known to require a disturbance to the flow field, therefore a
disturbance in the form of a cross-face motion was applied to the flow field near the inlet
leading edge.
The formation of the vortex in quiescent flow is presented in Figure 53 as still
images each with a 20/32 second time difference between them. Flourescein dye was
injected upstream of the inlet near the wall of the tunnel. The dye traveled along the
bottom surface until it was ingested into the inlet. The vortex formation can be seen in
frame a of Figure 53. The vortex formation was found to be a transient, unstable process,
as can be seen from frames a ? d. After frame d, the vortex became relatively stable, as
can be seen in as frames e ? h being almost identical.
80
Figure 53. Inlet Vortex Formation Re? = 0, dt = 20/32 seconds
Injection of dye into the flow field introduced a small, but non-negligible amount
of perturbations to the otherwise laminar freestream flow in the x-axis direction. This
addition of momentum was assumed to cause slight adverse effects on the flow field.
As an alternative method to capture the inlet vortex, a flourescein salt crystal was
sprinkled on the ground plane in the vicinity of the region where the inlet vortex was
observed to form. As the crystal dissolved, a solution of fluorescent dye was produced
and contained in the termination region of the vortex on the ground plane. The
fluorescent dye contained in this region can be seen as an intense bright region in Figure
54.
a b c d
e f g h
81
Figure 54. Inlet Vortex Stagnation Region, Re? = 0
The large axial velocities produced by the vortex caused a drop in pressure in the
vortex core. This drop in pressure entrained the fluorescent dye into the vortex core. The
entrained dye allowed the tight vortex to be seen. The inlet vortex originated on the
ground plane and terminated at the porous screen, representative of the fan-face, as can
be seen in Figure 54.
82
6 Computational Fluid Dynamic Simulations
6.1 Simulation of CFM56-5B
A vector plot on the symmetry plane is presented in Figure 55. The flow bifurcates
at the stagnation points of the duct leading edges, which is represented by dark blue, and
either flows externally around the duct, or is ingested into the engine. The flow that is
ingested decelerates, seen as colder coloration, while the flow that goes externally around
the duct accelerates, seen as warmer coloration.
Figure 55. Vector Flow Field of CFM56-5B at an Angle of Attack of two degrees
Deceleration causes the pressure coefficient to increase, while acceleration causes
the pressure coefficient to decrease. This can be seen in pressure coefficient contour plots
with the grid mesh superimposed onto the plots, Figure 56a. and Figure 56b. The pressure
83
coefficient is referenced from the free-stream pressure and is defined by the equation for
pressure coefficient:
?
??=
q
ppC
p (16)
Therefore, a pressure coefficient of zero represents regions where the pressure is
equal to the free-stream pressure, as can be seen in Figure 56a. as areas of bright green.
Figure 56. Flow field pressure coefficient contour plots for the CFM-56-5B
Mach number contours are plotted in Figure 57a and Figure 57b to show the
manner in which the geometry of the duct affects the mach number of the flow field
(Note that the two figures do not have the same scale). The fan inlet for the engine in
both figures can be seen to have a Mach number very near 0.4 as specified. Since the
pressure value set at the pressure outflow boundary condition was simply an estimate
assuming the freestream stagnation pressure, the solution confirms that this was in fact a
reasonable assumption for the fan face.
a b
84
Figure 57. Flow field Mach number contour plots for the CFM-56-5B
As previously stated, the boundary layer on the surface of the duct was resolved
using an aspect ratio boundary layer mesh. A closer examination of the vector flow field
of Figure 58 reveals that the boundary layer growth along the lengths of the surfaces was
indeed resolved and the growth of the boundary layer is evident.
Figure 58. Boundary Layer Growth of CFM56-5B AoA: 2?
a b
85
6.2 Optimized Geometry
The initial GA run was initiated for a total run of 10 generations with each
generation having 20 members. The run was initiated over the computer cluster as
defined previously. The GA found and selected the optimum goal values at the end of this
run and the results are shown in Figure 59 and Figure 60. Shown in Figure 60 is the
generational improvement of the total pressure ratio at the fan inlet of the engine, with the
baseline geometry results presented as a solid black line. It should be noted that for this
run, the total pressure ratio had a lower weighting factor than the flow uniformity, which
was the primary goal. As such, only marginal improvement could be expected for this
parameter as the run progressed. This is evident from results.
The flow uniformity showed a marked improvement over the course of the GA run.
Figure 59 shows the results for this parameter. Being the primary goal for this run, it was
found to improve by 25% over the baseline CFM-56-5B case. The improvement over the
best performer for the initial generation was 5% and the improvement over the worst
performer of the initial generation was found to be 9.5%.
86
Figure 59. Flow uniformity: best & worst performers vs. GA Generations
The total pressure improvement over the initial generation best performer was
found to be equal to 0.08%, shown in Figure 60. The improvement over the worst
performer of the initial generation was found to be equal to 0.2%. The GA generated best
performer however had a 1% decrease in total pressure compared to the baseline CFM56-
5B geometry. This was assumed to be due to the larger weighting given to the flow
uniformity.
87
Figure 60. Total pressure ratio: best & worst performers vs. GA generations
The method used to obtain an average of each design goal at the fan face was
determined to correctly model the fitness improvement trends. However, it could not be
assumed that that the values were quantitatively accurate. This was determined to be
adequate to prove the abilities of the optimization method and setup.
A comparison of the optimized and baseline geometries is presented in Figure 61.
As can be seen in the figure, the optimization decreased both the external chord lengths
from the baseline geometry.
88
Figure 61. Comparison of the original and the optimized CFM-56-5B Geometry
89
Conclusions
The capture area was found to be directly proportional to the freestream Reynolds
number, but independent of the incidence angle of the model. An inlet vortex was
determined to be a steady well behaved vortex, caused by cross-flow disturbances
introduced to the flow field.
Computational modeling of a full scale turbofan geometry results suggest that the
assumptions of grid spacing and y+ values for the mesh used were reasonable. The
computational model of the CFM56-5B engine was used as the baseline for a geometry
optimization study to improve total pressure and flow uniformity at the fan-face. The
improved turbofan inlet geometry, compared to the CFM56-5B model, had a 25%
increase in flow uniformity while at the cost of a 1% decrease in total-pressure at the fan-
face. The hardware and software setup was used for the optimization study was found to
be a fast, proven, robust, and effective system.
90
References
[1] Raymer, D. P. (1989). Aircraft Design: A Conceptual Approach, AIAA Education
Series, American Institute of Aeronautics and Astronautics, Inc, Washington, D.C.
[2] Mattingly, J.D., Heiser, W.H., Daley, D.H., Aircraft Engine Design, AIAA Education
Series, AIAA, New York, 1987, pp. 354-393
[3] Seddon, J., and Goldsmith, E. L., 1999, "Inlet aerodynamics," 2nd edition, AIAA
education series, AIAA
[4] Hill, P., Peterson, C., Mechanics and Thermodynamics of Propulsion, Addison-
Wesley Publishing, Massachusetts, 1992.
[5] Goldsmith. E.L., Seddon, J. 1993, ?Practical Inlet Aerodynamic Design?, AIAA
Educational Series
[6] Jakubowski, A.K., Luidens, R.W., ?Internal cowl-separation at high incidence
angles?, AIAA 13th Aerospace Science Meeting, Pasadena, California, January 20-22,
1975
[7] Hurd, R., ?Subsonic pitot inlets ? high-speed high-incidence performance?, Rolls-
Royce (Bristol) Report PD 2029, 1976
[8] Albers, J.A. and Miller, B.A. (1073) ?Effect of subsonic inlet lip geometry on
predicted surface and flow Mach number distributions?. NASA TN D7446
[9] Fox, R.W. and Kline, S.J. (1962) ?Flow regimes in curved subsonic diffusers?. J.
Basic Eng. Trans ASME.
[10] Carter, E.C (1972) ?Experimental determination of inlet characteristics and inlet and
airframe interference?. AGARD, LS 53
[11] Aulehla, F. (1982) ?Inlet swirl, a major disturbance parameter in engine/inlet
compatibility. 13th Congress of ICAS/AIAA, Seattle, August 1982.
[12] Hercock, R.G. and Williams, D.D. (1974) ?Distortion-induced engine instability
aerodynamic response?. AGARD,LS72-Paper No. 3.
[13] Colehour, J.L. and Farquhart B.W. Inlet Vortex. J. Aircraft, The Boeing
Company, Seattle, Wash. Vol. 8. no. 1. Jan. 1971
91
[14] Smith, David, Dorris III John, inventors; McDonnel Douglas Corporation.
Aircraft Engine Apparatus with Reduced Inlet Vortex. United States patent 6,129,309.
2000 Oct 10.
[15] Yadlin, Y. ?Simulation of Vortex Flows for Airplanes in Ground operations?,
AIAA Paper 2006-56,2006
[16] Laurent, R. "Jet Engine Ground Vortex Studies", Master?s Thesis, Cranfield
University Sept. 2007.
[17] Rodert, L. & Garrett, F. ?Ingestion of Foreign Objects into Turbine Engines by
Vortices?, NACA TN 3330, 1955
[18] Kendall, J. M. Jr., ?Experimental Study of a Compressible Viscous Vortex,? TR
No. 32-290, June 1962, Jet Propulsion Laboratory, C.I.T., Pasadena, Calif.
[19] Johns, C. ?The Aircraft Engine Inlet Vortex Problem?, AIAA?s Aircraft
Technology, Integrations and Operations (ATIO) 2002 Technical, 1-3rd 2002, Los
Angles, California, AIAA 2002-5894
[20] Rubbert, P. E., et al., ?A General Method for Determining the Aerodynamics
Characteristics of Fan-In Wing Configurations,? D-6-13476-1, Nov. 1967, The
Boeing Company, Seattle, Wash.
[21] ANSYS, Inc., Fluent 6.3 User?s Guide, 2008. http://fluent.com.
[22] White, F.M., Viscous Fluid Flow, 3rd ed. McGraw Hill, New York, 1991
[23] Clauser, F. H., ?The Turbulent Boundary Layer,? in Advances in Applied
Mechanics, Vol. IV, Academic Press, New York, 1956
[24] Dyer, J.D., ?Aerospace Design Optimization Using a Real coded Genetic
Algorithm?, Master?s Thesis, Auburn University, Alabama, May 2008.
[25] Doyle, J., Hartfield, R.J., and Roy, C. ?Aerodynamic Optimization for Freight
Trucks using a Genetic Algorithm and CFM?, AIAA 2008-0323, presented at the
46th Aerospace Sciences Meeting and Exhibit, Reno, NV, January 2008.
[26] Torella, G., Blasi, L., ?The Optimization of Gas Turbine Engine Design by
Genetic Algorithms?, AIAA Paper 2000-3710, 36th AIAA/ASME/SAE/ASEE Joint
Propulsion Conference and Exhibit, July 2000.
[27] J.E. Burkhalter, R.M. Jenkins, and R.J. Hartfield, M.B. Anderson, G.A. Sanders,
?Missile Systems Design Optimization Using Genetic Algorithms?, AIAA Paper
2002-5173, Classified Missile Systems Conference, Monterey, CA, November, 2002
92
[28] Hartfield, Roy J., Jenkins, Rhonald M., Burkhalter, John E., ?Ramjet Powered
missile Design Using a Genetic Algorithm?, AIAA 2004-0451, presented at the forty-
second AIAA Aerospace Sciences Meeting, Reno NV, January 5-8, 2004.
[29] Anderson, M.B., ?Using Pareto Genetic Algorithms for Preliminary Subsonic
Wing Design?, AIAA Paper 96-4023, presented at the 6th AIAA/NASA/USAF
Multidisciplinary Analysis and Optimization Symposium, Bellevue, WA, September
1996.
[30] Perez, R.E., Chung, J., Behdinan, K., ?Aircraft Conceptual Design Using Genetic
Algorithms?, AIAA Paper 2000-4938, presented at the 8th
AIAA/USAF/NASA/ISSMO Symposium on Multidisciplinary Analysis and
Optimization, Bellevue, WA, September 2000.
[31] Kulfan B., M., Bessoletti J., E., ?Fundamental Parametric Geometry
Representation for Aircraft Component Shapes?, 11th AIAA/ISSMO
Multidisciplinary Analysis and Optimization Conference, 6-6 September 2006,
Portsmouth, Virginia.
[32] Kulfan B., M., ?A Universal Parametric Geometry Representation Method ?
CST?, 45th AIAA Aerospace Sciences Meeting and Exhibit, 8-11 January, Reno,
Nevada, 2007.
[33] Burger, C. and Hartfield, R.J., ?Propeller Performance Optimization using Vortex
Lattic Theory and a Genetic Algorithm?, AIAA-2006-1067, presented at the Forty-
Fourth Aerospace Sciences Meeting and Exhibit, Reno, NV, Jan 9-12, 2006.
[34] Rifki, R., ?Flow Around Axisymmetric and Two-Dimensional Forward-Facing
Cavities?, Master?s Thesis, Auburn University, Alabama, May 2006
[35] Ahuja, V., ?Optimization of Fuel-Air Mixing for a Scramjet Combustor Geometry
using CFD and a Genetic Algorithm?, Master?s Thesis, Auburn University, Alabama,
Dec. 2008.
[36] Ahuja, V. and Hartfield, R.J., ?Optimization of Fuel-Air Mixing for a Scramjet
Combustor Geometry using CFD and a Genetic Algorithm?, Multidisciplinary
Analysis and Optimization Conference (MDO), Victoria City, Vancouver, Canada,
September 2008.
[37] Anderson, M. B., ?Using Pareto Genetic Algorithms for Preliminary Subsonic
Wing Design,? AIAA Paper 96-4023, presented at the 6th AIAA/NASA/USAF
Multidisciplinary Analysis and Optimization Symposium, Bellevue, WA, September
1996.
93
Appendices
1 CST Transformation & Bernstein Polynomials
There are a number of possible methods to approximate equations of airfoil
geometries. One of the most efficient methods is the class function, shape function
transformation (CST). Presented here is the theory developed by Kulfan [31][32].
The general equation of an airfoil can be represented as
( ) ( ) ( ) TESn ??????? ?+???= 1 (17)
The first two terms of Eq. (14) form the class function, Sn is the shape function,
and the final term is the trailing edge thickness. In the physical space Eq. (14) becomes:
( ) ( ) ( ) ( )TEczcxcxSncxcxcxcz ?+???= 1 (18)
A graphical representation of Eq. (14) is shown in Figure 62 .
Figure 62. General equation representation for a round LE, sharp TE airfoil [32]
2?zTE
? = x/c
?= z/c
?TE = ?zTE/c
94
The class function controls the LE radius, airfoil thickness, and boatail angle while
the shape function determines the geometry between the LE and TE. Depending on the
shape function chosen, a number of possible shapes in the design space can be modeled.
The class function in the design space is defined as [31][32].
( ) ( ) [ ] 211
2
1 NNNNC ??? ??= (19)
with ? being the fraction of the chord. In the physical space the unit class function
is:
( ) ( ) [ ] 21 1 NN cxcxcxC ??= (20)
where c is the chord length and x is the x position along the chord. The first term of
Eq. (17) affects the shape of the leading edge and the last term affects the shape of the
trailing term, as defined by N1 and N2. An example of possible shapes applicable to
airfoils can be seen in Figure 63.
N1 = 1.0, N2 = 1.0 N1 = 0.5, N2 = 1.0 N1 = 0.5, N2 = 0.5
Figure 63. Class Function 2D Design Space
The entire airfoil was represented by the combination of two unit class functions,
for the upper and the lower surfaces, multiplied by a unit shape function.
95
The unit shape function is defined by a BP of the order n with the variable x/c
ranging from 0-1.0. The BP?s were chosen due to the mathematical property of ?Partition
of Unity? which states that all of the terms of a BP sum to equal 1.0 [32]. This is a
desired quality because all powers of BP are equal. So, any order of n for BP can be used.
If BP of different orders of n were not all equal, then BP could not be used for this
method.
The shape function is defined as [32]
( ) ( ) ( )?
=
???
?=
n
r
rn
nr cxrnr
nxS
0
, 1!!
!
(21)
The first term of the equation defines the binomial coefficients with increasing
order of n for the BP. For each order of n, there exists n + 1 number of total terms in the
BP.
The first term of Equation (18) defines the leading edge radius by the equation:
First Term cRLE2= (22)
The second term of Eq. (18) defines the boatail angle by the equation:
Last Term czTan ?+= ? (23)
The remaining terms, those between the first and last, are known as shaping terms,
which affect the geometry of the airfoil between the leading and trailing edge.
96
The components of the peaks of the shape functions are equally spaced along the
chord, for i ranging from 0 to n, which is determined by the equation:
( ) nicx S =max (24)
The components of the peaks of the component airfoils are also equally spaced
along the chord, for i ranging from 0 to n, which is determined by the equation:
( ) ( ) ( )nNNiNcx Z +++= 211max (25)
Increasing the order of n increases the ability of the shape function to equate airfoil
geometries. This is because as the order of n increases, the number of peaks to be able to
match the desired geometry increases [32].
A negative effect of increased order of n is increased computational times.
Eventually increasing the order of n past a critical number will have diminishing returns;
improvements in accuracy between orders of n will be small enough to be negligible and
will not be worth the increased computational times. Values of n = 6-9 for BP accurately
modeled airfoil geometries [32]. A Bernstein Polynomial of order n = 6 was chosen
because it is a high enough order of n to accurately model an airfoil9 and has decreased
computational times compared to higher orders of n.
The entire 2D duct geometry that is to be curve fitted, with the exception of the
turbine blade geometry and nose cone, can be seen in Figure 64.
97
Figure 64. CFM56-5B Duct Geometry to Equation Fit
The entire airfoil can be created with two unit class functions, one for the lower
surface and one for the upper surface. The entire 2D duct, consisting of 2 airfoils, can be
created with 4 class functions. Equations 23 & 24 define the entire duct geometry. The
first two terms of each equation are the class function. The last terms represent the shape
function, BP of order n = 6.
The variables N1 and N2 were set equal to 1.0 and 0.5 to create a class-function with
a rounded leading edge and a sharp trailing edge8. The variables of A were modified [33]
to apply to the CFM56-5B coordinates and preliminary bounds were set at -100 to 100 to
allow for a larger design space. This 2D class/shape function for each curve consists of 9
variables. Each airfoil consists of an upper and lower surface, which are defined by two
different sets of BP equations. The entire 2D duct consists of two airfoils, with two
surfaces each, for a total of four surfaces and 36 variables for all of the surfaces.
98
Airfoil, Outer Surface definition:
( ) ( )[ ]
( ) ( ) ( )[ ]
( ) ( )[ ]
( ) ( )[ ]
( ) ( )[ ]
( ) ( )[ ] ( )[ ]
zcx
cxAcxcxA
cxcxA
cxcxA
cxcxA
cxcxAcxA
cxcxz NNOuter *)/(
1*1***6
1***15
1***20
1***15
1***6*
*1*
6
7
51
6
42
5
33
4
24
3
15
2
6
1
21 +
?
?
?
?
?
?
?
?
?
?
?
?
?
?
?
?
?
?
?+?+
?+
?+
?+
?+
?=
(26)
Airfoil Inner Surface definition:
( ) ( )[ ]
( ) ( ) ( )[ ]
( ) ( )[ ]
( ) ( )[ ]
( ) ( )[ ]
( ) ( )[ ] ( )[ ]
zcx
cxAcxcxA
cxcxA
cxcxA
cxcxA
cxcxAcxA
cxcxz NNInner *)/(
1*1***6
1***15
1***20
1***15
1***6*
*1*
6
14
51
13
42
12
33
11
24
10
15
9
6
8
43 +
?
?
?
?
?
?
?
?
?
?
?
?
?
?
?
?
?
?
?+?+
?+
?+
?+
?+
?=
(27)
99
2 Example GA Curve Fitting Design Space
Having fixed the input parameters, the GA design space could finally be defined by
fixing the range of values above and below the reference values. The resulting design
space is shown in Figure 65. In Equation 23, the variables A1-7 were given bounds of -200
and 200. One can see in Figure 65 that the boundary conditions of the Genetic Algorithm
used to fit the data. The comparison of the maximum and minimum lines to the known
data points of the duct geometry proved that a mathematical solution existed in these
boundaries.
-50
-40
-30
-20
-10
0
10
20
30
40
50
0 20 40 60 80 100 120 140
x-axis location, in
z-a
xis
lo
ca
tio
n,
in
Data to Fit
Max Bound
Min Bound
Figure 65. GA Design Space
100
3 Example Curve Fitting of Bernstein Polynomials to CFM56-5B Cowl
The number of generations that the GA was run for was increased from 50
generations to 200,000 generations to determine the ability of the GA to match the data.
It can be seen that the more generations that the GA was run for curve fitting the upper
surface of the top airfoil, the closer the equations came to matching the data. The curve
fitting of the upper surface of the top airfoil is represented in Figure 66 and Figure 67. All
four curves that create the duct geometry were curve fit, but only the fitting of the upper
surface are presented here.
0
2
4
6
8
10
12
0 20 40 60 80 100 120 140
x-axis location, in
z-a
xis
lo
cat
ion
, in
Data to Fit
GA Output
Figure 66. GA Equation Fitting after 50 Generations
101
0
2
4
6
8
10
12
0 20 40 60 80 100 120 140
x-axis location, in
z-a
xis
lo
cat
ion
, in
Data to Fit
GA Output
Figure 67. GA Equation Fitting after 200,000 Generations
At approximately 10,000 generations, the returns of increasing generations were
greatly diminished (Table 1). In Figure 68 a hyperbolic relationship between generations
and fitness can be seen, with an asymptote at approximately fitness equal to 0.2. For a
perfect curve fit, the fitness would be equal to 0. This discrepancy can be attributed to
errors in recording geometry data from the available CFM56-5B duct geometry as well as
limits of BP?s ability to fit the curve. However, the maximum distance between the
CFM56-5B duct geometry and the BP representation of the curve is .0944 in, less than a
tenth of an inch.
0
0.5
1
1.5
2
2.5
3
3.5
0 20,000 40,000 60,000 80,000 100,000 120,000 140,000 160,000 180,000 200,000
# of Generations
Fit
ne
ss
102
Figure 68. Equation Fitness with Increasing Generations of GA Run
Table 8. Fitness Ratio Data of Increased Generations
Generations Fitness ?Fitness % Difference
500 4.800183773 0 0.0000%
1,000 2.863285065 1.936898708 40.3505%
2,000 1.610103011 1.253182054 43.7673%
5,000 0.860965073 0.749137938 46.5273%
10,000 0.39534381 0.465621263 54.0813%
20,000 0.386857092 0.008486718 2.1467%
50,000 0.258321494 0.128535599 33.2256%
100,000 0.224858895 0.033462599 12.9539%
150,000 0.224622801 0.000236094 0.1050%
200,000 0.224622801 0 0.0000%
103
4 PIV Uncertainty Analysis
To ensure confidence in the data obtained using PIV, an uncertainty analysis was
conducted. Standard deviation is a gauge of the uncertainty of the data. Therefore the
standard deviation for each dataset was obtained to conduct the analysis. Shown below is
an example standard deviation contour plot.
Figure 69. Example standard deviation, Re? = 22000
The standard deviation was obtained for all test cases. Shown in Figure 70 is the
standard deviation for each test case. As can be seen in the figure, the uncertainty
increased as Reynolds number increased for all angles of incidence. Interestingly, the PIV
measurements taken when the model was placed at an angle of incidence of zero had the
largest uncertainty of all measurements. PIV measurements at a negative angle of attack
had the least uncertainty.
104
Figure 70: PIV Standard deviation: Variation in angle of incidence and Re
The average of the standard deviations for all datasets was found to be % 2.42. This
uncertainty value was assumed to negligible. Therefore the measured data was concluded
to be precise.