John W. Slater, John M. Abbott, and Richard H. Cavicchi

Glenn Research Center, Cleveland, Ohio

Validation of WIND for a Series of Inlet Flows

NASA/TM—2002-211907

October 2002

AIAA–2002–0669
The NASA STI Program Office . . . in Profile

Since its founding, NASA has been dedicated to

the advancement of aeronautics and space

science. The NASA Scientific and Technical

Information (STI) Program Office plays a key part

in helping NASA maintain this important role.

The NASA STI Program Office is operated by

Langley Research Center, the Lead Center for

NASA’s scientific and technical information. The

NASA STI Program Office provides access to the

NASA STI Database, the largest collection of

aeronautical and space science STI in the world.

The Program Office is also NASA’s institutional

mechanism for disseminating the results of its

research and development activities. These results

are published by NASA in the NASA STI Report

Series, which includes the following report types:

• TECHNICAL PUBLICATION. Reports of

completed research or a major significant

phase of research that present the results of

NASA programs and include extensive data

or theoretical analysis. Includes compilations

of significant scientific and technical data and

information deemed to be of continuing

reference value. NASA’s counterpart of peerreviewed formal professional papers but

has less stringent limitations on manuscript

length and extent of graphic presentations.

• TECHNICAL MEMORANDUM. Scientific

and technical findings that are preliminary or

of specialized interest, e.g., quick release

reports, working papers, and bibliographies

that contain minimal annotation. Does not

contain extensive analysis.

• CONTRACTOR REPORT. Scientific and

technical findings by NASA-sponsored

contractors and grantees.

• CONFERENCE PUBLICATION. Collected

papers from scientific and technical

conferences, symposia, seminars, or other

meetings sponsored or cosponsored by

NASA.

• SPECIAL PUBLICATION. Scientific,

technical, or historical information from

NASA programs, projects, and missions,

often concerned with subjects having

substantial public interest.

• TECHNICAL TRANSLATION. Englishlanguage translations of foreign scientific

and technical material pertinent to NASA’s

mission.

Specialized services that complement the STI

Program Office’s diverse offerings include

creating custom thesauri, building customized

databases, organizing and publishing research

results . . . even providing videos.

For more information about the NASA STI

Program Office, see the following:

• Access the NASA STI Program Home Page

at http://www.sti.nasa.gov

• E-mail your question via the Internet to

help@sti.nasa.gov

• Fax your question to the NASA Access

Help Desk at 301–621–0134

• Telephone the NASA Access Help Desk at

301–621–0390

• Write to:

 NASA Access Help Desk

 NASA Center for AeroSpace Information

 7121 Standard Drive

 Hanover, MD 21076
John W. Slater, John M. Abbott, and Richard H. Cavicchi

Glenn Research Center, Cleveland, Ohio

Validation of WIND for a Series of Inlet Flows

NASA/TM—2002-211907

October 2002

National Aeronautics and

Space Administration

Glenn Research Center

Prepared for the

40th Aerospace Sciences Meeting and Exhibit

sponsored by the American Institute of Aeronautics and Astronautics

Reno, Nevada, January 14–17, 2002

AIAA–2002–0669
Acknowledgments

The authors would like to thank Dave Saunders, Rene Fernandez, Dr. Jim DeBonis, and Dr. Charles Trefny of the

NASA Glenn Research Center for assistance with the experimental data.

Available from

NASA Center for Aerospace Information

7121 Standard Drive

Hanover, MD 21076

National Technical Information Service

5285 Port Royal Road

Springfield, VA 22100

The Aerospace Propulsion and Power Program at

NASA Glenn Research Center sponsored this work.

Available electronically at http://gltrs.grc.nasa.gov
NASA/TM—2002-211907 1

Validation of WIND for a Series of Inlet Flows

John W. Slater,∗ John. M. Abbott,† and Richard H. Cavicchi‡

National Aeronautics and Space Administration

Glenn Research Center

Cleveland, Ohio 44135

Abstract 

Validation assessments compare WIND CFD

simulations to experimental data for a series of inlet

flows ranging in Mach number from low subsonic to

hypersonic. The validation procedures follow the

guidelines of the AIAA. The WIND code performs

well in matching the available experimental data. The

assessments demonstrate the use of WIND and provide

confidence in its use for the analysis of aircraft inlets.

Introduction

The NASA Glenn Research Center (GRC) is

involved in the design and analysis of inlet concepts for

aerospace vehicles that operate at Mach numbers

spanning the range from low subsonic to hypersonic.

Inlet flow fields are fairly complex. The external flow

enters the inlet and passes through internal ducting that

may involve significant turning and curvature to reach

the engine. The curvature of internal ducting promotes

secondary flows. The viscous flow on the vehicle and

inlet surfaces may consist of laminar boundary layers

transitioning to turbulent boundary layers. The inlet is a

flow compression device, and so, the flow exists in an

adverse pressure gradient. Supersonic flows usually

contain shock waves that then interact with the

boundary layers. All these features potentially lead to

boundary layer separation. At hypersonic Mach

numbers, the possibility of high-temperature effects

exists. The flow may consist of local unsteady features

such as time-varying shocks, boundary layers, or

boundary layer separation regions. There may exist in

the inlet flow control devices such as bleed holes and

slots, jets, and vortex generators.

An analysis of the flow in an inlet should provide

qualitative insight into the general flow features, such

* Aerospace Engineer, AIAA Senior Member.

† Senior Researcher, AIAA Member

‡ Aerospace Engineer

as the character of the boundary layers and the location

of shocks. An analysis should also provide values for

the measures of performance of the inlet. The primary

measure of performance is the total pressure recovery,

which is defined as the ratio of an average total pressure

at the inlet exit to the freestream total pressure. It

represents the amount of loss of energy in the flow due

to viscosity and shock waves. At hypersonic speeds,

the kinetic energy efficiency is often used as the

measure of performance. Other flow properties to be

determined include the mass flow through the inlet and

the distribution of pressures on the inlet surfaces.

Computational fluid dynamics (CFD) is a useful tool

for performing the aerodynamic analysis of the inlet

flows. The CFD analysis process first involves defining

the flow problem and establishing what results are

required from the analysis. The inlet geometry and

flow domain are modeled and the grid is generated.

The boundary and initial conditions are then specified

and the CFD code is then run to obtain the flow field.

The flow field is then analyzed to obtain the

performance measures of the inlet. Of primary concern

is having confidence in the CFD methods for providing

accurate, credible results.

Credibility is obtained by performing verification

and validation assessments. Here verification and

validation are defined according to the AIAA

guideline.1 Verification is defined as the process of

determining that a model implementation accurately

represents the developer's conceptual description of the

model and the solution to the model. Verification

assessment looks for errors in the numerical

approximation of the models and the programming of

the code. Such errors are uncovered through careful

visual and computational examination of the code and

through comparison of CFD simulation results to highly

accurate solutions to model problems. Validation is

defined as the process of determining the degree to

which a model is an accurate representation of the real

world from the perspective of the intended uses of the

model. Validation assessment looks for errors in the
NASA/TM—2002-211907 2

geometric and physical models through comparison of

the CFD simulation results to experimental data, which

is assumed to be the controlled observation of the real

world. Both verification and validation assessment

require that the solutions are consistent with physical

models and that the levels of iterative convergence error

and spatial and temporal discretization errors be

examined and quantified. Verification assessment

should usually precede validation assessment; however,

both are a continuous activity as long as CFD codes

incorporate new models and methods and their range of

application is extended.

In this paper, the WIND CFD code is assessed.2,3 A

verification assessment of the WIND code for several

aspects of inlet flows has been examined in an earlier

paper.4 The focus of the current paper is the validation

assessment of WIND for use in the analysis of inlet

flow fields over a Mach number range of 0.1 to 6.0.

The next section describes the WIND code. The

section following discusses procedures for performing a

validation assessment. The remaining sections then

discuss validation assessments performed for

simulations of five inlet flow fields: the Stanitz elbow,

scarf subsonic inlet, the NASA VDC supersonic inlet,

the NASA strut-jet hypersonic inlet, and the NASA

GTX hypersonic inlet.

WIND CFD Code

The WIND CFD code is being developed by the

NPARC Alliance (National Program for Applicationsoriented Research in CFD), which is an alliance of the

NASA Glenn Research Center, the Air Force's Arnold

Engineering Development Center, and the Boeing

Company.2,3 WIND solves the time-dependent,

Reynolds-averaged Navier-Stokes equations for

turbulent, compressible flows using a cell-vertex, finitevolume, time-marching approach on multi-zone,

structured grids. Spatial accuracy is formally secondorder using the Roe flux-difference splitting upwind

formulation. Steady flows are simulated through an

iterative process using local time stepping. Unsteady

flows are simulated through a second-order marching in

time; however, the Reynolds-averaging precludes the

simulation of anything other than gross unsteady flow

features. Turbulence is modeled using algebraic, oneequation, or two-equation eddy viscosity models. The

Baldwin-Lomax model is the primary algebraic model.

The Spalart-Allmaras model is the primary oneequation model. The SST model is the primary twoequation model, but the Chien k-ε model is also

available. WIND is capable of solving for flows of

speeds ranging from low subsonic to hypersonic. At

hypersonic Mach numbers, WIND has models to

simulate high-temperature effects in air.

Validation Assessment

The validation assessment of WIND for the analysis

of inlet flows recognizes the “building-block” approach

suggested in the AIAA Guideline.1 The approach

involves dividing a complex system such as an inlet

into progressively simpler phases: subsystem cases,

benchmark cases, and unit problems. Each phase

involves simpler level of geometrical complexity and

flow physics coupling, as well as, increased levels of

experimental accuracy. The validation assessments

involve a series of procedures that are discussed in the

following paragraphs:

Examine the simulation for iterative convergence.

The CFD simulations discussed here are steady-state

flow simulations in which the time-marching numerical

methods are iterated in pseudo-time until flow

properties no longer change. One measure of iterative

convergence used for these simulations was the

decrease and asymptotic convergence of the residuals

of the flow and turbulence equations. Another measure

used was the asymptotic convergence of the total

pressure recovery and mass flow through the inlet.

The typical iteration convergence criterion was that the

change in the total pressure recovery be less than

0.00001 over 500 iterations. The amount of variation

that is accepted as the convergence criterion is a

measure of the iterative convergence error.

Examine the simulation for consistency. The

simulations should be consistent with the general

principles of the models. For the inlet simulations

discussed here the conservation of mass through the

duct was checked. Furthermore, the total pressure

recovery was checked to see if it decreased, or at least

remained constant along the duct.

Examine the simulation for spatial (grid)

convergence. The basis of CFD is that as the grid is

refined for a steady-state simulation, the CFD results

should asymptotically approach the true solution of the

equations. For the inlet simulations discussed here, the

variation of the static pressure distributions and the total

pressure recovery with grid refinement was examined

as an indicator of grid convergence. When possible, a

grid convergence index (GCI) was calculated as a way

of reporting the grid convergence.5 The change in

pressure recovery with grid refinement indicates the

level of spatial discretization error.

Compare the CFD simulation results to the

experimental data. The comparison of the CFD results

to experimental data examines how well the CFD

analysis represents the real world as observed by the

experiment. The limits of the experimental data define

the limits of the validation assessments. For the inlets

considered here, the experimental data consists mainly

of static pressure distributions. Thus, the validation

assessments primarily assess how well the WIND code
NASA/TM—2002-211907 3

can predict the static pressure distributions. Any errors

in the experimental data are also reported.

Examine the simulation for uncertainties in the

physical models. For the inlet cases examined here, the

primary models that create the most uncertainty are

those modeling turbulence. Simulations were run with

at least two turbulence models to examine the level of

physical modeling error in the turbulence models.

NPARC Verification and Validation Web Site

Further details on performing CFD verification and

validation assessments can be found on the NPARC

Alliance CFD Verification and Validation web site. The

web site was created to aid the development and

support of the WIND CFD code; however, it is publicly

available and provides a useful resource for users of

other CFD codes, as well as, the worldwide CFD

community. The URL for the web site is

http://www.grc.nasa.gov/www/wind/valid. The site

includes a fairly self-contained tutorial that includes

information on conducting verification and validation

assessments. The tutorial also contains a glossary of

terms, bibliography, and links to other web sites. The

site contains an archive of verification and validation

cases representing various geometries and flow

conditions. Each case contains information on its

geometry, grid, and available analytical and

experimental data. Many of the files (grid, solution,

input, and output) can be viewed and downloaded. The

archive also includes further information on the inlet

cases reported in this paper.

Inlet Validation Cases

Validation assessments of the WIND CFD code

have been performed for a series of inlet flow cases that

span the Mach number range from incompressible

through hypersonic speeds. The cases were all

experiments conducted at the NASA Glenn Research

Center (or one of its predecessors), which in most cases

allowed direct access to the people who collected the

data. However, the experiments were primarily tests to

examine some concept related to inlet flows rather than

explicit experiments conducted to provide data for CFD

validation assessment. The experimental data mostly

consists of static pressure distributions along the

surfaces of the inlets. In some of the cases, data for the

total pressure recovery or kinetic energy coefficient is

reported. All the cases involve steady flow which is

mostly turbulent and which high-temperature effects are

not considered significant (i.e. calorically perfect air).

The following sections discuss each of the cases along

with the results of the validation assessments.

Stanitz Elbow

Figure 1. Geometry of the Stanitz elbow with total

pressure contours (flow enters from the bottom).

The Stanitz elbow was a duct of rectangular crosssection that was studied at NASA GRC in the early

1950s (at that time the NACA Lewis Flight Propulsion

Laboratory) to examine secondary flow structures in

low-speed flow ducts with turning. This duct was of

interest for a CFD validation study because it

represented a class of low-speed internal flows with

simple geometry and flow features.

Figure 1 shows the shape of the surfaces of the

elbow. The streamwise cross-section was rectangular.

The inner (suction) and outer (pressure) surfaces turned

the flow approximately 90 degrees.

The flow entered the elbow from the bottom in

Fig. 1. The flow was subsonic throughout the elbow

with a maximum Mach number of approximately 0.3,

which resulted in the flow being fairly incompressible.

The Stanitz elbow was designed using potential flow

methods to continually accelerate the flow as is turned

through the elbow while avoiding boundary layer

separation. The absence of boundary layer separation

allowed better examination of the secondary flow

features. As the flow accelerated through the elbow, a

passage vortex formed on the inner surface and was

located nearer the plane sidewall than toward the midspan of the elbow. The sense of the passage vortex was

clockwise from the perspective of an observer looking

out the exit in the direction of the main flow. Thus the

secondary flow imposed a sideways velocity

component from the plane sidewall towards the midspan of the elbow.
NASA/TM—2002-211907 4

The experiment was conducted with the elbow

attached to the top of a plenum chamber. The flow

went through the elbow and exited into the test facility

room. The experiment was conducted with a series of

spoilers upstream of the elbow that modified the shape

of the boundary layer of the flow entering the elbow.

The case considered here is that with no spoiler. The

tank gage pressure was 20 inches of water. The mass

flow through the elbow was measured from a total

pressure rake survey at the exit of the elbow to be

14.60 lbm/sec. The experimental data consist of static

pressure distributions on the suction and pressure

surfaces at several spanwise stations and total pressure

surveys at the exit plane. This case can almost be

considered a benchmark validation case in that the

geometry and flow are fairly simple; however, the

experimental data lacks information on errors.

The geometry was simple and could be modeled

fairly accurately. Geometric symmetry along the midplane allowed the modeling of only half of the elbow

for the flow domain. The flow domain included the

constant-area “tunnel” section that connected the elbow

to the plenum chamber. The tunnel section in the

experiment had a length of 24 inches. Rather than

model the details of the plenum chamber, the inflow

boundary was placed at the start of the tunnel section.

To match the experimental boundary layer velocity

profile at the entrance to the elbow, the length of the

tunnel section as modeled in the flow domain was

increased to 30 inches. The outflow boundary was

placed at the exit of the elbow.

The inflow boundary conditions assumed a total

pressure equal to the tank static pressure and a total

temperature equal to the ambient static temperature.

The outflow boundary condition was specified as a

constant mass flow condition set to the mass flow

measured in the experiment. The elbow surfaces were

assumed to be no-slip, adiabatic walls. A reflection

boundary condition was applied at the plane of

symmetry of the flow domain. Thus, the boundary

conditions were accurately modeled in the CFD

simulations. The initial conditions were the plenum

conditions with a Mach number of 0.1 assumed.

The rectangular cross-section of the flow domain

allowed a highly accurate, single-zone, structured grid

to be generated. The grid had 161 grid points in the

streamwise direction, 157 grid points from the suction

to pressure surface, and 81 grid points from the

symmetry plane to the plane wall. The total number of

grid points was 2047437. This grid size allowed a

medium grid (81x79x41) to be extracted by removing

every other grid point in each direction. Similarly a

coarse grid (41x40x21) could be extracted by removing

every other grid point from the medium grid.

Iterative convergence was determined through

examination of the decrease and asymptotic nature of

the residual of the flow equations. Further, the pressure

recovery at the elbow exit was monitored until absolute

changes in the recovery were on the order of 0.00001

over 500 iterations with a clear stabilization of the

pressure recovery.

Examining the conservation of mass through the

elbow checked the consistency of the solution. The

simulations on the fine grid indicated that the mass

fluxes integrated on the streamwise grid planes differed

by less than 0.1% of the average mass flow. The

differences on the medium grid were about 0.2%.

The spatial or grid convergence was examined by

comparing the variation of the total pressure recovery at

the elbow exit as determined from simulations on the

fine, medium, and coarse grids. Figure 2 shows those

variations for simulations performed on the various

grids and turbulence models. The relative grid spacing

is with respect to the spacing on the fine grid. Thus the

medium grid has a relative grid spacing of 2 and the

coarse grid has a relative grid spacing of 4. It should

first be noted that the low-speed character of this flow

results in very small viscous losses, and so, high

recoveries. The recovery for the inviscid simulations

should be 1.0 since viscous losses are not to exist. The

simulation on the medium grid suggests an error of

0.063%. The trend appears encouraging that, as the

grid is refined, the error would reduce further. The

laminar simulations indicate slightly more viscous

losses; however, the drastic change in slope between

the medium and fine grids indicates some irregular

behavior in the simulation. The lower recoveries of the

turbulence models seem consistent; however, the

recoveries from the simulations using the Chien

k-ε model seem inconsistent with the consistent

grouping of the recoveries of the simulations using the

Baldwin-Lomax, Spalart-Allmaras, and SST turbulence

models. This clearly warrants a closer examination of

the k-ε model.

0.9970

0.9975

0.9980

0.9985

0.9990

0.9995

0.0 1.0 2.0 3.0 4.0 5.0

Relative Grid Spacing

Pressure Recovery

Inviscid

Laminar

Baldwin-Lomax

Spalart-Allmaras

SST

k-epsilon

Figure 2. Pressure recovery with respect to grid

spacing and turbulence model.

The grid convergence indices (CGI) computed for

the variations from the simulations using the BaldwinLomax and SST models were approximately 0.001%
NASA/TM—2002-211907 5

and 0.005% for the fine and coarse grids, respectively.

The order of convergence was approximately 2.5.

These results indicated a very small variation of the

pressure recovery with grid spacing.

The elbow was designed using potential flow

methods such that the exit velocity would be

approximately twice that of the inflow velocity. This

could be verified through comparison of the theoretical

velocity variation through the elbow to that obtained

from an inviscid flow simulation. Figure 3 shows that

comparison. The velocity plotted for the CFD

simulation is an average velocity at each streamwise

grid plane. The comparison is very good until towards

the exit of the elbow. At the exit, the error is

approximately 4%, which is fairly significant and

deserves further examination of WIND.

0.0 10.0 20.0 30.0 40.0 50.0

s, inches

0.40

0.60

0.80

1.00

1.20

V / Vexit

Theory

CFD

Figure 3. Comparison of the theoretical velocity

through the elbow to the average velocity of the

inviscid CFD simulation.

Figures 4 and 5 present the comparison of

experimental and CFD static pressures on the inner and

outer surfaces. Figure 4 presents the streamwise static

pressures along the centerline of the elbow for both the

inner and outer surfaces. Figure 5 presents the spanwise

static pressures at three streamwise stations denoted by

the coordinate φ = (0.0, 3.0, 4.5), which relates to the

velocity potential used in designing the surfaces of the

elbow and scales according to the streamwise distance

along the surfaces of the elbow. The experiment report

(reference 6) did not comment on the level of error in

the experiment, and so, error bars could not be plotted.

Figure 4 shows good agreement with the experimental

data, but the differences are greatest on the inner

surface near the exit. This is the region where the

secondary flows are most significant. The absolute

difference between the experimental data and the CFD

result at the last streamwise data point is approximately

0.03 psi, which is 4.2% of the tank gage pressure.

Figure 4 shows that the static pressures from the

simulations on the fine grid were not much different

from those on the coarse grid. Furthermore, the

inviscid flow simulation indicated that viscosity did not

have a huge effect on the static pressures.

Figure 5 shows the spanwise character of the static

pressures and shows good agreement of the CFD

simulations with the experimental data. The coordinate

z/w = 0 indicates the sidewall surface. The increase of

static pressure at the sidewall reflects the presence of

the passage vortex.

Further discussion of CFD simulations of the Stanitz

elbow can be found on the NPARC Verification and

Validation web site and in Ref. 7.

0.0 20.0 40.0 60.0

s, inches

14.60

14.80

15.00

15.20

15.40

p, psia

Exp(Inner)

Exp(Outer)

Inv (medium grid)

SST (coarse grid)

SST (fine grid)

Inner

Surface

Outer

Surface

Figure 4. Streamwise distribution of the static

pressures on the inner (suction) and outer (pressure)

surfaces along the centerline of the elbow.

0.00 0.10 0.20 0.30 0.40 0.50

z / w

14.60

14.80

15.00

15.20

15.40

p, psia

Exp(Inner) Phi 0.0

Exp(Inner) Phi 3.0

Exp(Inner) Phi 4.5

Exp(Outer) Phi 0.0

Exp(Outer) Phi 3.0

Exp(Outer) Phi 4.5

SST(Inner)

SST(Outer)

Phi 3.0

Phi 4.5

Figure 5. Spanwise distribution of the static pressures

on the inner (suction) and outer (pressure) surfaces at

streamwise stations φ = (0.0, 3.0, 4.5) of the elbow.
NASA/TM—2002-211907 6

Scarf Subsonic Inlet

Figure 6. Geometry of the scarf subsonic inlet.

The scarf subsonic inlet was an inlet concept studied

at NASA GRC in the late 1970’s (at that time the

NASA Lewis Research Center) with potential

applications for subsonic aircraft.8 This inlet concept

was studied because it promised lower fly-over noise,

less ingestion of foreign objects from the ground during

take-off and landing, and greater angle-of-attack

tolerance than an axisymmetric inlet with the same lip

thickness. This inlet was of interest for a CFD

validation study because such three-dimensional

subsonic inlets are currently being studied once again at

NASA GRC as part of a comprehensive parametric

study using the WIND code for the flow analysis.9 This

validation case directly supported that study.

Figure 6 shows the surfaces of the scarf inlet. The

main geometric feature is the lower lip that extends

ahead of the upper lip with a straight side profile.

The experimental data available for validation come

from tests of the scarf inlet conducted in 1977 in the

NASA GRC 9x15-foot wind tunnel.8 The inlet was

attached to a vacuum system that allowed accurate

measurement of the inlet mass flow. The freestream

condition of the test was a Mach number of 0.12 with an

ambient static pressure of 14.63 psi and static

temperature of 533.74 °R. The freestream flow was

accelerated into the inlet and reached its highest velocity

and lowest pressure as it was turned into the inlet by the

inlet lip. The average throat Mach number was 0.63;

however, a small transonic region was formed in which

the Mach number reached approximately 1.3. A weak

normal shock changed the local supersonic flow to

subsonic conditions. Aft of the inlet throat, the flow was

diffused to decelerate and compress the flow prior to

ingestion into the vacuum system.

The experimental data consist of static pressure

distributions along the axial direction at 0, 90, and

180-degree stations along the circumference of the inlet

and total pressure contours and rake-averaged total

pressure recoveries at the exit of the diffuser. The data

of interest for this case was collected at 0 and

50 degrees angle-of-attack. This case can be

considered a subsystem validation case since the inlet

was not attached to an actual engine, and so, considered

only the aerodynamics of the flow through the inlet.

The flow domain for the CFD simulations consisted

of only one-half of the inlet due to geometric and

flowfield symmetry. Since the flowfield is subsonic the

farfield boundaries of the flow domain were extended

approximately 15 cowl diameters away from the outer

surface of the inlet. The boundary conditions at the

farfield boundaries were characteristic boundary

conditions that used the freestream conditions. The

internal portion of the flow domain extended

downstream of the diffuser exit approximately one cowl

diameter to reduce the influence of the mass flow

boundary condition applied on that boundary. The

boundary conditions on the surfaces of the inlet and

spinner were no-slip, adiabatic walls.

A structured grid was generated that contained six

zones in which the grid lines matched contiguously

across the zonal boundaries. The grid was clustered on

the inlet and spinner surfaces to resolve the turbulent

boundary layers such that the first grid point off the

viscous surfaces had a y+ of less than 1.0. The

stretching between consecutive grid points along a grid

line was kept below 15 to 20%. The baseline grid

consisted of 439484 grid points.

Simulations were performed on the baseline grid

using the Spalart-Allmaras turbulence model. Figures 7

and 8 show the comparisons between the CFD results

and the experimental data for the axial static pressure

distributions at 0 and 50 degrees angle-of-attack,

respectively. These figures were taken directly from

Ref. 9. The comparisons show good agreement,

although there is considerable disagreement at the

location of maximum thickness of the cowl lip, which

corresponds to the lowest local static pressures.

To examine if the disagreement was due to the

choice of turbulence model, simulations were

performed using the Baldwin-Lomax and SST models.

No significant differences in the static pressure

distributions were observed between the turbulence

models. Further details can be found in Ref. 9.

To examine if the disagreement was due to grid

resolution, simulations were performed in which the

number of grid points was doubled along the surfaces in

the streamwise direction, which contained the greatest

amount of curvature. No significant differences in the

static pressure distributions were observed between the

two grids. Further details can be found in Ref. 9.
NASA/TM—2002-211907 7

0

0.2

0.4

0.6

0.8

1

-1.4 -1.2 -1 -0.8 -0.6 -0.4 -0.2 0

Axial Position, ft.

Surface Static to Freestream Total Pressure Ratio, p P/ o

WIND Data

Leeward

Windward

Side

Leeward

Windward

Side

Figure 7. Comparison of the static pressure

distributions in the axial direction at 0, 90, and 180

degrees at 0 degrees angle-of-attack.

0

0.2

0.4

0.6

0.8

1

-1.4 -1.2 -1 -0.8 -0.6 -0.4 -0.2 0

Axial Position, ft.

Suface Static to Freestream Total Pressure Ratio, p/Po

WIND Data

Leeward

Windward

Side

Leeward

Windward

Side

Figure 8. Comparison of the static pressure

distributions in the axial direction at 0, 90, and 180

degrees at 50 degrees angle-of-attack.

The comparison of the total pressure recoveries at

the diffuser exit between the experimental data and the

CFD simulations with respect to the throat Mach

number is shown in Fig. 9, which was taken from

Ref. 9. The plots show the characteristic drop off in

recovery due to higher viscous losses as the throat

Mach number increases. The WIND simulations

consistently under-predicted the total pressure recovery

by about 0.4 percent at a throat Mach number of around

0.6. Changing the turbulence model or grid spacing

had no significant effect on the pressure recovery.

The parametric design study currently being

conducted by the second author is examining the angleof-attack at which the boundary layer starts to separate

from the internal surfaces of the inlet as a measure of

performance of the inlet. Determining this separation

angle-of-attack through the CFD simulation and

comparing it to experimental data are discussed in Ref.

9. A summary of that discussion is that the validation

of WIND to predict the separation angle-of-attack was

not completely conclusive. The separation angle-ofattack was determined in the experiment by monitoring

the static pressure on the cowl lip and total pressure at

the diffuser exit. However, for CFD simulations, the

separation angle-of-attack was determined by

monitoring the skin friction and noting when it first

became zero. The lack of experimental data that is

complete and consistent with CFD simulations prevents

conclusive validation of the separation angle-of-attack.

0.9

0.91

0.92

0.93

0.94

0.95

0.96

0.97

0.98

0.99

1

0.3 0.4 0.5 0.6 0.7 0.8

Throat Mach Number

α = 0o

α = 50o

WIND - Open Symbols

Data - Solid Symbols

Inlet Total Pressure Recovery, PDE/Po Figure 9. Comparison of total pressure recoveries.

Questions arose during the validation assessment as

to whether the geometry that was simulated by the grid

was the same as that tested in the wind tunnel. It was

fairly certain that the CFD model matched the design

specification of the scarf inlet; however, doubts existed

as to whether the wind tunnel model matched those

specifications. A number of CFD simulations were

performed for an axisymmetric inlet that was tested in

the same series as the scarf inlet. In the CFD model of

the axisymmetric inlet, the leading edge radius of the

CFD model was varied slightly to examine the effect of

this variation on the static pressures. The details of that

study are reported in Ref. 9. A summary of that

discussion is that small changes in the leading edge

radius had a significant effect on the static pressure

distribution on the internal surfaces of the inlet near the

leading edge and the location of maximum lip

thickness. Furthermore, it was observed that the

experimental data for the static pressure at 0 and

180-degree locations for 0 degrees angle-of-attack were

not symmetric, as they should have been. All this

suggested that there might have been variations in the

geometry of the wind tunnel models at the leading edge

and in the circumferential direction. It was indicated

that the models were fabricated of fiberglass and some

final “hand-finishing” was involved. This may have

been enough to impact the final shape of the wind

tunnel model. The wind tunnel model no longer exists

to allow confirmation of this conclusion. However, this

does show the impact of errors in geometry modeling.
NASA/TM—2002-211907 8

NASA VDC Supersonic Inlet

Figure 10. The geometric features of the NASA VDC

mixed-compression, supersonic inlet.

The NASA Variable Diameter Centerbody (VDC)

inlet was an axisymmetric, mixed-compression

supersonic inlet that was studied at NASA GRC starting

in the early 1970's and then tested in 1993.10 The term

“mixed-compression” refers to the condition that

supersonic compression occurs on the external surfaces

of the centerbody and within the internal ducting of the

inlet. A normal terminal shock exists downstream of

the throat of the inlet to create subsonic flow for intake

by a gas turbine engine. The inlet was studied as a

concept to provide good pressure recovery and variable

geometry for inlet operations for a vehicle capable of

supersonic cruise. This inlet was of interest for a CFD

validation study because it represents a class of mixedcompression, supersonic inlets that continue to be

studied at NASA GRC. This validation case directly

supports those studies and provides an example on the

use of WIND for analyzing such inlets.

Figure 10 shows some of the main geometric

features of the inlet, which includes the centerbody,

cowl, and support struts. The centerbody had the

feature of overlapping leaves, which allowed the

centerbody to collapse in a manner similar to an

umbrella. This feature allowed the cross-sectional area

of the inlet to vary to adjust to inlet operating

conditions. The entire centerbody mechanism could

also translate forward to allow further area variation.

The gap between the forward and aft portions of the

centerbody served as a bleed slot. Three struts

supported the centerbody. The cowl was axisymmetric

and included bleed holes and passages to stabilize the

shock waves and improve performance. Vortex

generators were located on the centerbody and cowl

surfaces downstream of the throat. The vortex

generators acted to energize the surface boundary layers

to reduce the likelihood of boundary layer separation in

the subsonic diffuser.

The flow field about the inlet was supersonic. The

case considered here involved a freestream Mach

number of 2.498 with a static pressure of 0.744 psi and

a static temperature of 247.44 °R. A conical shock

formed at the nose of the centerbody and impinged near

the cowl lip. An oblique shock was generated by the

internal surface of the cowl and intersected the

centerbody at its “shoulder.” The turning of the

shoulder nearly canceled the cowl shock. The Mach

number approached 1.0 as the internal supersonic flow

encountered the minimum area or throat of the inlet. A

slight diffusion of the area accelerated the flow to

approximately Mach 1.3 where a terminal normal shock

was established to decelerate the flow to subsonic

conditions while further compressing the flow. Further

subsonic diffusion reduced the Mach number at the

compressor face station to approximately 0.35 for

ingestion by the engine. Several of these flow features

are shown in the Mach number contours of Fig. 11.

Figure 11. CFD geometry and flow domain model of

the NASA VDC supersonic inlet and Mach number

contours.

The inlet was tested in the 10x10 Foot Supersonic

Wind Tunnel (SWT) at NASA GRC in 1993. The

available experimental data consist of static pressure

distributions along the centerbody and cowl and the

total pressure recovery at the compressor face station.

The wind tunnel tests were designed to demonstrate the

inlet concept rather than provide data for CFD

validation. This case can be considered a system level

validation case since the test article had many of the

complexities of an operational inlet and several tests

were conducted with an engine attached.

The geometry modeling for the CFD simulations

involved simplification of the details of the overlapping

leaves and slot to represent the centerbody and cowl as

continuous axisymmetric profiles. Furthermore, the

vortex generators and support struts were not modeled.

These simplifications introduced acknowledged

physical modeling errors into the CFD simulations

lessened the credibility of the validation assessment.
NASA/TM—2002-211907 9

The flow domain for the CFD simulations is shown

in Fig. 11. Since the inlet geometry as modeled was

axisymmetric, an axisymmetric flow domain was used

which consisted of a 10-degree section of the inlet.

Symmetry boundary conditions were applied on the

sides of the 10-degree section. Since the freestream

flowfield was supersonic, the inflow and farfield

boundaries were placed fairly close to the exterior

surfaces of the inlet, and fixed boundary conditions

could be imposed. For the supersonic outflow

boundaries on the exterior, extrapolation boundary

condition were imposed. On the surfaces of the inlet,

no-slip, adiabatic wall boundary conditions were

imposed. The bleed flow through the slot and bleed

holes was modeled using a bleed boundary condition in

which the amount of mass flow was directly specified.

The primary difficulty for a CFD simulation of a

mixed-compression inlet was the establishment of the

terminal shock. Here a varying area nozzle was

attached to the flow domain at the compressor face

station to control the amount of back-pressure at the

compressor face station and position the terminal shock.

A planar, structured grid was generated with two

zones—one placed along the centerbody for the internal

flow and a second placed along the cowl for the

external flow. The three-dimensional grid was obtained

by extruding the planar grid circumferentially over the

10-degree section of the flow domain. The grid was

clustered near the surfaces of the inlet to resolve the

turbulent boundary layers such that the first grid point

off the wall results in a y+ value of less than 1.0.

The CFD simulations were performed at zero angleof-attack with a bleed mass flow of 2.575% of the

nominal captured mass flow imposed at the centerbody

bleed slot. The initial flow field for the simulation was

the freestream conditions. The supercritical flow was

first developed in which there was supersonic flow

through the inlet. The nozzle area was then reduced

until subsonic flow and a normal terminal shock

developed in the diffuser. The nozzle area was then

gradually reduced until the static pressure at the

compressor face station matched that of the experiment.

The baseline simulation was performed using the

Spalart-Allmaras turbulence model. The comparison of

the static pressures along the centerbody and cowl as

computed by WIND with those of the experiment is

shown in Fig. 12. Estimates of the experimental error

within the static pressures were not available. Overall,

the comparisons are good. Figure 12(a) shows the

profile of the inlet for reference. WIND accurately

predicts the increase in pressure across the change in

conical sections of the forward portion of the

centerbody. The sharp rise in static pressure near the

slot and shoulder is due to the shock generated by the

cowl lip that intersects the centerbody just upstream of

the slot. The bleed that is extracted at the slot prevents

excessive boundary layer separation which would grow

and result in the unstart of the inlet. Downstream of the

shoulder, the static pressure drops and then rises

sharply across the terminal shock. The comparison

with the experimental data suffers at this point. It is

believed that the differences between the experimental

data and the CFD results at this point are due to the lack

of the modeling of the vortex generators in the WIND

simulation. A large region of boundary layer separation

existed in the CFD simulation at this point, which was

probably not present in the experiment as indicated by

the lower static pressures.

Figure 12(b) shows the comparison of static

pressures on the interior cowl surface. The axis has a

smaller range than Fig. 12(a), and so, the differences

show up more; however, the comparisons are good.

0.0 20.0 40.0 60.0

x, inches

0.0

2.0

4.0

6.0

8.0

10.0

Pressure, p, psi

Data

WIND (S−A)

WIND (SST)

WIND (S−A) Coarse

(a) Centerbody.

15.0 20.0 25.0 30.0 35.0

x, inches

2.0

4.0

6.0

8.0

Pressure, p, psi

Data

WIND (S−A)

WIND (SST)

WIND (S−A) Coarse

(b) Cowl.

Figure 12. Comparison of static pressures computed

by WIND with those of experiment for the NASA

VDC supersonic inlet.
NASA/TM—2002-211907 10

Typically the static pressure data are the easiest to

match by CFD. In supersonic, internal, turbulent flows,

the static pressure is significantly affected by shock

location and shock / boundary layer interactions. Thus,

comparisons with static pressures are more meaningful

than for subsonic inlet experiments.

Figure 12 shows the effects of grid refinement on the

pressure distributions by comparing the results on the

baseline and coarse grids. The coarse grid contained

every other grid point of the baseline grid in the

streamwise and radial directions. Some of the peaks are

not resolved as well, but the coarse grid solution was

essentially the same as the baseline grid solution. This

provided confidence that the baseline grid was of

sufficient resolution.

Figure 12 includes the static pressure distribution

obtained using the SST turbulence model. The static

pressures for the SST model follow the behavior of the

Spalart-Allmaras model. The cowl shock and terminal

shock are slightly further downstream than for the

Spalart-Allmaras model. Examination of the boundary

layer on the centerbody indicated that the boundary

layer thickness for the Spalart-Allmaras model was

greater than that for the SST model. This affected the

blockage through the inlet. The thicker boundary layers

tended to push the terminal shock forward slightly.

Simulations using the Baldwin-Lomax turbulence

model over-predicted the extent of the boundary layer

separation in the subsonic diffuser and would not yield

a reasonably steady-state solution.

The experiment indicated the total pressure recovery

as computed on a 40-probe, area-weighted rake to be

0.699. The baseline CFD simulations using the SpalartAllmaras model indicated a total pressure recovery of

0.726 on the fine grid and a recovery of 0.719 on the

coarse grid. The CFD simulation using the SST model

indicated a recovery of 0.729. These represent an

approximately 4.0% difference from the experimental

value. The higher pressure recoveries for the CFD

simulations are questionable considering that the vortex

generators were not modeled and large regions of

boundary layer separations were observed in the

simulations. One would expect the experimental

pressure recovery to be higher than those of the CFD

simulations. The pressure recoveries from the CFD

simulations were computed using a mass-weighted

average on the CFD grid at the compressor face station

rather than interpolating the CFD results to the rake

positions. The differences in these approaches to

computing the recovery from the CFD results can be

evaluated; however, past comparisons indicated a small

amount of difference. It was assumed that such a

difference would be small for these simulations and

given the simplifying approximations of the geometry

modeling, probably not meaningful to examine.

RBCC Strut-Jet Hypersonic Inlet

Cowl removed

Sidewall removed

0.0 in. 11.2 in.

16.47 in.1.6 in.

0.4 in.

Pre-compression

plate

Interchangeable

struts

Mass flow plug

Rake Actuator

Transversing

Rake

22.89 in.

2.64 in.

27.96 in.

34.26 in.

Figure 4.– Sub-scale inlet model.

Figure 13. The geometry of the RBCC Strut-Jet

hypersonic inlet.

The Strut-Jet hypersonic inlet was a concept studied

at NASA GRC as an inlet for a rocket-based combinedcycle (RBCC) engine.11 The term “combined cycle”

refers to the combination of rocket and ramjet engine

cycles that allow such an engine to operate from static

conditions to beyond Mach 8. This inlet was of interest

for a CFD validation study because it represents a class

of hypersonic inlets that continue to be studied at

NASA GRC. This case supports those studies.

Figure 13 shows a diagram of the geometry of the

Strut-Jet inlet. The inlet had a rectangular cross-section

with two struts that divided the inlet flow into three

separate flow paths that combined again at the base of

the struts. The inlet was symmetric with respect to a

plane down the center of the center flow path. Rocket

engines were located within the base of each strut.

The flowfield was hypersonic with a freestream

Mach number of 6.0. A pre-compression plate ahead of

the inlet generated an oblique shock that entered the

inlet and reflected off the cowl. Oblique shocks were

also generated by the leading edges of the struts and

entered the inlet. In operations as a ramjet, the subsonic

combustion would occur downstream of the struts. The

case considered here is that for supercritical flow in

which there is supersonic flow throughout the inlet.

The experiment was conducted in the NASA GRC

1x1 Foot SWT.11 The experimental data available for

comparison consist of static pressure distributions along

the centerline of the center flow passage on the cowl

and body, static pressure distributions on the inner

surfaces of the left and right sidewalls, total pressure

maps at the end of the isolator, and exit total pressure

recovery and kinetic energy efficiency. This case can be

considered a subsystem validation case since the test

article was a sub-scale model of the actual inlet and

considered only the aerodynamics of the inlet rather

than the combined inlet and ramjet operation.
NASA/TM—2002-211907 11

Figure 14. Flow domain and surfaces of RBCC

Strut-Jet inlet.

Figure 14 shows the flow domain, which used

symmetry to allow the modeling of only half of the

inlet. The boundary conditions were fixed at inflow

boundaries and extrapolated at the outflow boundaries.

No-slip, adiabatic wall boundary conditions were

imposed on the pre-compression plate and inlet

surfaces. The initial flow field was set to freestream.

The CFD simulations used the same grid as the

simulations of Ref. 12, which used the NPARC code.

The grid consisted of 6 zones with the grid clustered

near the inlet surfaces with a normal wall spacing of

approximately 4.0E-05. The total size of the grid was

1381946 grid points. The CFD simulations were

performed with the assumption of completely turbulent

flow using the Spalart-Allmaras and SST models.

Figure 15 show the comparison of the experimental

data and CFD results for the static pressures on the

body and cowl surfaces. The experimental error in

measuring the static pressure was reported to be

0.02 psi, which was too small to be plotted as error

bars. The comparisons between the experimental data

and CFD results are good. Both turbulence models

gave essentially the same results, but the SpalartAllmaras model tended to indicate higher peaks in the

static pressure. Both models seemed to place the shock

locations slightly downstream of the experimental data.

Also plotted in Fig. 15 are the results from the CFD

study of Ref. 12 that used the NPARC CFD code with

the Chien k-ε turbulence model. The NPARC results

indicate a large spike in the pressures on the cowl at

approximately x = 17 inches that is not indicated in the

WIND simulations. This may be due to the use of an

upwind TVD limiter in WIND, whereas the NPARC

code used a central-difference formulation with

artificial dissipation. Elsewhere along the distribution,

the NPARC results compare well with the experimental

data and perhaps compare better than the WIND results.

10.0 15.0 20.0 25.0 30.0

x, inch

0.0

5.0

10.0

15.0

20.0

25.0

ps / pso

Data: 1x1

WIND, S−A

WIND, SST

NPARC (ref. 12) 

(a) Body

15.0 20.0 25.0 30.0

x, inch

0.0

10.0

20.0

30.0

40.0

50.0

ps / pso

Data, 1x1

WIND, S−A

WIND, SST

NPARC (Ref. 12) 

(b) Cowl

Figure 15. Comparison of the static pressure

distributions along the body and cowl of the RBCC

strut-jet hypersonic inlet.

The comparison of the total pressure recoveries and

kinetic energy efficiencies is presented in Table 1.

Both CFD simulations over-predict the performance.

The kinetic energy efficiencies of the CFD simulations

were computed using the mass-averaged total pressures

and Mach numbers of the center and side passages.

The percent difference of the CFD values to the

experimental values is indicated in parenthesis. The

large differences in total pressure recovery become

smaller differences in kinetic energy efficiency.

Table 1. Performance of the Strut-Jet inlet.

ηpt ηKE

Data, 1x1 0.30 0.943

WIND, S-A 0.3186 (6.2%) 0.9463 (0.35%)

WIND, SST 0.3402 (13.4%) 0.9499 (0.73%)
NASA/TM—2002-211907 12

GTX Rig 2.1 Hypersonic Inlet

Figure 16. Geometry and Mach number contours

for the GTX Rig 2.1 sub-scale hypersonic inlet.

The GTX Rig 2.1 hypersonic inlet was a sub-scale

inlet model studied at NASA GRC as part of a current

research program to develop technologies for a rocketbased combined-cycle (RBCC) engine.13 This inlet was

of interest for a CFD validation study because the study

supported the use of the WIND code for the aerodynamic analysis of the inlets for the GTX program.

Figure 16 shows the geometry of the inlet. Only half

of the inlet is shown since it is symmetric about the

center plane. The inlet was a 220-degree section of an

axisymmetric inlet and consisted of a conical

centerbody and an axisymmetric cowl. The inlet was

mounted on a pylon that set the inlet above the

boundary layer generated on the vehicle body. The

vehicle has three such inlets mounted about the

circumference of the body. The experiment used a

body simulator fairing that started just ahead of the

nose of the centerbody. The centerbody was translated

as to provide a geometric contraction ratio of 7.14. The

half-angle of the conical centerbody was 12 degrees.

The experiment was conducted in the NASA GRC

1x1 Foot SWT.13 The inflow conditions were a Mach

number of 6.02, a total pressure of 146 psi, and a total

temperature of 811 °R. Figure 16 shows the Mach

number contours. The center-body generated a conical

shock that passed just outside of the cowl lip. The

conical shock interacted with the turbulent boundary

layer on the body fairing to generate local disturbances

of the boundary layer on the body.

The experimental data consist of streamwise static

pressure distributions along the centerbody and cowl at

various circumferential stations. This case can be

−10.0 −8.0 −6.0 −4.0 −2.0

X, inches

0.0

1.0

2.0

3.0

4.0

5.0

p, psi

Data

WIND (S−A)

WIND (Laminar)

(a) centerbody

−10.0 −8.0 −6.0 −4.0 −2.0

X, inches

0.0

1.0

2.0

3.0

4.0

5.0

p, psi

Data

WIND (S−A)

WIND (laminar)

(b) cowl

Figure 17. Comparison of the static pressures at the

centerline plane along the centerbody and cowl for

the GTX Rig 2.1 hypersonic inlet.

considered a subsystem validation case since the test

article was a sub-scale model of the actual inlet and

only examined the aerodynamics of the inlet.

The baseline grid consisted of 19 zones with a total

of 2469391 grid points. The grid points were clustered

near the surfaces to resolve the turbulent boundary

layers with y+ values less than 1.0 for the first grid

points off the surfaces. A coarse grid was extracted

from the baseline grid by removing every other grid

point in each coordinate direction.

The WIND simulations used the tunnel conditions as

its initial solution. The inlet was simulated in

supercritical mode in which the core flow remains

supersonic throughout the inlet. The baseline

simulation used the Spalart-Allmaras turbulence model.

The total pressure recovery from the CFD results was
NASA/TM—2002-211907 13

0.41998 on the baseline grid and 0.41032 on the coarse

grid, which was about a 2.3% difference and assured

that the baseline grid provided acceptable resolution.

Figure 17 shows the comparison between the CFD

results and the experimental data for the static pressure

distributions along the centerbody and cowl at the

centerline of the inlet. The experimental error in

measuring the static pressure was reported to be

0.02 psi, which was too small to be plotted as error

bars. The “peaks” and “valleys” indicate the presence

of oblique shocks bouncing through the inlet near the

throat. The results of the baseline simulation compare

well with the experimental data; however, a noticeable

“dip” in pressure occurs on the centerbody at

approximately x = –6.0 inches, which is not indicated in

the experimental data. This is the location at which the

cowl shock impinges onto the centerbody. The

experimental data suggests that there is a small

separation region. It was suggested that the flow was

not fully turbulent as assumed. Simulations were then

performed assuming laminar flow. Figure 17 shows

those distributions of the static pressure. The laminar

simulation indicated a small separation region and

higher values of static pressures at the location of the

“dip.” This suggested that the flow on the centerbody

was perhaps a mix of laminar and turbulent flow, which

was difficult to simulate with CFD methods and

confounds a conclusive validation assessment.

Summary and Conclusions

A series of cases has been presented for the

validation assessment of the WIND code that increases

the confidence in the use of WIND for the CFD

analysis of aerodynamic of aircraft inlets. The

assessment mainly examined the prediction of static

pressure distributions and pressure recovery. The use

of WIND to predict such things as inlet drag requires

further validation assessment. It should also be

understood that validation is an on-going process and

the use of any CFD code relies on a basic understanding

of the flow problem and of the flow physics involved.

References

1. AIAA, “Guide for the Verification and Validation

of Computational Fluid Dynamics Simulations,”

AIAA G-077-1998, 1998.

2. Bush, R.H., G.D. Power, and C.E. Towne, “WIND:

The Production Flow Solver of the NPARC

Alliance,” AIAA Paper 0935, January 1998.

3. WIND CFD Code web site:

http://www.grc.nasa.gov/www/winddocs.

4. Slater, J.W., “Verification Assessment of Flow

Boundary Conditions for CFD Analysis of

Supersonic Inlet Flows,” AIAA-2001-3882, July

2001.

5. Roache, P.J., Verification and Validation in

Computational Science and Engineering, Hermosa

Publishers, Albuquerque, New Mexico, 1998.

6. Stanitz, J.D., W.M. Osborn, and J. Mizisin, “An

Experimental Investigation of Secondary Flow in

an Accelerating, Rectangular Elbow,” NACA TN3015, October 1953.

7. Cavicchi, R.H., “A Three-Dimensional CFD

Investigation of Secondary Flow in an

Accelerating, 90° Elbow,” NASA/TM—2001-

211219. December 2001.

8. Abbott, J.M, “Aerodynamic Performance of Scarf

Inlets,” NASA TM–79055, January 1979.

9. Abbott, J.M. and J.W. Slater, “Computational

Study of the Aerodynamic Performance of ThreeDimensional Subsonic Inlets,” AIAA-2001-3886,

July 2001.

10. Wasserbauer, J.F., R.J. Shaw, and H.E. Neumann,

“Design of a Very-Low-Bleed Mach 2.5 MixedCompression Inlet with 45 Percent Internal

Contraction,” NASA TM X–3135, 1974.

11. Fernandez, R., C.J. Trefny, S.R. Thomas, and M.J.

Bulman, “Parametric Data from a Wind Tunnel

Test of a Rocket-Based Combined-Cycle Engine

Inlet,” NASA/TM—2001-107181, November

2001.

12. DeBonis, J.R. and S. Yungster, “Rocket-Based

Combined Cycle Engine Technology Development

– Inlet CFD Validation and Application,” NASA

TM–107274 (AIAA-96-3145), July 1996.

13. DeBonis, J.R., C.J. Trefny, and C.J. Steffen, Jr.,

“Inlet Development for a Rocket Based Combined

Cycle, Single Stage to Orbit Vehicle Using

Computational Fluid Dynamics,” AIAA-99-2239,

June 1999.

14. DeBonis, J.R. and C.J. Trefny, “Supersonic Wind

Tunnel Tests of a Half-Axisymmetric 12°-Spike

Inlet to a Rocket-Based Combined-Cycle

Propulsion System,” JANNAF, November 2000.

15. NPARC Verification and Validation web site:

http://www.grc.nasa.gov/www/wind/valid.
This publication is available from the NASA Center for AeroSpace Information, 301–621–0390.

REPORT DOCUMENTATION PAGE

2. REPORT DATE

19. SECURITY CLASSIFICATION

 OF ABSTRACT

18. SECURITY CLASSIFICATION

 OF THIS PAGE

Public reporting burden for this collection of information is estimated to average 1 hour per response, including the time for reviewing instructions, searching existing data sources,

gathering and maintaining the data needed, and completing and reviewing the collection of information. Send comments regarding this burden estimate or any other aspect of this

collection of information, including suggestions for reducing this burden, to Washington Headquarters Services, Directorate for Information Operations and Reports, 1215 Jefferson

Davis Highway, Suite 1204, Arlington, VA 22202-4302, and to the Office of Management and Budget, Paperwork Reduction Project (0704-0188), Washington, DC 20503.

NSN 7540-01-280-5500 Standard Form 298 (Rev. 2-89)

Prescribed by ANSI Std. Z39-18

298-102

Form Approved

OMB No. 0704-0188

12b. DISTRIBUTION CODE

8. PERFORMING ORGANIZATION

 REPORT NUMBER

5. FUNDING NUMBERS

3. REPORT TYPE AND DATES COVERED

4. TITLE AND SUBTITLE

6. AUTHOR(S)

7. PERFORMING ORGANIZATION NAME(S) AND ADDRESS(ES)

11. SUPPLEMENTARY NOTES

12a. DISTRIBUTION/AVAILABILITY STATEMENT

13. ABSTRACT (Maximum 200 words)

14. SUBJECT TERMS

17. SECURITY CLASSIFICATION

 OF REPORT

16. PRICE CODE

15. NUMBER OF PAGES

20. LIMITATION OF ABSTRACT

Unclassified Unclassified

Technical Memorandum

Unclassified

National Aeronautics and Space Administration

John H. Glenn Research Center at Lewis Field

Cleveland, Ohio 44135–3191

1. AGENCY USE ONLY (Leave blank)

10. SPONSORING/MONITORING

 AGENCY REPORT NUMBER

9. SPONSORING/MONITORING AGENCY NAME(S) AND ADDRESS(ES)

National Aeronautics and Space Administration

Washington, DC 20546–0001

Available electronically at http://gltrs.grc.nasa.gov

October 2002

NASA TM—2002-211907

AIAA–2002–0669

E–13597

WU–708–90–43–00

19

Validation of WIND for a Series of Inlet Flows

John W. Slater, John M. Abbott, and Richard H. Cavicchi

Computational fluid dynamics; Inlet flow; Subsonic flow; Supersonic flow;

Hypersonic flow

Unclassified -Unlimited

Subject Categories: 02 and 07 Distribution: Nonstandard

Prepared for the 40th Aerospace Sciences Meeting and Exhibit sponsored by the American Institute of Aeronautics and

Astronautics, Reno, Nevada, January 14–17, 2002. Responsible person, John W. Slater, organization code 5850,

216–433–8513.

Validation assessments compare WIND CFD simulations to experimental data for a series of inlet flows ranging in Mach

number from low subsonic to hypersonic. The validation procedures follow the guidelines of the AIAA. The WIND code

performs well in matching the available experimental data. The assessments demonstrate the use of WIND and provide

confidence in its use for the analysis of aircraft inlets.