Daniel L. Tweedt 

AP Solutions, Inc., Solon, Ohio

Computational Aerodynamic Simulations of a 

Spacecraft Cabin Ventilation Fan Design 

NASA/CR—2010-216330

December 2010
NASA STI Program . . . in Profi le

Since its founding, NASA has been dedicated to the 

advancement of aeronautics and space science. The 

NASA Scientifi c and Technical Information (STI) 

program plays a key part in helping NASA maintain 

this important role.

The NASA STI Program operates under the auspices 

of the Agency Chief Information Offi cer. It collects, 

organizes, provides for archiving, and disseminates 

NASA’s STI. The NASA STI program provides access 

to the NASA Aeronautics and Space Database and 

its public interface, the NASA Technical Reports 

Server, thus providing one of the largest collections 

of aeronautical and space science STI in the world. 

Results are published in both non-NASA channels 

and by NASA in the NASA STI Report Series, which 

includes the following report types:

• TECHNICAL PUBLICATION. Reports of 

completed research or a major signifi cant phase 

of research that present the results of NASA 

programs and include extensive data or theoretical 

analysis. Includes compilations of signifi cant 

scientifi c and technical data and information 

deemed to be of continuing reference value. 

NASA counterpart of peer-reviewed formal 

professional papers but has less stringent 

limitations on manuscript length and extent of 

graphic presentations.

• TECHNICAL MEMORANDUM. Scientifi c 

and technical fi ndings 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. Scientifi c and 

technical fi ndings by NASA-sponsored 

contractors and grantees.

• CONFERENCE PUBLICATION. Collected 

papers from scientifi c and technical 

conferences, symposia, seminars, or other 

meetings sponsored or cosponsored by NASA.

• SPECIAL PUBLICATION. Scientifi c, 

technical, or historical information from 

NASA programs, projects, and missions, often 

concerned with subjects having substantial 

public interest.

• TECHNICAL TRANSLATION. Englishlanguage translations of foreign scientifi c and 

technical material pertinent to NASA’s mission.

Specialized services also include creating custom 

thesauri, building customized databases, organizing 

and publishing research results.

For more information about the NASA STI 

program, 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 STI Help Desk 

at 443–757–5803

• Telephone the NASA STI Help Desk at

 443–757–5802

• Write to:

 NASA Center for AeroSpace Information (CASI)

 7115 Standard Drive

 Hanover, MD 21076–1320
Daniel L. Tweedt 

AP Solutions, Inc., Solon, Ohio

Computational Aerodynamic Simulations of a 

Spacecraft Cabin Ventilation Fan Design 

NASA/CR—2010-216330

December 2010

National Aeronautics and

Space Administration

Glenn Research Center

Cleveland, Ohio 44135

Prepared under Contract NNC06BA07B, Task 190
Acknowledgments

Final Report Submitted to ASRC Aerospace Corporation for Purchase Order Number AS6461 NASA Glenn Research Center Prime 

Contract Number NNC06BA07B, Task 190. The author would like to thank Dr. Rodrick V. Chima of the NASA Glenn Research 

Center for the many helpful discussions regarding computational fl uid dynamics code development and application. The author 

would also like to thank Hamilton Sundstrand for supplying the fan design information, and Mr. Timothy M. Roach of the NASA 

Glenn Research Center for extracting coordinate data from the supplied three-dimensional fan model.

Available from

NASA Center for Aerospace Information

7115 Standard Drive

Hanover, MD 21076–1320

National Technical Information Service

5301 Shawnee Road

Alexandria, VA 22312

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

Trade names and trademarks are used in this report for identifi cation 

only. Their usage does not constitute an offi cial endorsement, 

either expressed or implied, by the National Aeronautics and 

Space Administration.

Level of Review: This material has been technically reviewed by expert reviewer(s).
NASA/CR—2010-216330 1

Computational Aerodynamic Simulations of a 

Spacecraft Cabin Ventilation Fan Design 

Daniel L. Tweedt 

AP Solutions, Inc. 

Solon, Ohio 44139

Abstract 

Quieter working environments for astronauts are needed if future long-duration space exploration 

missions are to be safe and productive. Ventilation and payload cooling fans are known to be dominant 

sources of noise, with the International Space Station being a good case in point. To address this issue cost 

effectively, early attention to fan design, selection, and installation has been recommended, leading to an 

effort by NASA to examine the potential for small-fan noise reduction by improving fan aerodynamic 

design. As a preliminary part of that effort, the aerodynamics of a cabin ventilation fan designed by 

Hamilton Sundstrand has been simulated using computational fluid dynamics codes, and the computed 

solutions analyzed to quantify various aspects of the fan aerodynamics and performance. Four simulations 

were performed at the design rotational speed: two at the design flow rate and two at off-design flow rates. 

Following a brief discussion of the computational codes, various aerodynamic- and performance-related 

quantities derived from the computed flow fields are presented along with relevant flow field details. The 

results show that the computed fan performance is in generally good agreement with stated design goals. 

Introduction 

Quieter working environments for astronauts are needed if future long-duration space exploration 

missions are to be safe and productive. Ventilation and payload cooling fans are known to be dominant 

sources of noise, with the International Space Station being a good case in point. Noise management by 

means of externally applied mechanisms, such as surface acoustic treatments and mufflers, is common and 

effective, but tends to be costly in terms of subsystem performance and weight (Refs. 1 to 3). To address 

this issue more cost effectively, early attention to fan design, selection, and installation has been 

recommended. 

The current study is part of a larger effort to examine the potential for small-fan noise reduction through 

improvements in fan aerodynamic design. To initiate that effort, a cabin ventilation fan designed by 

Hamilton Sundstrand was selected for detailed analysis using computational fluid dynamics (CFD) codes. 

The analysis involves computationally simulating the aerodynamics of the fan at its design operating point, 

and then examining and quantifying various aspects of the fan aerodynamics and performance from the 

computed solutions. It is anticipated that these results, presented below, will serve as a reference for future 

aerodynamic design investigations aimed at quieter fan operation. 

In addition to simulating the cabin ventilation fan at its aerodynamic design point, two off-design 

simulations were also performed, one at a higher flow rate and the other at a lower flow rate, to quantify the 

fan operating characteristics at the design rotational speed. 

Fan Geometry and Design Operation 

Geometric and aerodynamic design information for the cabin ventilation fan design was supplied by 

Hamilton Sundstrand to the NASA Glenn Research Center. A computer-generated picture of the fan is 

shown in Figure 1, where a three-dimensional cutaway view reveals the fan assembly with all of its major 

components. The electric drive motor is an integral part of the subsystem, as is a flow straightener upstream 

of the fan. The inlet flow straightener is a honeycomb structure with an effective/flow path diameter of 

3.50 in., a thickness of 0.9375 in., and a cell size (or center-to-center cell spacing) of 0.1875 in.
NASA/CR—2010-216330 2

A meridional view of the fan system flow path is shown in Figure 2, which also indicates the location of 

each blade row. The rotor has nine blades, a tip clearance of 0.009 in., and a design rotational speed of 

16 000 rpm at 70 °F. The vertical dashed line below the hub contour in Figure 2 indicates the end of the 

rotor hub. Downstream of this location the hub is stationary. The stator has 11 blades, and each blade has a 

virtually uniform profile shape along its span. At the stator exit is an annular duct that extends downstream 

over three stator chord lengths, or four duct heights, and provides an annulus area increase before ending 

abruptly as the hub radius steps to zero at the back face of the centerbody. Blade section profiles for the 

rotor and stator are shown in Figure 3. 

The specified design flow rate for the fan is 150.3 ft3

/min, with a corresponding total-pressure rise of 

3.64 in. of water from inlet to exit. For this specification, the inlet is defined as the upstream side of the flow 

straightener, and the exit is defined as some (unspecified) location in the circular duct downstream of the 

centerbody. Design conditions at the inlet are a total pressure of 14.7 psia and a total temperature of 70 °F. 

The total-pressure drop across the inlet flow straightener is calculated from the average flow velocity 

using an empirical correlation provided by Hamilton Sundstrand. For the design flow rate, the calculated 

pressure drop is 0.0735 in. of water. 

Computational Fluid Dynamics 

Two different CFD codes were used to simulate the airflow through the fan system: an axisymmetric 

viscous solver called AVCS and a three-dimensional viscous turbomachinery solver called TSWIFT. 

Multiple solution domains (grid blocks) were used, with axisymmetric solutions coupled to 

three-dimensional solutions at mixing planes by means of a separate computer program called SMPI, 

developed as a companion program for AVCS and TSWIFT. SMPI was also used to couple rotating and 

stationary three-dimensional solutions together at mixing planes. In general, the three-dimensional 

TSWIFT solver was used for computational domains in and near blade rows, and the axisymmetric AVCS 

solver was used for computational domains upstream and downstream of the fan, sufficiently far away from 

the blade rows.1

The AVCS and TSWIFT codes use similar numerical algorithms; both solve the Reynolds-averaged 

Navier-Stokes equations on body-fitted grids using an explicit, finite-difference scheme. The codes include 

viscous terms in all grid directions, except that TSWIFT neglects the mixed-derivative viscous terms 

containing derivatives in the predominantly streamwise grid direction. The discretized equations are solved 

with a multistage Runge-Kutta time-marching scheme using a spatially varying time step, implicit residual 

smoothing, and preconditioning (Refs. 4 to 7). All simulations discussed herein were run using a two-stage 

Runge-Kutta scheme with a CFL (Courant-Friedrichs-Lewy) number of 2.5 and the H-CUSP (convective 

upwind split pressure) upwind scheme (Refs. 8 and 9). Initial solutions were run using the AUSM+

(advection upstream splitting method) upwind scheme (Ref. 10), which is considered the best for accuracy, 

but laminar-free shear-layer instabilities were encountered near the rotor blade tip and just downstream of 

the rotor trailing edge. It is believed that the instabilities are due to the relatively low Reynolds numbers 

involved, with concomitant laminar/transitional shear layers, and the H-CUSP scheme provides enough 

artificial dissipation to suppress the laminar instabilities and allow solution convergence. 

The TSWIFT code was derived from, and has the same basic features as the SWIFT code (Ref. 11)

developed by Chima at the NASA Glenn Research Center. TSWIFT also has a fairly general multiblock 

capability (when used with SYNCEX; see preceding footnote), includes the two-equation SST (shear stress 

transport) turbulence model developed by Menter (Ref. 12), and implements Giles’ two-dimensional, 

steady-state, nonreflecting boundary conditions (Refs. 13 and 14) at flow inlet, exit, and mixing-plane 

boundaries.2 Note that when a two-equation turbulence model is used, either the Wilcox k-ω model 

 1

All program-to-program communications, for mixing planes and direct block-to-block interfaces, were handled using 

a facility called SYNCEX (pronounced sink-ex). SYNCEX is a message-passing interface that enables two or more 

executing programs to efficiently exchange data on a single computer and/or over a network. 

2

The SMPI code also implements Giles’ two-dimensional, steady-state, and nonreflecting boundary conditions.
NASA/CR—2010-216330 3

(Ref. 15) or the Menter SST model, it is necessary at mixing planes to circumferentially average the 

computed turbulence properties on the upstream side of the mixing plane. In that case the turbulence kinetic 

energy, k, and the ratio of turbulence kinetic energy to turbulence dissipation, k/ω, are each mass-averaged. 

The resulting average values of k and (indirectly) ω are then used as inflow boundary values for the domain 

on the downstream side of the mixing plane.

For Mach number levels below about 0.3, it becomes necessary to use preconditioning, sometimes 

referred to as artificial compressibility, to obtain good solution convergence. The preconditioning can also 

be used at higher Mach numbers, typically because it has been found to generally improve convergence 

behavior. Mach number levels in the current fan system are nominally around 0.1 or less, except in the rotor 

where blade-tip-relative Mach numbers exceed 0.3. 

Initial solution results revealed that it was also necessary to use double precision for CFD solver 

execution. Single precision was sufficient for grid generation, solution preprocessing, and solution 

postprocessing, but proved inadequate for solver execution because of truncation errors in density and 

pressure. In general, as Mach number levels approach zero, the dimensionless density and pressure each 

approach a constant positive value with an order of magnitude of one. The resulting flow-field solutions 

involve relatively small spatial variations in density and pressure, such that property differences computed 

in single precision are significantly affected by the truncation error. 

Fan System Aerodynamic Simulations 

The aerodynamic simulations were performed for air modeled as a perfect gas with a ratio of specific 

heats, γ, equal to 1.400, and with inlet total (stagnation) flow conditions set at standard day sea-level (SSL) 

values. Since a nonstandard inlet temperature was specified for the design, it was necessary to apply a 

correction to values of rotational speed, volumetric flow rate, and unit Reynolds number to maintain 

aerodynamic similarity. The SSL-corrected values were used as input data for the CFD solver, and are now 

being used for standardized data presentations and comparisons. For the inlet total temperature of 70 °F, the 

total-temperature correction factor, θ, is equal to 1.0218. Note that a total-pressure correction is not 

necessary because for an inlet total pressure of 14.7 psia, the total-pressure correction factor, δ, is equal to 

1.0000. Applying the temperature correction gives a design rotational speed, N θ , of 15 828 rpm, a 

design flow rate, Q θ , of 148.7 ft3

/min, and a unit Reynolds number based on inlet total conditions, 

(ρc/μ)SSL δ/θ7/6, of 5.768×105 in.–1

, where ρ is density, c is the speed of sound, and μ is dynamic viscosity. 

The fan inlet conditions are specified for the upstream side of the flow straightener. The inlet 

computational domain, however, begins on the downstream side, so the total pressure at the computational 

boundary must include the pressure loss of the straightener. Consistent with the Hamilton Sundstrand 

pressure-loss correlation for the straightener, applied at the specified design flow rate of 150.3 ft3

/min at 70 

°F, a total-pressure drop of 0.0735 in. of water was used. The corresponding total-pressure ratio for the 

straightener is 0.999819, which is the value specified as input to the CFD solver. Note that this value was 

used even though the SSL-corrected design flow rate is slightly different. It was also used at the two 

off-design flow rates that differ from the design value by several percent. 

The effects of turbulence were modeled using the Wilcox k-ω turbulence model (Ref. 15), with 

free-stream turbulence at the upstream computational boundary set at 1.0 percent, along with a turbulence 

(eddy) viscosity equal to 0.5 times the molecular viscosity. The corresponding turbulence kinetic energy is 

1.68×10–7 (dimensionless; multiply by reference speed-of-sound squared to obtain a dimensional value). 

Two versions of the model were applied, a high-Reynolds-number version and a low-Reynolds-number 

version, the latter being considered more appropriate and accurate for the cases being computed. The 

high-Reynolds-number model is known to simulate the onset of transition much too soon, which potentially 

could have a significant impact on the simulation results at such low Reynolds numbers; blade-chord 

Reynolds numbers are on the order of 70 000 for the rotor and 45 000 for the stator. Applying both models 

allows an assessment to be made of the relative importance of this effect. Note that both models were 
NASA/CR—2010-216330 4

applied only at the design flow condition; at the two off-design flow rates, the low-Reynolds-number model 

was used. 

For computational efficiency, the fan solution and the discharge flow field at the fan system exit were 

computed separately; that is, the exit discharge solution was not close-coupled to the fan solution. Both 

computational domains include a section of the annular diffuser duct, so there is a substantial overlap 

region. The fan solution, the domain of which terminates at the exit of the annular duct, was computed first, 

with the exit-tip static pressure specified and simple radial-equilibrium solved to determine the radial 

static-pressure distribution. For the design flow simulation, the exit static pressure was adjusted iteratively 

to achieve the design flow rate, and the same pressure value was used for both the low- and 

high-Reynolds-number turbulence model simulations. The corresponding solution for the exit discharge 

region was then computed using the fan solution to supply upstream boundary values. The exit region 

solution mainly provides computational total-pressure loss results for the discharge flow, as well as 

information about the extent of the separation (reverse flow) bubble downstream of the annular diffuser 

centerbody. 

Computational Grids 

Hub and tip/casing flow path coordinates were modified slightly to avoid slope discontinuities (sharp

corners), since cubic splines were used for interpolation during grid generation. The modifications involved 

deleting sharp corner points, while adding points to create a small fillet. 

A meridional view of the fan system grid blocks is shown in Figure 4, where different colors are used to 

differentiate nine different blocks. For clarity, only every other grid line has been drawn for each grid. The 

blue and light-blue blocks on the far left in the inlet duct, and the blue block on the far right in the annular 

diffuser duct, are two-dimensional/axisymmetric H-grids. The location of the far-left boundary corresponds 

to the downstream side of the inlet flow straightener, and the lower boundary of the light-blue inlet block is 

on the fan centerline. The two black blocks represent three-dimensional blade row C-grids: one on the left 

for the rotor and the other on the right for the stator. The two green blocks represent three-dimensional 

H-grids that extend the rotor domain upstream and downstream, and the two red blocks represent 

three-dimensional H-grids that extend the stator domain upstream and downstream. Not indicated in the 

figure is a rotor-tip clearance gap O-grid block. 

The system exit domain contains three two-dimensional/axisymmetric grid blocks, shown in Figure 5. 

The front part of the blue block, the part located within the annular diffuser duct, is identical to the grid used 

for the fan system (see Fig. 4, blue grid block on right). The lower boundary of the light-blue base grid and 

the violet downstream extension tube grid is on the fan centerline. 

Both of the inlet duct grid blocks were generated using a Poisson partial differential equation (PDE) 

solver, otherwise known as an elliptic grid generator, which produces grids with good boundary-normal 

node clusterings and spacings, and generally good local orthogonality. The annular diffuser duct and 

system exit grid blocks were generated using an algebraic method because the grid lines are naturally 

orthogonal, or nearly so. 

The blade row grids, except for the rotor exit and stator exit H-grid blocks, were generated using a 

computer program called TTGRID, which is a modified version of TCGRID (Ref. 16), a three-dimensional 

grid generator for turbomachinery developed by Chima at the NASA Glenn Research Center. TTGRID 

applies an elliptic PDE solver to the streamwise-pitchwise (blade-to-blade) mesh surfaces of blade row Cand H-grids. 

A three-dimensional view of the rotor grid is shown in Figure 6. Note that the (green) upstream/inlet 

H-grid overlaps the (black) C-grid and has node-to-node alignment with it. The (green) downstream/exit 

H-grid also overlaps the C-grid, but the grid nodes are not aligned. An axial-circumferential (blade-to

-blade) mesh plot of the rotor grid at the blade tip is shown in Figure 7(a), which also includes magnified 

views of the blade leading and trailing edge regions. The tip clearance gap O-grid block (light gray)

overlaps the C-grid with node-to-node alignment. A circumferential-radial view of the tip clearance grid at 

a midchord cross section is included in Figure 7(a), on the right. An axial-circumferential mesh plot of the 
NASA/CR—2010-216330 5

rotor grid at the hub is shown in Figure 7(b), along with three circumferential-radial-view mesh plots of the 

grid at the cross sections indicated. 

A three-dimensional view of the stator grid is shown in Figure 8. Many of the comments in the previous 

paragraph also apply to the stator grid, except that the stator does not have an endwall clearance gap, and the 

upstream and downstream extension H-grid blocks are red. An axial-circumferential mesh plot of the stator 

grid at midspan is shown in Figure 9, along with three circumferential-radial-view mesh plots for the cross 

sections indicated. 

Turbulent boundary-layer flow solutions near solid walls always involve direct computation of the 

viscous sublayer; that is, wall functions are not used. It is important, therefore, that node spacings at solid 

walls be sufficiently small. The nominal wall-normal spacing at hub and tip endwalls is 0.00025 in., and at 

blade surfaces is 0.00010 in. Corresponding inner-variable wall distances, y+, are typically between 1.0 and 

2.0 at the endwalls, and between 0.2 and 0.8 at blade surfaces. 

Table 1 summarizes the grid blocks and their sizes for the fan system computational domain, and 

Table 2 summarizes the grid blocks and their sizes for the system exit computational domain. 

TABLE 1.—FAN SYSTEM COMPUTATIONAL GRID BLOCKS 

Grid block Size

(I×J×K)

Number of 

nodes

Inlet duct inner H-grid (2–D) 81×1×81 6,561

Inlet duct outer H-grid (2–D) 81×1×81 6,561

Rotor inlet H-grid 13×38×85 41,990

Rotor blade C-grid 201×49×85 837,165

Rotor exit H-grid 73×89×77 500,269

Rotor tip clearance O-grid 157×15×17 40,035

Stator inlet H-grid 13×32×73 30,368

Stator blade C-grid 201×49×73 718,977

Stator exit H-grid 65×89×73 422,305

Exit duct H-grid 29×1×73 2,117

TABLE 2.—FAN EXIT COMPUTATIONAL GRID BLOCKS 

Grid block Size

(I×J×K)

Number of 

nodes

Exit duct/outer H-grid (2–D) 69×1×73 5037

Exit duct/inner H-grid (2–D) 61×1×49 2989

Exit extension tube H-grid (2–D) 57×1×89 5073

Aerodynamic Simulation Results 

Fan system CFD results are presented below using averaged and nonaveraged data. Circumferential 

(pitchwise) averaging of the three-dimensional flow fields was performed on a structured meridional grid 

for some selected solutions, allowing contour plots to be generated for the averaged flow fields. Detailed 

comparisons are made at the axial stations indicated with red vertical dashed lines in Figure 10. The stations 

are labeled as indicated. Note that the vertical blue lines in Figure 10 show mixing plane locations, and the 

(near-) vertical gray lines show grid block interface locations. Stations 1a and 4b, respectively, are at the 

upstream and downstream boundaries of the computational domain(s), and are included only for 

completeness, as well as possible future reference. 
NASA/CR—2010-216330 6

Overall averages, obtained by spanwise (radial) averaging of the circumferentially averaged flow field, 

were calculated at stations 2b, 3d, and 4a, to provide representative performance numbers for the rotor and 

fan stage. These results are summarized below in Tables 3 and 4, and are presented first because they 

provide a convenient overview of the operating points and performance values computed for the fan. Note 

that all simulated cases are included, off-design as well as design, and that the left column indicates the 

turbulence model used. A fan performance map generated from these results is shown in Figure 11, where 

total-pressure rise and hydraulic efficiency are graphed against volumetric flow rate. 

TABLE 3.—COMPUTED ROTOR PERFORMANCE

Turbulence 

model

Flow rate

Q θ ,

ft3/min

Pressure rise

Δpt,2b,

in. water

Work input

Δht,2b,

in. water

Hydraulic efficiency

ηH,2b

Rotor torque

T/δ,

in.-oz

Low Re 143.18 4.523 5.409 0.8362 7.779

Low Re 148.60 4.313 5.156 0.8366 7.695

Low Re 153.73 4.097 4.909 0.8345 7.579

High Re 148.37 4.299 5.129 0.8381 7.644

TABLE 4.—COMPUTED FAN STAGE PERFORMANCE

Turbulence 

model

Flow rate

Q θ ,

ft3

/min

Pressure rise

Δpt,3d,

in. water

Work input

ΔH,3d,

in. water

Pressure rise

ηH,3d

in. water

Hydraulic efficiency

ηH,4a

Low Re 143.18 3.899 0.7208 3.658 0.6763

Low Re 148.60 3.690 0.7157 3.435 0.6663

Low Re 153.73 3.480 0.7090 3.209 0.6538

High Re 148.37 3.720 0.7252 3.441 0.6709

Figure 11, as well as in Tables 3 and 4, show the turbulence model version has only a small impact on 

the computed overall performance for the fan, at least for operation near the aerodynamic design point. At 

the design flow rate, the computed total-pressure rise is 3.435 in. of water for the fan system (station 4a, 

low-Reynolds-number model), which is 5.6 percent less than the design objective of 3.640 in. of water. The 

corresponding hydraulic efficiency of 0.6663 also falls below the design value, estimated to be 0.686. 

Although the computed total-pressure rise and hydraulic efficiency are less than the values anticipated for 

the design, the general level of agreement is considered to be good. 

Referring again to Figure 11, notice the relative amount of total-pressure loss incurred between stations 

3d and 4a. That loss, the exit discharge total-pressure loss, is significant. At the design flow rate the 

discharge loss is 0.255 in. of water, which is equal to 7.4 percent of the total-pressure rise for the entire fan 

system. 

Several contour plots showing the fan system flow field and the exit discharge region flow field, for the 

design flow rate, are contained in Figures 12 and 13, respectively, where for Figure 12 the 

three-dimensional blade-row flow solutions were mixed-out averaged in the circumferential direction.3

Note that the grid blocks in Figure 4 correspond to the contour plots of Figure 12, the grid blocks in Figure 5 

correspond to the contour plots of Figure 13, and all of the contour plots were generated from the solution 

set obtained with the low-Reynolds-number k-ω turbulence model. The entropy rise and turbulence kinetic 

energy plots involve dimensionless values, with entropy rise nondimensionalized by the gas constant, R, for 

air, and turbulence kinetic energy normalized by the inlet kinetic energy. The inlet kinetic energy is based 

on the magnitude of the mean flow velocity at the flow straightener, Q A θ , which has a value of 

 3

Turbulence kinetic energy was mass-averaged in the circumferential direction.
NASA/CR—2010-216330 7

37.09 ft/s at the design flow rate. Note also that Figure 13 uses the contour legends in Figure 12, as 

appropriate, with static-pressure rise using the same legend as total-pressure rise, and axial velocity using 

the same legend as velocity magnitude. 

Noteworthy in Figure 12 are the relatively thick, higher-entropy regions generated at the rotor hub and 

tip, but especially at the tip. The regions widen as the flow convects downstream, until at the stator they 

encompass almost 30 percent of the span by the hub, and about 45 percent of the span by the tip. Such 

extensive endwall viscous-loss regions are somewhat unusual, and are a direct result of the relatively low 

Reynolds numbers involved. Simple considerations from flat-plate boundary-layer theory suggest that this 

effect should be expected, although at the tip the highly viscous, three-dimensional nature of the clearance 

flow seems to amplify it considerably. When the Reynolds number for a flat-plate boundary-layer flow is 

decreased by a factor of 10, for example, the thickness of the layer increases by a factor of 10 (equal to 

3.2) if it is laminar, or by a factor of about 5 10 (equal to 1.6) if it is turbulent. Lower Reynolds numbers 

are also generally associated with delayed, or even nonexistent, laminar-to-turbulent transition, as well as 

with decreased turbulence viscosity levels. 

Also of interest in Figure 12 are the inlet- and exit-diffuser flow fields. The velocity magnitude plot

shows the flow in the inlet undergoes a rapid acceleration as it enters the annular passage. On the 

hub/spinner nose, the flow is overexpanded (accelerated to excessive velocities) because of the high 

endwall curvature. This overexpansion, combined with a small separation bubble (not visible) just above 

the sharp corner, leads to a thicker hub boundary layer going into the rotor and adds to the static-pressure 

rise across the rotor. In the exit diffuser, the flow is aerodynamically clean along the hub, but not along the 

tip endwall where a viscous boundary-layer separation exists. The separated (reverse flow) region is large 

enough that the average axial velocities are slightly negative very near the endwall. Later, more detailed 

results will be provided that show the flow structure of the separated region is highly three-dimensional. At 

the hub there is no reverse flow until after the flow discharges into the downstream tube, as revealed by the 

axial velocity contour plot in Figure 13. The thick black contour in that plot corresponds to a value of zero 

and outlines a region of reverse flow (negative axial velocity) just downstream of the diffuser centerbody. 

Axial distributions of static-pressure rise at the hub and tip endwalls for the fan system and the exit 

discharge region are shown in Figures 14 and 15, respectively. These results correspond to the design flow 

rate and involve circumferentially mixed-out averaged flow-field solutions. Both the low- and 

high-Reynolds-number turbulence model results are included for comparison, but the differences between 

them are small. Blade row locations are indicated by thin vertical lines with labels, so various sections of the 

flow path can be identified along with corresponding static-pressure rise changes and gradients. As 

expected, static pressure generally increases in the axial/streamwise direction; however, the static-pressure 

rise and associated pressure gradients are by far the largest in and across the rotor. Static-pressure recovery 

for the diffuser is good, with static pressure increasing by 0.780 in. of water from station 3a to station 3d. 

The corresponding total-pressure loss is somewhat high, however, at 0.308 in. of water. When this loss is 

added to the discharge loss, the total-pressure loss for the entire diffusion process (station 3a to station 4a) is 

0.563 in. of water, or 16.4 percent of the total-pressure rise for the entire fan system, for a corresponding 

static-pressure rise of 1.176 in. of water. 

Line graphs of circumferentially mixed-out averaged results at all axial stations from 1b through 3d, for 

the design flow rate, are presented in Figures 16 through 23, respectively. A fairly extensive set of graphs is 

included for documentation purposes, so many of the graphs are not discussed. Again, results for the lowand high-Reynolds-number turbulence models are included for comparison, and the differences between 

them are generally small. Note that the contour plots of Figure 12 may be helpful for interpreting these line 

graphs, by providing a broader perspective for the station data. 

Referring to Figures 17(a) and 19(a), corresponding respectively to stations 2a and 2b, the 

total-pressure rise and work input distributions downstream of the rotor are fairly flat for much of the 

passage, that is, from about 15 to 70 percent of passage height, in which region the hydraulic efficiency is 

high at around 0.950. Near the endwalls, the efficiency decreases as a result of higher total-pressure losses 

there, appearing as higher entropy in the contours of Figure 12. Note that it is common practice with pumps 
NASA/CR—2010-216330 8

and low-speed fans to calculate hydraulic efficiency using work input based on changes in tangential 

velocity multiplied by blade speed, Δ(uvθ), a kinematic quantity. At low Reynolds numbers, however, this 

approach leads to excessive errors because viscous effects are too prevalent. To avoid such errors here, the 

work input has been calculated using total-enthalpy rise, Δ(ht), a thermodynamic quantity. A comparison of 

the two methods at station 2a is provided in Figure 18, where the errors are substantial near the endwalls. 

Similarly, it would be more accurate to use thermodynamic adiabatic efficiency rather than hydraulic 

efficiency, but convention favors the latter. In general, calculated hydraulic efficiencies are greater than 

corresponding adiabatic efficiencies, with the differences depending on the particular conditions involved, 

and decreasing to zero as flow compressibility approaches zero. For all cases presented herein, 

representative hydraulic efficiency values are greater than adiabatic efficiency values by an amount 

somewhere between 0.0023 and 0.0038.

As the rotor exit flow convects downstream, first through the stator blade row, and then through the 

annular diffuser, the flow property profiles become progressively more rounded; that is, less flat (compare 

results at stations 2a through 3d in Figs. 17(a) through 23(b)). Viscous dissipation and blade-row generated 

secondary flows are the fluid dynamic mechanisms producing this effect, both working to expand the 

influence of the endwalls by mixing the endwall fluid with the high-efficiency core flow. Most of the rotor 

exit flow swirl (negative tangential velocity) is removed by the stator, which leaves less than 8° of residual 

swirl at its exit. Near the hub and tip endwalls, secondary flow effects in the stator blade row lead to some 

overturning, that is, to positive tangential velocities at the stator exit (see station 3a in Fig. 20), but the 

amount of overturning is not excessive. 

Line graphs showing several blade row parameters relevant to the aerodynamic design and 

performance of the fan are presented in Figures 24 and 25. Parameters for the rotor blade row are shown in 

Figure 24, and parameters for the stator blade row are shown in Figure 25. The results graphed are based on 

circumferentially mixed-out average quantities at blade leading and trailing edge meridional stations, and 

results for the low- and high-Reynolds-number turbulence models are both included for comparison. For 

the rotor (see Fig. 24(a)), the graph of total-pressure loss coefficient shows low losses over most of the span, 

corresponding to the high hydraulic efficiencies discussed earlier for the same approximate region of the 

passage. Near the hub and tip endwalls, however, the loss coefficients are much higher due to the additional 

losses generated by the endwall flows. The high-loss regions, especially the tip, involve a substantial 

fraction of the passage flow, and therefore have a large effect on overall performance. The graph of 

diffusion factor shows a nearly constant value of around 0.4 everywhere outside the endwall flow regions, 

indicating low to moderate levels of aerodynamic blade loading, at least by conventional standards. Near 

the hub and tip, diffusion factor follows roughly the same trend as loss coefficient. Given the nominal 

diffusion factor value of 0.4, excluding the high-loss regions, the amount of endwall-generated loss 

(entropy) seems inordinately large and demonstrates the increased influence of viscosity at low Reynolds 

numbers. 

For the stator (see Fig. 25(a)), the graph of loss coefficient indicates moderate total-pressure loss levels, 

and the graph of diffusion factor reveals low to moderate blade loading. Notice that the loss coefficients 

very near the endwalls are negative (truncated by the graph), but that the maximum values are somewhat 

close by, that is, in the general vicinity of each endwall. This is a result of secondary flow migration in the 

blade row, where low-momentum fluid is transported away from the endwalls. Although the diffusion 

factors are fairly low by conventional standards, it is noteworthy that the flow deviation angles are 

relatively large (see Fig. 25(a)), around 15° over most of the span. Apparently, the large deviation angles 

are also a low-Reynolds-number effect. 

The rotor blade-to-blade flow field in the rotating frame-of-reference is shown in Figure 26 for three 

stream surfaces of revolution: one at 85 percent of passage flow (near the tip), one at 50 percent of passage 

flow (near midspan), and one at 15 percent of passage flow (near the hub). Contours of relative velocity 

magnitude are plotted using the same contour range for all three stream surfaces, and flow solutions for both 

the low- and high-Reynolds-number turbulence models are presented for comparison. In Figure 27, 

contours of turbulence kinetic energy (normalized by inlet kinetic energy) are shown for the 50 percent of 

passage flow stream surface, with small red arrows indicating locations where laminar-to-turbulent 
NASA/CR—2010-216330 9

boundary layer transition occurs. Transition behavior and turbulence development on the blade surface for 

the near-hub and near-tip stream surfaces are generally similar to that at midspan, so turbulence kinetic 

energy contours are not shown for those locations.4 Line graphs showing chordwise distributions of rotor 

blade surface pressure coefficient, Cp, for the 15, 50, and 85 percent of passage flow stream surfaces are 

provided in Figure 28. The pressure coefficient accounts for the effects of rotation and radius change and 

the reference values for static and relative total pressure are based on the mixed-out average conditions at 

the blade leading edge. In these line graphs, the top curve corresponds to the blade pressure surface, the 

bottom curve corresponds to the blade suction surface, and the vertical spacing between the curves is 

related to the local aerodynamic loading (static pressure difference) at a particular chordwise location. In 

the contour plots, the upper blade surface corresponds to the suction surface. 

In general, the blade-to-blade flow field for all three stream surfaces is aerodynamically clean and 

robust. The pressure coefficient distributions are all similar and show that the rotor blade loading is 

maximum at the front of the blade, very near the leading edge, and decreases almost linearly from about 10 

percent of the chord to the trailing edge. On the blade suction surface, the static-pressure gradient, or rate of 

flow deceleration/diffusion, is fairly uniform, and the boundary layer remains attached. With the 

low-Reynolds-number turbulence model, the blade boundary layers are mostly laminar, and the 

suction-surface transition to turbulence takes place somewhere between midchord and the trailing edge, 

depending on spanwise location (see footnote). At midspan, the transition occurs at 75 percent chord (see 

small red arrow in Fig. 27). With the high-Reynolds-number model, transition to turbulence generally 

occurs at the front of the blade, on both sides, and the resulting turbulent boundary layers are noticeably 

thicker, as is the wake. Aside from that, however, the flow fields are very similar. It might be added that it is 

unusual to have a nearly all-laminar blade flow, such as that simulated using the low-Reynolds-number 

model, but the solution is probably correct, or is at least more accurate than the solution obtained using the 

high-Reynolds-number model. 

Relative velocity magnitude and turbulence kinetic energy contour plots in Figure 29 show the 

computed flow field in and around the rotor tip clearance gap, which has a height equal to 2.0 percent of 

span. The blade-to-blade contours in Figures 29(a) and 29(b) were calculated on a surface of revolution 

located spanwise near the middle of the clearance gap, and the contours in Figure 29(c) were calculated on 

a plane perpendicular to the axis of rotation at a midchord axial location (see Figs. 1 and 2). A comparison 

of the flow-field solutions obtained with the low- and high-Reynolds-number turbulence models reveals 

significant differences, but the impact on overall performance is small, and both solution sets indicate 

acceptable aerodynamic characteristics. Notable is the lack of turbulence for most of the tip flow region as 

computed using the low-Reynolds-number model. Of particular interest is the laminar-free shear layer 

between the tip jet and the flow just below the jet, on the suction side of the blade (see Fig. 29(c), left side of 

figure, right side of blade). The region below the shear layer is also laminar and involves a radial-tangential 

secondary flow that is considerably larger than that computed using the high-Reynolds-number turbulence 

model (compare to right side of Fig. 29(c)). The free shear layer itself exhibits a peculiar flow instability, 

mentioned earlier in the discussion of the CFD codes, which led to numerical difficulties for the AUSM+ 

upwind scheme. Evidence of the instability can be seen in Figure 29(a), in the left plot, but its existence is 

far more apparent in Figure 30, which shows entropy contours at a spanwise location about 0.001 in. above 

the blade tip. Property oscillations in the chordwise directions on the blade suction side reveal a wavetype 

instability for the low-Reynolds-number turbulence model (left plot), but not for the high-Reynolds-number 

model (right plot). The physical existence of such waves is uncertain, but their general appearance is 

reminiscent of that observed for various other types of unstable laminar-shear flows at the onset of 

turbulence (Ref. 17). 

The rotor exit flow field at station 2b, located over one chord-length downstream of the rotor blade row, 

is shown in Figure 31, where contour plots of relative velocity magnitude, total-pressure rise, entropy rise, 

and turbulence kinetic energy are presented. Solution results for both the low- and high-Reynolds-number 

 4

For the low-Reynolds-number turbulence model, boundary layer transition on the blade suction surface occurs at 

midchord, near the hub, and slightly upstream of the trailing edge near the tip. 
NASA/CR—2010-216330 10

turbulence models are included, and are generally similar. Close inspection reveals some differences in 

local flow features, but their significance is thought to be minimal. Note that the contour levels of relative 

velocity magnitude are the same as those in Figures 26 and 29, that total-pressure rise is in the stationary 

system, entropy rise is nondimensionalized by the gas constant, and turbulence kinetic energy is normalized 

by inlet kinetic energy (see discussion of Fig. 12). Rotation is in the direction indicated, so the wakeconvecting flow field is moving counterclockwise, and the circumferential property variations are, in the 

stationary frame of reference, transient fluctuations. Tone noise is generated as this periodic unsteady flow 

interacts with the stator blades at the blade-passing frequency of the rotor. Although the stator blade row is 

actually located further downstream, it is close enough that the fluctuation patterns and amplitudes there 

should be similar to those existing at station 2b. No effort has been made as yet to predict the tone noise, and 

the acoustic complexities involved require specialized methods to do so. At the risk of oversimplification, 

however, it might be suggested that the total-pressure contours give at least some impression of the 

noise-generating wake intensity. It might be added that turbulence kinetic energy is also related to noise, but 

to noise of a different type, namely, broadband noise. 

The stator blade-to-blade flow field in the stationary frame of reference is shown in Figure 32 for the 

same three stream surfaces of revolution used for the rotor: 85, 50, and 15 percent of passage flow. Velocity 

magnitude and turbulence kinetic energy contours are plotted, each using the same contour range for all 

three stream surfaces, and flow solutions for both the low- and high-Reynolds-number turbulence models 

are presented for comparison. Small red arrows in the turbulence kinetic energy plots indicate locations of 

laminar-to-turbulent transition on the blade surface, except at 85 percent of passage flow where the blade 

boundary layer is turbulent all the way from the leading edge. Line graphs showing chordwise distributions 

of stator blade surface pressure coefficient, Cp, for all three stream surfaces are provided in Figure 33. The 

reference values of static- and total-pressure for the pressure coefficient are based on the mixed-out average 

conditions at the blade leading edge. The top curve in each line graph corresponds to the blade pressure 

surface, the bottom curve corresponds to the blade suction surface, and the vertical spacing between the 

curves is related to the local aerodynamic loading (static pressure difference) at a particular chordwise 

location. In the contour plots, the lower blade surface corresponds to the suction surface. 

The contour plots show the flow field downstream of the stator (in the diffuser duct) differs a lot for the 

three stream surfaces, but that the blade-to-blade flow field within the stator blade row itself is basically the 

same, except near trailing edge on the suction surface. Differences due to the turbulence model are 

noticeable, but of only minor significance overall. The general similarity in the stator blade-to-blade flow is 

also seen in the pressure coefficient distributions, which reveal that the blade loading is fairly constant over 

the front 40 percent of the blade, and then decreases gradually to the trailing edge. Most of the flow 

diffusion (deceleration and static-pressure rise) on the blade suction surface takes place from about 40 to 

70 percent of blade chord. On the blade suction surface near the hub and tip, the boundary layer separates 

before reaching the trailing edge; separation near the tip occurs at around 65 percent of chord and near the 

hub at around 75 percent of chord. The tip separation, however, is disproportionately more severe, as the 

contour plots suggest. On the suction surface near midspan there is no boundary-layer separation at the 

trailing edge, although for the low-Reynolds-number turbulence model there is a small laminar separation 

bubble, followed by transition to turbulence, at around 60 percent of chord. 

Contour plots showing the stator exit flow field at station 3c, located over one chord-length 

downstream of the stator blade row, are provided in Figure 34. Plots of velocity magnitude, total-pressure 

rise, entropy rise, turbulence kinetic energy, and axial velocity are presented for both the low- and 

high-Reynolds-number turbulence models. Note that the contour levels of velocity magnitude are the same 

as those in Figure 32, that entropy rise is nondimensionalized by the gas constant, and turbulence kinetic 

energy is normalized by inlet kinetic energy (see discussion of Fig. 12). The legend for axial velocity is the 

same as for velocity magnitude, so it does not include values below zero, even though negative axial 

velocities are included in the contour plot. As has generally been the case, the turbulence-model-related 

differences are relatively minor. 

The three-dimensional structure and extent of the tip endwall separation in the annular diffuser duct can 

be readily inferred from the contour plots in Figure 34 and by comparing the velocity magnitude plots in 
NASA/CR—2010-216330 11

Figure 34(a) to those in Figure 32. From the structure of the separation it is apparent that both wake and 

endwall low-momentum fluids are contained in it. The exact region where the axial velocity is negative 

(indicating upstream fluid migration) is outlined in Figure 34(c) by the thick black contour corresponding to 

an axial velocity of zero. As the contour plots in Figures 34(a) (bottom) and 34(b) (top) show, this region is 

also associated with a relatively low total-pressure rise and a relatively high entropy rise. The location and 

extent of the reverse-flow region further upstream, at station 3b, can be seen in Figure 35, which also shows 

axial velocity contours and more clearly reveals the wake-endwall nature of the separation. 

Summary and Concluding Remarks 

The aerodynamics of a cabin ventilation fan designed by Hamilton Sundstrand was successfully 

simulated using CFD codes, and the computed solutions were analyzed to quantify various aspects of the 

fan aerodynamics and performance. Four simulations were performed at the design rotational speed: two at 

the design flow rate and two at off-design flow rates. The two design-flow simulations involved different 

versions of the turbulence model: one more suitable for high-Reynolds-number flows and the other for 

low-Reynolds-number flows. Results show that the turbulence model version had only a small impact on 

the computed aerodynamics, in spite of significant differences in the turbulence solution. 

Fan performance quantities derived from the computed flow fields are in generally good agreement 

with stated design goals. The design, however, seems to leave some room for aerodynamic improvement, 

especially in the exit diffuser. The rotor flow is aerodynamically clean, as is also the stator flow, except near 

the trailing edge at the stator tip where boundary layer separation on the suction surface is somewhat 

excessive. In the annular diffuser downstream of the stator, the total-pressure loss is higher than what might 

be expected, and the flow in the tip region involves a substantial wake-endwall separation. The 

total-pressure loss for the diffuser exit discharge also seems to be higher than what should be practically 

achievable. In the fan inlet the flow is well behaved, although there is a small separation above the sharp lip 

on the hub/spinner nose. More importantly, the high curvature of the nose surface produces an 

overexpansion of the flow, which increases the hub static-pressure rise across the rotor significantly beyond 

what is really necessary. 

References 

1. Munch, C.L.: Noise Reduction Study of Orbiting Workshop Ventilation Fans. NASA CR–102287 

(Wyle Laboratories Research Staff Technical Memorandum 69–4), 1969. 

2. Misoda, John; and Magliozzi, Bernard: Fan and Pump Noise Control. NASA CR–128986 (Hamilton 

Standard SVHSER 6183), 1973. 

3. Lovell, John S.; and Magliozzi, Bernard: Design Guidelines for Quiet Fans and Pumps for Space 

Vehicles. NASA/CR—2008-215427 (Hamilton Standard SVHSER 6225), 2008. 

4. Chima, R.V.: Viscous Three-Dimensional Calculations of Transonic Fan Performance. CFD 

Techniques for Propulsion Applications, AGARD Conference Proceedings CP510 (NASA 

TM–103800), AGARD, 1992, pp. 21–1 to 21–19. 

5. Chima, R.V.; and Yokota, J.W.: Numerical Analysis of Three-Dimensional Viscous Flows in 

Turbomachinery. AIAA J., vol. 28, no. 5, 1990, pp. 798–806. 

6. Tweedt, Daniel L.; and Chima, Rodrick V.: Rapid Numerical Simulation of Viscous Axisymmetric 

Flow Fields. NASA TM–107103 (AIAA–96–0449), 1995. 

7. Tweedt, Daniel L.; Chima, Rodrick V.; and Turkel, Eli: Preconditioning for Numerical Simulation of 

Low Mach Number Three-Dimensional Viscous Turbomachinery Flows. NASA TM–113120 

(ICOMP–97–11 and AIAA–97–1828), 1997. 

8. Tatsumi, S.; Martinelli, L.; and Jameson, A.: Design, Implementation, and Validation of Flux Limited 

Schemes for the Solution of the Compressible Navier-Stokes Equations. AIAA Paper 94–0647, 1994. 

9. Tatsumi, S.; Martinelli, L.; and Jameson, A.: A New High Resolution Scheme for Compressible 

Viscous Flows With Shocks. AIAA Paper 95–0466, 1995. 
NASA/CR—2010-216330 12

10. Chima, R.V.; and Liou, M.-S.: Comparison of the AUSM+ and H-CUSP Schemes for Turbomachinery 

Applications. AIAA Paper AIAA–2003–4120 (NASA/TM—2003-212457), 2003. 

11. Chima, R.V.: Swift—Multiblock Analysis Code for Turbomachinery. User's Manual and 

Documentation, Version 300, 2003. 

12. Menter, R.F.: Two-Equation Eddy-Viscosity Turbulence Models for Engineering Applications. AIAA 

J. (NASA TM–111958), vol. 32, no. 8, 1994, pp. 1598–1605. 

13. Giles, Michael B.: Nonreflecting Boundary Conditions for Euler Equation Calculations. AIAA J., vol. 

28, no. 12, 1990, pp. 2050–2058. 

14. Giles, Michael: UNSFLO: A Numerical Method for the Calculation of Unsteady Flow in 

Turbomachinery. GTL Report No. 205, 1991, pp. 45–56. 

15. Wilcox, David C.: Turbulence Modeling for CFD. Third ed., DCW Industries, Inc., La Cañada, CA, 

2006.

16. Chima, R.V.: TCGRID 3–D Grid Generator for Turbomachinery. User's Manual and Documentation, 

Version 300, 2003. 

17. Van Dyke, Milton: An Album of Fluid Motion. The Parabolic Press, Stanford, CA, 1982, pp. 60–87. 
NASA/CR—2010-216330 13
NASA/CR—2010-216330 14
NASA/CR—2010-216330 15
NASA/CR—2010-216330 16
NASA/CR—2010-216330 17
NASA/CR—2010-216330 18
NASA/CR—2010-216330 19
NASA/CR—2010-216330 20
NASA/CR—2010-216330 21
NASA/CR—2010-216330 22
NASA/CR—2010-216330 23
NASA/CR—2010-216330 24
NASA/CR—2010-216330 25
NASA/CR—2010-216330 26
NASA/CR—2010-216330 27
NASA/CR—2010-216330 28
NASA/CR—2010-216330 29
NASA/CR—2010-216330 30
NASA/CR—2010-216330 31
NASA/CR—2010-216330 32
NASA/CR—2010-216330 33
NASA/CR—2010-216330 34
NASA/CR—2010-216330 35
NASA/CR—2010-216330 36
NASA/CR—2010-216330 37
NASA/CR—2010-216330 38
NASA/CR—2010-216330 39
NASA/CR—2010-216330 40
NASA/CR—2010-216330 41
NASA/CR—2010-216330 42
NASA/CR—2010-216330 43
NASA/CR—2010-216330 44
NASA/CR—2010-216330 45
NASA/CR—2010-216330 46
NASA/CR—2010-216330 47
NASA/CR—2010-216330 48
NASA/CR—2010-216330 49
NASA/CR—2010-216330 50
NASA/CR—2010-216330 51
NASA/CR—2010-216330 52
NASA/CR—2010-216330 53
NASA/CR—2010-216330 54
NASA/CR—2010-216330 55
NASA/CR—2010-216330 56
NASA/CR—2010-216330 57
NASA/CR—2010-216330 58
NASA/CR—2010-216330 59
REPORT DOCUMENTATION PAGE Form Approved 

OMB No. 0704-0188 

The 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 Department of Defense, Washington Headquarters Services, Directorate for Information Operations and Reports (0704-0188), 1215 Jefferson Davis Highway, Suite 1204, Arlington, VA 22202-4302. 

Respondents should be aware that notwithstanding any other provision of law, no person shall be subject to any penalty for failing to comply with a collection of information if it does not display a currently valid OMB 

control number. 

PLEASE DO NOT RETURN YOUR FORM TO THE ABOVE ADDRESS. 

1. REPORT DATE (DD-MM-YYYY)

01-12-2010 

2. REPORT TYPE

Final Contractor Report 

3. DATES COVERED (From - To)

4. TITLE AND SUBTITLE

Computational Aerodynamic Simulations of a Spacecraft Cabin Ventilation Fan Design 

5a. CONTRACT NUMBER

NNC06BA07B 

5b. GRANT NUMBER

5c. PROGRAM ELEMENT NUMBER

6. AUTHOR(S)

Tweedt, Daniel, L. 

5d. PROJECT NUMBER

5e. TASK NUMBER

Task 190 

5f. WORK UNIT NUMBER

WBS 439906.04.01.02.02 

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

AP Solutions, Inc., 

5075 Everton Ave. 

Solon, Ohio 44139 

8. PERFORMING ORGANIZATION

 REPORT NUMBER

E-17264 

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

National Aeronautics and Space Administration 

Washington, DC 20546-0001 

10. SPONSORING/MONITOR'S

 ACRONYM(S)

NASA 

11. SPONSORING/MONITORING

 REPORT NUMBER

NASA/CR-2010-216330 

12. DISTRIBUTION/AVAILABILITY STATEMENT

Unclassified-Unlimited 

Subject Categories: 02 and 71 

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

This publication is available from the NASA Center for AeroSpace Information, 443-757-5802

13. SUPPLEMENTARY NOTES

14. ABSTRACT

Quieter working environments for astronauts are needed if future long-duration space exploration missions are to be safe and productive. 

Ventilation and payload cooling fans are known to be dominant sources of noise, with the International Space Station being a good case in 

point. To address this issue cost effectively, early attention to fan design, selection, and installation has been recommended, leading to an 

effort by NASA to examine the potential for small-fan noise reduction by improving fan aerodynamic design. As a preliminary part of that 

effort, the aerodynamics of a cabin ventilation fan designed by Hamilton Sundstrand has been simulated using computational fluid dynamics 

codes, and the computed solutions analyzed to quantify various aspects of the fan aerodynamics and performance. Four simulations were 

performed at the design rotational speed: two at the design flow rate and two at off-design flow rates. Following a brief discussion of the 

computational codes, various aerodynamic- and performance-related quantities derived from the computed flow fields are presented along 

with relevant flow field details. The results show that the computed fan performance is in generally good agreement with stated design 

goals. 

15. SUBJECT TERMS

Fans; Aerodynamics; Noise; Performance 

16. SECURITY CLASSIFICATION OF: 17. LIMITATION OF

 ABSTRACT

UU 

18. NUMBER

 OF 

 PAGES

65 

19a. NAME OF RESPONSIBLE PERSON

STI Help Desk (email:help@sti.nasa.gov) 

a. REPORT

U 

b. ABSTRACT

U 

c. THIS 

PAGE

U 

19b. TELEPHONE NUMBER (include area code)

443-757-5802 

Standard Form 298 (Rev. 8-98)

Prescribed by ANSI Std. Z39-18