M.M. Athavale, Y.H. Ho, and A.J. Przekwas

CFD Research Corporation, Huntsville, Alabama

Analysis of Coupled Seals, Secondary and

Powerstream Flow Fields in Aircraft

and Aerospace Turbomachines

NASA/CR—2005-212716 CFDRC 4117/1

November 2005
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
M.M. Athavale, Y.H. Ho, and A.J. Przekwas

CFD Research Corporation, Huntsville, Alabama

Analysis of Coupled Seals, Secondary and

Powerstream Flow Fields in Aircraft

and Aerospace Turbomachines

NASA/CR—2005-212716 CFDRC 4117/1

November 2005

National Aeronautics and

Space Administration

Glenn Research Center

Prepared under Contract NAS3–27392
Acknowledgments

Available from

NASA Center for Aerospace Information

7121 Standard Drive

Hanover, MD 21076

National Technical Information Service

5285 Port Royal Road

Springfield, VA 22100

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

During the course of this project, the authors had to draw on the expertise, experience and help from a number of

individuals which was essential in the successful completion of the project. Bob Hendricks and Bruce Steinetz,

NASA Glenn Research Center, provided continuous encouragement, guidance, help and patience, which were

vital for this effort. The authors have had occasion to draw on the expertise on a number of individuals from

CFD Research Corporation. Thanks are due to Ashok Singhal, President, CFDRC, for guidance and

encouragement during the course of the project. Thanks are due to S. Bayyuk, M.Z. Pindera,

N. Vaidya, H.Q. Yang, Y. Jiang, and R.K. Avva, for technical advice and discussions at various

stages of this work. Thanks are due to John Munson and Jim Forry, Allison Engine Co.,

for providing the geometries and data for the T-56 turbine calculations. Work on the

G.E. aspirating seal needed help from Mr. Shapiro, Shapiro Associates, Alan

Mcnickle, Stein Seal, and Norm Turnquist, Bharat Bagepalli, and Tom Tseng,

GE CR&D and GEAE. Finally, thanks are due to Jennifer Swann

for preparation of this manuscript as well as the

numerous publications attached in this report.
NASA/CR—2005-212716 iii

Contents 

Abstract......................................................................................................................................................... 1 

1. Introduction...................................................................................................................................... 2 

2. Flow and Heat Transfer Simulations in T-56 Turbine Drum........................................................... 3 

 2.1 Simulations on Individual Disk Cavity Pairs...................................................................... 4 

 2.2 Complete Turbine Drum Flow and Conjugate Heat Transfer Simulations....................... 10 

 2.3 Summary........................................................................................................................... 16 

3. Aspirating Face Seal Modeling...................................................................................................... 16 

 3.1 Aspirating Seal Geometry and Operation ......................................................................... 17 

 3.2 Simulations Performed ..................................................................................................... 18 

 3.3 2–D Simulations ............................................................................................................... 19 

 3.4 3–D Simulations ............................................................................................................... 20 

 3.5 Summary........................................................................................................................... 26 

4. Flow and Heat Transfer in Disk Cavities....................................................................................... 26 

 4.1 Flow in Contra-Rotating Disk Cavity............................................................................... 27 

 4.2 Simulation of Heat Transfer in Rotating Cavities............................................................. 37 

5. 3–D Secondary and Power Stream Coupling Methodology .......................................................... 41 

 5.1 Flow Codes ....................................................................................................................... 43 

 5.2 Functions of Interface Routines........................................................................................ 44 

 5.3 Issues in Formulation of Interface Methodology.............................................................. 47 

 5.4 Flow Treatment at the Interface........................................................................................ 48 

 5.5 Interface Data Interpolation Methodology........................................................................ 50 

 5.6 Summary........................................................................................................................... 53 

6. Coupled, Transient Analyses of Power Stream-Secondary Flows................................................. 53 

 6.1 Bladeless Rotor+Stator+Cavity in Turbine Section.......................................................... 53 

 6.2 UTRC High-Pressure Rig Simulations ............................................................................. 56 

 6.3 NASA Low-Speed-Air Compressor (LSAC) Rig............................................................. 64 

 6.4 Summary........................................................................................................................... 66 

7. Summary and Recommendations for Future Work ....................................................................... 68 

 7.1 Recommendations for Future Work.................................................................................. 69 

8. References...................................................................................................................................... 69 

Appendix A—Selected Publications........................................................................................................... 71 

Appendix B—An Algorithm for Interpolation Between Computational Interfaces with 

 Arbitrary Grid Matching.............................................................................................................. 141 

Appendix C—Users’ Manual for Coupled, Time-Accurate, Three-Dimensional Computations of 

 Primary-Secondary Flow Interactions at Rim Seals With SCISEAL-MS–TURBO Codes......... 151 

Analysis of Coupled Seals, Secondary and Powerstream Flow 

Fields in Aircraft and Aerospace Turbomachines

Mahesh M. Athavale, Y.H. Ho, and Andrzej J. Przekwas 

CFD Research Corporation 

Huntsville, Alabama 35805 

Abstract 

This project was established with rather broad goals of 1. application of the present-day 

computational fluid dynamics (CFD) tools to the complex flow and heat transfer phenomena in the 

secondary flow system elements in gas turbine engines, 2. application to specific OEM problems, and 

3. coupling of two computational tools to treat the complex, time-unsteady interaction of the primary and 

secondary flow streams in a gas turbine engine. 

All of the above objectives were met successfully during the course of this project. Some of the 

specific achievements from this work are: 

1. Flow and thermal analysis of the secondary flow system in an actual turbine section. The T-56 

turbine section data was provided by Allison Engine Co of Rolls Royce Aerospace Group. Flow 

and conjugate heat transfer calculations in the three inner disc-cavity pairs + associated mainpath 

were completed. Results in terms of rim seal flows at various locations, gas temperatures, 

temperatures in the rotor disks were compared with data from Allison. Other numerical 

experiments included effects of reduction of coolant flows, changes in seal clearances, and 

changes in the mainpath flow conditions on the cavity flow fields. 

2. Flow analysis of the GE/NASA aspirated face seal. This seal is being developed as a candidate 

for the GE90 balance piston replacement for an existing labyrinth seal. Flow and load 

characteristics of the seal were calculated using 2–D analyses and compared with experiments 

and other calculations during the design stages. Subsequently a test rig for the seal was built, and 

it was found to show different operational characteristics. Full 3–D CFD analysis was then 

performed on the face seal. Flow details showed interference of flow streams from the two major 

components of the seal that prevented the proper operation. A fix for this was suggested and 

implemented in the seal. After the modification, the seal performance was close to the design 

specifications. 

3. SCISEAL code was coupled with MS-TURBO, a CFD code developed at Mississippi State 

University for the treatment of the multi-stage rotor-stator and rimseal-cavity flow interaction in 

gas turbines. Both codes were appropriately modified, and an interface algorithm was developed 

to link the two codes during parallel execution. The interface treatment allows for the relative 

motion generated by the rotor stages, interpolated fluxes and flow variables from one code to 

another and ensures flux conservation across the interface. This coupled algorithm has been 

successfully used to simulate the interaction of the disc cavity and primary flow in the UTRC 

H.P. Rig. Additional simulations may be undertaken to assist the ongoing experimental efforts on 

this rig. 

In addition to these major tasks, several additional tasks were accomplished. These include validation 

of the CFD codes on the flow and heat-transfer processes in typical disc cavities, assessment of the flow 

in planar honeycomb seals and comparison with experiments, and support to NASA as well as others for 

dissemination and utilization of NASA seals code SCISEAL. 

NASA/CR—2005-212716 1
1. Introduction 

With the increasing importance on improvements of gas turbine engine performance in terms of 

efficiency and power output, all of the major subsystems of a typical gas turbine are under scrutiny. The 

secondary flow system in a turbine engine, which includes the coolant air circuits as well as the leakage 

flows in seals and the disk cavity flows is one of the areas that has shown promise of substantial gains in 

the overall engine efficiency through optimization of coolant flows and improvements in seal 

performance [1]. Impact of such changes, however, on the overall engine performance must be 

thoroughly evaluated before the changes are implemented. The secondary flow system is intimately tied 

with the other major flow stream in an engine, namely the power or mainpath flow stream. The power 

stream essentially is the flow above the blade platforms, and generates the engine power. 

The above-blade platform flows have received considerable attention in the past and present and is a 

fairly mature technology. Computational fluid dynamics (CFD) codes for multi-stage flow calculations of 

the power stream are available and are routinely used in design calculations [2]. The power-stream 

calculations and designs typically have included the effects of the secondary flow streams (coolant 

leakage in turbine section and the seal leakage in the compressor) using simplified models of the 

leakage/coolant flows entering into the power stream at the rim seal locations. 

The power-stream flow in inherently time-transient because of the relative motion between successive 

rotor and stator stages that exist in typical multi-stage compressor and turbine sections. There has been 

interest in performing such time-accurate interactions in the power stream flows during the design stages 

of a machine. Effects of this time-transient nature on the interaction of the power stream with the 

secondary stream flows therefore need to be investigated as well and is the logical next step in 

calculations of the primary and secondary flow interaction. 

In a typical multi-stage turbine section the coolant flows serve to cool the rotor disks and other 

support structures and protect these from the hot power-stream gases. The coolant flow typically is highpressure air from the compressor section, and hence it is ‘expensive’ and represents a net parasitic loss in 

terms of lost power and efficiency; at the same time, it is essential for cooling of the structural parts. For 

these reasons, optimum coolant flow rates need to be found that would provide adequate cooling 

performance at the lowest coolant flow rates to minimize the parasitic losses. Under these requirements, 

the interaction between the power stream and the secondary stream at and around the rim seals becomes 

of extreme importance. The transient nature of the power-stream flows must be taken into consideration 

when evaluating the rim seal flows. 

The main objectives of the present work were several fold: 

1. Develop a coupled, transient simulation methodology for calculations of the interaction between 

the powerstream and the secondary flow in a typical gas turbine engine turbine and compressor 

sections. 

2. Apply the coupled simulation methodology to typical multi-stage turbine and compressor 

problems. Validate the codes against available experimental data; 

3. Apply the 3–D CFD code SCISEAL to different secondary flow and/or seal turbomachinery seal 

problems. To provide relevance to the simulation results, the problem definitions were obtained 

from different gas turbine manufacturers, namely Rolls Royce Allison Engine Co. and GE 

CR&D. Results of the simulations for GE were found to be of importance in their face seal design 

improvements. 

4. Further validate the CFD codes on cavity flow and heat-transfer problems using quality published 

experimental and numerical data. 

All of these objectives were successfully met during the course of this work. The following chapters 

in this report present the details of the work. The work done on the Allison T-56 turbine cavities and 

interaction with the mainpath is presented in Chapter 2. Chapter 3 deals with the work that was performed 

on a novel aspirated face seal design from GE. 3–D simulations of the flow in the face seal were done to 

NASA/CR—2005-212716 2
provide crucial flow insight for a successful seal design. Results of a validation study performed on disk 

cavity flow and heat transfer are presented in Chapter 4. 

Description of the methodology for coupled transient powerstream and secondary flow is presented in 

Chapter 5 where the CFD codes, interface strategy, and treatment is described. Some sample validation 

results for the interface are also presented. The coupled codes were then applied to the coupled powersecondary flow streams in the UTRC High-Pressure Turbine Stage Rig. This rig was built to provide such 

data for code validations. Details of the calculations, simulation results and some comparisons with the 

experimental data are presented in Chapter 6. A brief summary and recommendations for future work are 

outlined in Chapter 7. 

2. Flow and Heat Transfer Simulations in T-56 Turbine Drum 

The typical multi-stage turbine section in a gas turbine engine presents a very complex flow and heattransfer problem. The power stream consists of fast moving hot gas from the combustor that is expanded 

through the stator and rotor rows to generate work. The disk cavities usually have compressed air as purge 

flow introduced at one or more locations, which serve to cool the rotor disks as well as supporting 

structures for the labyrinth seals. The purpose of the purge flow is twofold: to cool the rotor disks, and 

also to prevent the powerstream gases from entering the disk cavities through the rim seals. 

The advanced CFD code, SCISEAL [3] is ideally suited to analyze these complex flow and heattransfer problems in the turbine disk cavities and associated labyrinth seals. As a demonstration/validation 

problem, the turbine section disk cavities of the T-56 gas turbine engine were considered. These engines 

are currently installed on C-130 Military transport planes. The characteristics of the engine are: pressure 

ratio of 14.1, mass flow rate 15.7 kg/s, engine speed of 14240 rpm and a power rating of 5250 h.p. at 

sea-level takeoff conditions. Geometries of the disc cavities and flow conditions were obtained from 

Allison Engine Company, Rolls Royce Aerospace Group (RRAE). A cross-section through the turbine 

section of this engine is shown in figure 2-1. The turbine section consists of four rotor stages and three 

intermediate stator vanes. There are three inter-stage disk cavity pairs (Stage 1-2, 2-3 and 3-4 cavities) 

and a single disk cavity ahead of the first rotor and aft of the fourth rotor. 

The present work was focused on the three pairs of the interstage cavities. Simulations were first 

carried out on the individual disk cavity pairs for flow and heat transfer, with particular focus on the stage 

1-2 cavity, where the flow conditions are most severe (highest pressures and temperatures with multiple 

NASA/CR—2005-212716 3
coolant injection and exhaust paths). Variations in the labyrinth seal clearances, and effects of coolant 

flow reduction on the flow field were studied. Baseline flow and heat transfer calculations on the other 

two individual pairs (Stage 2-3 and 3-4) were also performed. Flow information obtained from RRAE 

design codes was made available for comparison with present results, and included pressure and 

temperatures in the cavities as well as seal mass flow rates and total temperatures. 

One of the problems faced during the heat transfer calculations in the individual cavity simulations 

was the thermal boundary condition to be imposed on the cavity walls. Typically, the rotor disks as well 

as labyrinth seal supports conduct heat across and in this sense all the inner cavity pairs are ‘connected’ to 

each other. Due to this reason, the wall temperatures and/or heat fluxes are dependent on the flow and 

thermal conditions in the cavities, and so are not known a-priori. The only way to properly treat these wall 

conditions is to include the solid parts in the solution domain together with the flow in the cavities. This 

necessitates solution of a conjugate heat transfer problem where the energy equation in the solid parts is 

coupled with the fluid energy equation, with appropriate treatment at the solid-fluid interfaces. To 

perform this calculation properly, however, the calculation domain has to extend to cover all of the solid 

and fluid domains that are likely to participate in the conjugate heat transfer. 

The second set of calculations thus focused on the conjugate heat transfer problem in the turbine 

drum. In the present case, all of the inner cavity pairs as well as solid parts of all four rotors were included 

in the calculations. 

All of the calculations presented in this chapter assumed that there were no circumferential variations 

in the flow and heat-transfer in the cavities and power-stream flows. This allows the use of a 2–D 

axisymmetric computational domain as well as steady-state treatment of the flow. This treatment 

simplifies the problem and reduces the computational requirements, and for these reasons has been used 

widely. It generally will account for all of the important flow features in disk cavity flows in a timeaveraged sense. The flow in the power stream, however, is inherently time-dependent due to rotor blade 

motion and can generate dynamic flow conditions near the rim seal, which will affect the cavitypowerstream flow interaction. Solution methodology and results for such calculations are presented in 

later chapters of this report. 

Following subsections discuss the two sets of simulations and additional details are found in two 

publications [4,5], copies of which are attached in appendix A. 

2.1 Simulations on Individual Disk Cavity Pairs 

As outlined above, the three inner cavity pairs in the turbine section of T-56 engine were considered 

in this work, with all the appropriate coolant injection in each of the pair. Of the three pairs, the first pair 

(Stage 1-2) is relatively small in radial extent, while the second and third pairs are large in radial direction 

which provide axial thrust balancing forces for the turbine shaft. The Stage 1-2 pair was also used to 

perform some parametric studies, namely effects of change in the labyrinth seal clearance and effects of 

reduction in the coolant flow injection in the cavity. 

2.1.1 Geometry and Grids.—Geometries of the three disk cavity pairs were obtained from RRAE in 

the form of drawings. Also obtained from RRAE were the flow conditions for the power streams and the 

purge flow inlets in the different cavity sets. Multi-domain, structured grids were built on each of the 

pairs. All of the major details in the geometry were accurately reproduced in the grids, including the 

clearance gaps in the labyrinth seals. The labyrinth seals have honeycomb surfaces on the stator side, 

which can be represented by increasing the surface friction factors, but in the present case such data was 

unavailable, and hence a smooth stator surface in the labyrinths seals was assumed. A very limited 

amount of grid refinement studies were performed on these complex geometries. The final configurations 

were: 

Stage 1-2 Cavity: 34 domains, 8700 computational cells. 

Stage 2-3 Cavity: 37 domains, 45000 computational cells. 

Stage 3-4 Cavity: 44 domains, 29000 computational cells. 

NASA/CR—2005-212716 4
Figure 2-2 a, b, and c show the computational grids for the three cavity pairs. The grid sizes for the 

Stage 2-3 and 3-4 cavities are much higher than Stage 1-2 cavities due to their larger physical sizes as 

well as more complicated labyrinth seals. 

2.1.2 Flow and Boundary Conditions.—The flow in the cavities and power stream was assumed 

compressible with air as the working fluid with variable properties, with the viscosity variation governed 

by Sutherland's law. The standard k-ε model of turbulence was used to treat the turbulent flow. No slip 

walls with appropriate tangential/rotational velocities were assumed on the solid walls. For this series of 

runs, all walls were assumed to be adiabatic. The conditions at takeoff were assumed with an engine 

rotational speed of 14200 rpm.

The powerstream conditions were specified on separate domains attached at each individual rim seal 

location. Each of the powerstream block was defined with appropriate boundary conditions: an inlet 

boundary with specified mass flow, an exit boundary with a specified static pressure, stationary walls on 

the outer wall/casing and rotating or stationary walls on the rotor/stator. The powerstream flow was thus 

split in six separate streams with individual sets of boundary conditions that were held fixed with no 

connection between the successive power stream domains. The values of the boundary conditions for the 

powerstream were obtained from the RRAE design codes. 

The coolant/purge flows were specified as inlet boundaries at the appropriate locations. Appropriate 

temperature, pressure and mass flow conditions were specified at these coolant injection locations. 

Several different runs were completed on the individual pair configurations: 

1. Baseline/design condition steady state runs: where the boundary conditions and geometry of the 

cavities were at the nominal design values. The flow rates and gas temperatures at the different 

rim seal locations were calculated and compared with the data from RRAE design codes. 

2. Study of change on the labyrinth seal clearance on the flow field: Stage 1-2 cavities were used to 

perform this study, where the effects of doubling the labyrinth seal clearance was studied and 

results compared with design data. 

3. Effects of reduction in the coolant flowrates: Again the Stage 1-2 cavity pair was used at nominal 

geometry, and the coolant flow rates were successively decreased to evaluate the effects on the 

cavity flow field and the interaction between the powerstream and cavity flow. 

NASA/CR—2005-212716 5
2.1.3 Results and Discussion.—For all the baseline studies, the flow conditions were held at a 

nominal design point. The results in terms of streamlines, static pressure fields, and temperature fields are 

presented in figures 2-3 through 2-5. 

In the Stage 2-3 and 3-4 cavities, the purge flow enters in the labyrinth seal at one or more 

intermediate points and then is carried over to the cavities on either side (figures 2-3a and b). Both pairs 

have ‘upstream’ (left of the labyrinth seal) cavities that are relatively narrow in the axial direction; these 

cavities interface with a powerstream domain that has a higher pressure. The “downstream” cavities both 

have relatively “squarer” cross-sections which show stronger recirculation zones as compared to the 

recirculation zones in the upstream cavities. The design of all rim seals is such that the powerstream flow 

sees a backward facing step at each rim seal. This generates a recirculation zone at the rim seal and the 

purge flow has to work around it, typically entering the powerstream near the upstream edge of the back 

step. In all four rim seals, in the present case, the net flow direction is from the cavity to the powerstream, 

i.e., there is no ingestion of the hot powerstream gas in the cavities. The flow rates and average gas 

temperatures at each rim seal are of importance and the values from present calculations are compared 

with the values from RRAE design data in table 2-1. As seen from these results the calculated flow splits 

show a higher flow rate through the downstream rim seal while the design calculations show an opposite 

trend. The calculated rim seal temperature and the average cavity pressure values however are fairly close 

to the design data. 

TABLE 2-1.—COMPARISON BETWEEN THE DESIGN DATA AND THE PREDICTION 

FOR STAGES 2-3 AND 3-4 CAVITIES (SEE FIGURE 2-2A FOR PATH NO. NOTATION) 

Location Design Predicted 

(without conjugate heat transfer) 

 Mass (kg/s) Pressure 

(Pa)*x105

Temperature 

(k) 

Mass (kg/s) Pressure 

(Pa)*x105

Temperature 

(K) 

A 0.0567 3.309 741 0.0376 3.275 786 

B 0.0376 2.137 698 0.0540 2.068 716 

C 0.0340 1.724 705 0.0240 1.689 700 

D 0.0209 1.103 703 0.0272 1.069 666 

NASA/CR—2005-212716 6
TABLE 2-2.—COMPARISON BETWEEN THE DESIGN DATA AND THE PREDICTION FOR STAGE 1-2 

CAVITIES (SEE FIGURE 2-2A FOR PATH NO. NOTATION; LABYRINTH SEAL CLEARANCE = 0.012 IN) 

Path No. Design Prediction 

Massflow (lb/s) Temp (°F) Massflow (lb/s) Temp (°F) 

4 0.249 1058 0.308 1032 

5 0.041 1058 0.030 1029 

6 0.099 1058 0.095 1100 

The Stage 1-2 cavity is much more compact in radial direction and has multiple coolant flow injection 

points, with different coolant flow properties at each injection location. The baseline calculation shows a 

main recirculation zone in each of the cavities (figure 2-4). The coolant injection points are marked in this 

figure and effects of the coolant on the streamline pattern can be seen. As indicated in figure 2-4, the 

coolant injection points are all in the upstream cavity. Part of the coolant flow then enters the power 

stream flow through the upstream rim seal. The remaining flow goes in the downstream cavity through 

the labyrinth seal and then exits into the powerstream at the downstream rim seal. Both the rim seals have 

the backward facing step structure. The powerstream flow generates recirculation zones near the rim 

seals, and the purge flow has to exit around these zones. As before, flow rates and temperatures of the air 

at the rim seals as well as through the labyrinth seal are of interest and the calculated values are shown in 

table 2-2 (see figure 2-2a for location of measurement locations); also presented are the values from 

RRAE design data. As seen, the two sets show good correlation. The temperature contours in the cavities 

are shown in figure 2-5, and the effects of coolant injection on the upstream cavity flow are apparent. The 

gas temperatures near the rim seals also show absence of powerstream gas ingestion. 

As outlined earlier, one parametric study on Stage 1-2 cavities involved increasing the labyrinth seal 

clearance by a factor of two while maintaining all other conditions constant. During engine operation, 

rotor excursions are common, and typically the labyrinth teeth contact the stator and increase the effective 

seal clearance. The effects of such clearance changes need to be understood during the design stage and 

this parametric study was an attempt to see how sensitive the cavity flow is to changes in the labyrinth 

seal. 

NASA/CR—2005-212716 7
A simulation was performed on the Stage 1-2 cavity with the labyrinth seal clearance enlarged to 0.024 inches 

from the nominal value of approx. 0.5 mm (0.012 inches). All of the other parameters, including coolant injection 

rates were kept fixed. The calculated streamline pattern in the cavities for larger labyrinth clearance is shown in 

figure 2-6, along with the streamline pattern for the baseline case for comparison. Dramatic changes in the flow 

pattern in the upstream cavity and the upstream rim seal are seen as a result of the clearance increase. The large 

recirculation bubble in the upstream cavity is pushed down and there is clear evidence of powerstream flow 

ingestion, as indicated by the streamline pattern at the upstream rim seal. This ingested flow then mixes with the 

coolant flow injected in the upstream cavity, passes through the labyrinth seal into the downstream cavity, and 

finally exits in the powerstream at the downstream rim seal. As a result of the powerstream gas ingestion in the 

upstream cavity, the average temperatures in the cavities as well as the temperatures of the air through the rim seals 

are higher (see fig. 2-7). This is seen in table 2-3 (figure 2-2a for location of measurement locations), where the rim 

seal flow data for the Stage 1-2 cavities at the higher labyrinth seal clearance are given along with the design data 

from RRAE. The computed results show fair-good correlation with the design numbers, including the flow rate and 

gas temperature at the upstream rim seal, where a negative flow rate indicates ingestion in the cavity. 

NASA/CR—2005-212716 8
TABLE 2-3. COMPARISON BETWEEN THE DESIGN DATA AND THE PREDICTION FOR STAGE 1-2 

CAVITIES (SEE FIGURE 2-2A FOR PATH NO. NOTATION; LABYRINTH SEAL CLEARANCE = 0.024 IN) 

Path No. Design Prediction 

Massflow (lb/s) Temp (°F) Massflow (lb/s) Temp (°F) 

4 0.510 1223 0.610 1315 

5 0.038 1223 0.041 1148 

6 -0.153 1691 -0.220 1830 

The second parametric study on the Stage 1-2 cavities involved flow simulations under decreasing 

coolant flow rates. During these parametric runs, the coolant flow rates were reduced progressively for all 

of the coolant injection sites by the same percentage. Simulation runs at 100, 75, 65, and 50 percent of the 

nominal coolant flow rates were performed with fixed powerstream conditions. The temperature plots for 

these runs are shown in figures 2-8A through 2.8D. The temperature field plots reveal that there is no 

powerstream gas ingestion at 75 percent coolant flow rate. At 65 percent coolant flow, gas temperatures at 

the upstream rim seal show substantial increase, indicating possible ingestion. The overall cavity 

temperatures are still similar to 75 percent case, indicating that the ingestion, if any, is at a fairly small 

rate. The overall temperature levels in the cavities rise slightly with reduction in coolant flow rates as 

expected. At 50 percent of the design coolant flow, the upstream rim seal temperatures as well as the 

upstream cavity temperatures are substantially higher, indicating gas ingestion at large flow rates. These 

simulations indicate that the cavity designs have some margin of safety built in for the coolant flow rates. 

Clearly, if one was willing to sacrifice some or this safety margin, perhaps the coolant flow rates could be 

reduced by some percentage without affecting the disk cooling substantially. Obviously if such a 

reduction is envisaged, much more detailed 2–D and 3–D simulations and experiments need to be done to 

ensure that adequate cooling is indeed still available even after the reduction in the coolant flow rates. The 

high-pressure, coolant air is expensive and represents a loss in engine power and efficiency. Hence the 

possibility in coolant flow reductions is one of the major considerations behind engine performance 

enhancement via secondary flow stream optimization. 

NASA/CR—2005-212716 9
Another parametric study on the Stage 1-2 cavity involved calculations of the cavity flows under the 

influence of a sudden change in the powerstream conditions, such as would take place during the change 

of an engine power setting, e.g., from fast idle to take-off power and takeoff-power to cruise. Steady state 

simulations for the initial condition (e.g., fast idle) were first obtained, then the powerstream conditions 

changed/ramped to the another set (e.g., takeoff) and the effects of the change on the cavity flow were 

calculated. Details of the computation are given in [6]. The simulations showed that under both these 

power setting changes, the cavity flows remained fairly stable, and did not ingest powerstream gas, even 

when switching from fast idle (low pressures in powerstream) to takeoff (maximum temperature and 

pressure conditions in powerstream). 

2.2 Complete Turbine Drum Flow and Conjugate Heat Transfer Simulations 

As remarked in the previous section, the walls of the rotors and stators were assumed to be adiabatic 

in the earlier calculation. Clearly this is not a correct boundary condition, and in the absence of 

temperature/heat flux profile data, can lead to thermal field solutions that may contain discrepancies. In 

order to estimate such differences, the entire turbine drum was considered in the next set of calculations. 

All of the solid parts under the blade platform, including all four rotor disks and the supports of the 

honeycomb stators were included in the solution domain. The computational model of the entire turbine 

drum is shown in figure 2-9, where the fluid and solid parts are marked, as well as the flow and thermal 

boundary conditions. As seen in this figure, the computational domain, which contains fluid as well as 

solid parts, is very complex. A multi-domain grid with 140 domains and 91K cells was built for these 

NASA/CR—2005-212716 10
simulations. A small-scale grid independence study showed that changes in the grid sizes showed small 

effects on the flow solutions. 

Working fluid for this calculation was also taken as air with variable properties. The six powerstream 

domains with the associated inlet and exit boundary conditions as well as all the cavity purge flow 

locations and the flow rates were also kept the same as for the individual cavity pair calculations. The 

main difference here was the use of implicit, conjugate heat transfer conditions at all of the walls that 

were in contact with the working fluid in the disk cavities. Isothermal conditions were imposed at the 

blade platform walls that are in contact with the powerstream, with temperature values that corresponded 

to the local powerstream fluid temperatures. Boundary conditions at the bases of the rotor disks as well as 

the outer walls of rotor 1 and rotor 4, and the walls of the labyrinth teeth also were boundaries where 

external thermal conditions were needed. In the present calculations, these walls were assumed 

isothermal, with the wall temperatures set at the coolant temperature. The reasoning for this was that these 

solid parts are in contact with the coolant flow, and hence at or near the coolant temperature. The standard 

k-ε model was used to treat turbulence. 

The results of the simulations are shown in terms of field plots of streamlines, temperatures and 

pressures in the computational domain. Figures 2-10 through 2-12 show these plots for the entire drum. 

The radial extents of Stage 1-2 cavity-pair are much different from the other two pairs, and plots of Stage 

1-2 pair are shown separately in subsequent plots for clarity. 

Results for the Stage 1-2 cavity pair are shown in figure 2-13a (streamlines) and 2-13b (temperature). 

The basic streamline/flow pattern is very similar to that shown in figure 2-4. An egress of cavity fluid in 

the powerstream is seen at both rim seals (path No. 4 and 6). The temperature plot in figure 2-13a also 

shows the distribution in the solid parts of the computational domain (seal support, rotor disk). Compared 

to figure 2-5, the cavity temperatures are generally higher. The temperatures in the rotor disk and the 

labyrinth seal supports show highest temperatures near the upper side where the solids are in contact with 

the powerstream gases. The temperatures then decrease as one moves towards lower radii, indicating that 

there is conductive transfer of heat in the solid parts from the hot powerstream gases to the cavity flow. 

NASA/CR—2005-212716 11
NASA/CR—2005-212716 12
This heat transfer represents additional heat load on the coolant flow supplied in the cavity, and this is 

reflected in an increase in the cavity flow temperature levels. 

Corresponding streamline and temperature plots for the Stage 2-3 and 3-4 cavities are shown in 

figure 2-14a and 2-14b. Again, the cavity streamline pattern is similar to the pattern obtained with isolated 

cavity calculations (see figs. 2-3a and 2-3b), with an elongated, weak recirculation zone in the upstream 

cavity in each pair, and a strong zone in the downstream cavity. Flow patterns at all rim seals (Paths 

marked A – D in figure 2-9) show cavity fluid egress into the powerstream flow. Temperature contour 

plots show strong temperature gradients in the rotor disks, with highest temperatures near the blade 

platforms, and decreasing towards smaller radii. This temperature gradient generates additional thermal 

load on the coolant flows with a consequent increase in cavity flow temperature, similar to the Stage 1-2 

cavity flow. 

The additional thermal loads imposed on the cavity flow by the conduction in the rotor disks and 

labyrinth seal supports can be assessed by considering the gas temperatures at the rim seals. These results 

are shown in tables 2-4 and 2-5, together with the RRAE design numbers. Also shown in the tables are 

the results of the earlier calculations, where the conduction in solids was not considered. As seen from 

these tables, the calculated mass flux rates through the various rim seals show minimal changes as a result 

of the inclusion of the conjugate heat transfer in the solid parts. The gas temperatures through the rim 

seals, however, show an increase from the earlier solutions which varies from 4 K to 70 K for the 

Stage 2-3 and 3-4 cavity pairs and the increase is about 30 K at the upstream rim seal, path 6, in the 

Stage 1-2 cavity pair. This increase represents the thermal load placed on the cavity flow by conduction in 

the solid parts. The temperatures are generally higher than the RRAE design numbers, where the heat 

transfer through the solid parts was not included. The temperature increases in the rim seal gas flows are 

fairly substantial and indicate that the conjugate heat transfer problem with conduction in the solid parts 

has to be considered when performing these calculations. The usual way of calculations with adiabatic 

walls will generate gas temperatures that will be cooler than actual, and thus overpredict the cooling 

performance. This can lead to inadequate cooling performance in an actual engine, especially as the 

coolant flow rates get optimized. 

NASA/CR—2005-212716 13
NASA/CR—2005-212716 14
NASA/CR—2005-212716 15
TABLE 2-4.—COMPARISON BETWEEN THE DESIGN DATA AND THE PREDICTION 

FOR STAGE 1-2 CAVITIES (SEE FIGURE 2-2A FOR PATH NO. NOTATION) 

Design Prediction 

(include conjugate heat 

transfer for solid parts) 

Prediction 

(without conjugate heat 

transfer) 

Path No. 

Massflow 

(kg/s) 

Temperature 

(K) 

Massflow 

(kg/s) 

Temperature 

(K) 

Massflow 

(kg/s) 

Temperature 

(K) 

4 0.1129 843 0.1284 870 0.1397 829 

5 0.0186 843 0.0249 984 0.0136 827 

6 0.0449 843 0.0481 893 0.0431 866 

TABLE 2-5.—COMPARISON BETWEEN THE DESIGN DATA AND THE PREDICTION FOR 

STAGES 2-3 AND 3-4 CAVITIES (SEE FIGURE 2-2A FOR LOCATIONS NOTATION) 

Design Prediction 

(include conjugate heat 

transfer for all solid parts) 

Prediction 

(without conjugate heat 

transfer) 

Location 

Mass 

(kg/s) 

Pressure 

(Pa)*x105

Temp. 

(K) 

Mass 

(kg/s) 

Pressure 

(Pa)*x105

Temp. 

(K) 

Mass 

(kg/s) 

Pressure 

(Pa)*x105

Temp. 

(K) 

A 0.0567 3.309 741 0.0390 3.282 790 0.0376 3.275 786 

B 0.0376 2.137 698 0.0522 2.089 794 0.0540 2.068 716 

C 0.0340 1.724 705 0.0249 1.6823 769 0.0240 1.689 700 

D 0.0309 1.103 703 0.0263 1.082 732 0.0272 1.069 666 

*Values at the center of the cavities 

2.3 Summary 

To summarize this chapter, the flow and heat transfer processes in the turbine section of the RRAE 

T-56 engine were simulated. Three pairs of inner disk cavities in the turbine section were first 

individually considered at the design operating point and simulations showed flow egress into the 

powerstream at all rim seals. The rim seal temperatures correlate well with RRAE design data. Stage 2-3 

and 3-4 flow splits in the two cavities, however, showed discrepancies from the design data, which may 

have been due to coolant flow injection location mismatch and/or grid refinements. Stage 1-2 cavity flows 

showed good agreement with design data. Dramatic effects on the Stage 1-2 cavity were seen with 

increase in the labyrinth seal clearance, and demonstrated the sensitivity of the cavity flows to this 

parameter. Simulations on Stage 1-2 cavity pair with varying coolant flow rates also indicated that 

powerstream gas ingestion did not occur till the coolant flows were reduced to 50 percent of the design 

values. Such information will be of significant use when designing the cavities with optimized coolant 

flow rates. 

The complete turbine drum calculation including heat-transfer in solid parts indicated that heat 

conduction in the solids provided another path for the hot powerstream gas to transfer thermal energy to 

the cavity flows. This thermal load resulted in increase in the overall temperature levels in all inner 

cavities. These effects can be substantial and need to be included when assessing the effectiveness of the 

coolant in the disk cavity flows. Additional studies are needed to further explore some of the differences 

found in the calculated results and RRAE design data. 

3. Aspirating Face Seal Modeling 

An enhanced aspirating face seal is being evaluated by GE Aero Engine Co. (GEAE), GE Corporate 

Research and Development Center (GE CR&D)[7-9] and NASA Glenn Research Center. The seal is 

being considered as a replacement for labyrinth seals in aircraft engines for reduced leakage and 

improved engine efficiency. This chapter deals with the simulation work that was performed during the 

design stages of this seal as well as the full scale testing in a test rig during which a performance problem 

NASA/CR—2005-212716 16
design stages of this seal as well as the full scale testing in a test rig during which a performance problem 

was discovered. Using 3–D simulations of the face seal flow, the reason for the performance problem was 

identified and a fix suggested. This fix was tried out successfully in the test rig and the seal performance 

with the fix was found to be very close to the original design specifications. Following sections describe 

the seal configuration, the simulation work that was performed during the initial design stages as well as 

during the rig-testing phase. 

3.1 Aspirating Seal Geometry and Operation 

The aspirating face seal is being considered as a replacement for the conventional labyrinth seal, 

especially at larger diameters. The labyrinth seal typically has larger clearances with increasing diameters, 

with consequent increased leakage, and hence the aspirating face seal design is expected to be very 

attractive in large diameter seals. The seal is non-contacting type, with a typical working clearance of 

0.0015 to 0.003 inches. Unlike the conventional face seals, the aspirated face seal design has a clearance 

that is dynamically adjusted depending on the seal operating conditions. The seal relies on a 

hydrodynamic air-bearing to provide a stiff air film that generates the film loads to maintain the working 

clearances to prevent rubbing and thus provide long operational life. 

A schematic of the seal is shown in figure 3-1 (also table 3-1). The high-pressure air is located on the 

seal inner diameter and the low-pressure air is on the outer diameter side. The L-shaped component is the 

primary seal. A secondary piston ring is provided on the primary seal to allow the primary seal to 

translate axially in response to air pressure changes and rotor motion. A garter spring and a set of axial 

compression springs keep the piston ring seal in its housing and provide sealing force. 

The primary seal is mounted on the seal housing on rotation locks. A number of retraction springs 

located at the outer circumference of the primary seal provide the force needed to retract the seal away 

from the rotor when there is no air pressurization. The primary seal has two load bearing surfaces that 

face the smooth surfaced rotor: a primary seal dam and the hydrostatic bearing, which are separated by a 

circumferential vent slot. The air bearing has a number bearing feed holes located circumferentially, 

which are connected to the high-pressure side and deliver high-pressure air to the bearing to create a loadbearing film. 

The leakage air going radially outward from the dam and inward from the bearing is collected in a 

vent slot/trench and vented to the low-pressure region through several axial and radial slots, also placed at 

several circumferential locations. A labyrinth tooth (called as aspirating tooth) controls the flow rate 

through the seal dam when the seal is in open position. At equilibrium, the various forces that act on the 

seal are shown in figure 3-2. Forces F1 and F2 are generated in the hydrostatic bearing and the dam 

respectively and the two forces act to open the seal. The high-pressure air at Phigh generates a force Fb on 

the seal that tries to close the seal gap. The retraction spring force, Fs, acts to open the seal as well. The 

sliding friction at the secondary piston seal provides a frictional force that opposes any axial motion of the 

primary seal. 

TABLE 3-1.—ASPIRATING FACE SEAL COMPONENTS 

1 Primary face seal ring 

2 Secondary piston ring 

3 Radial garter spring 

4 Axial compression springs 

5 Seal housing 

6 Primary seal dam 

7 Vent groove 

8 Hydrostatic gas bearing surface 

9 Vent slots 

10 Aspirator tooth 

11 Retraction coil springs 

12 Flow deflector (enhanced seal only) 

NASA/CR—2005-212716 17
 

In the ’open’ position, the air pressures are same on the high pressure and low pressure side, and the 

retraction spring force Fs (see figure 3-2) keeps the primary seal away from the rotor surface at maximum 

clearance. Once the seal is pressurized, i.e., Phigh > Plow, the flow through the labyrinth tooth creates a 

lower pressure in the lower cavity and a closing force, Fc, is generated due to Phigh acting on the seal outer 

surfaces. When the seal closely approaches the rotor, pressure drop now is across the seal dam rather than 

the aspirating tooth. The hydrostatic bearing, also fed with the high-pressure air, starts providing an 

opening force that opposes the closing force Fc. The bearing opening force increases rapidly as the seal 

clearance reduces, and thus the air bearing provides a very stiff air film that provides sufficient balancing 

force to counteract Fc and Fs and maintain the seal in equilibrium at a design clearance of 0.0015 to 

0.003 inches. Any changes in the film thickness are discouraged because of the restoring changes in the 

bearing servo forces that restore the force equilibrium. The seal will track changes in Phigh as well as any 

changes in the rotor position by sliding on the piston ring till the equilibrium position is achieved. The 

seal can be operated at very tight clearances over the entire range of operating conditions and maintains 

low leakage rates. 

3.2 Simulations Performed 

The simulations that were performed on this seal were at two different levels during the seal design 

and testing program. The first series of simulations were performed during the design stages. 2–D 

axisymmetric simulations on the overall seal geometry were performed to corroborate the film stiffness 

and load calculations performed with simpler design codes. These calculations covered a large range of 

clearance and seal pressurization values. Another of the aim of this study was to assess the seal loads at 

relatively larger clearances (> 0.01 inches), which are outside the valid range for the design codes. Results 

for two different aspirated face seals were considered: one was a test seal with a smaller diameter, built to 

test the validity of the concept. The second seal was the full-size seal that was to be used in the test rig. 

The second set of simulations was performed during the testing phase of the full sized rig. This set 

involved full 3–D simulations of the full-sized seal as well as the smaller test seal. These simulations were 

performed to analyze the flow field in the seal and to explain anomalous behavior that was observed 

during the testing of the full-size seal. Details of the two sets of results follow: 

NASA/CR—2005-212716 18
3.3 2–D Simulations 

These simulations were performed using a 2–D axisymmetric seal configuration. The actual seal has a 

finite number of radial and axial slots as well as bearing holes that feed high-pressure air to the 

hydrostatic bearing. For the 2–D results these were converted to channels and the channel widths were 

adjusted to maintain the flow areas in the 2–D configuration. An 8 domain 2–D grid with 16000 

computational cells was built for these simulations and is shown in figure 3-3 along with the boundary 

conditions. 

The working fluid was air and was treated as compressible and with variable properties. The flow in 

parts of the seal is turbulent and in parts it is near-laminar (e.g., hydrostatic bearings at small clearances). 

The low-Re k-ε model was used in this case to treat the turbulence, because this model can handle 

laminarization of flow in the bearing. Total pressure and temperature conditions were specified at the 

aspirating tooth inlet as well as the inlet to the bearing feed holes. Exit pressure conditions were specified 

at the radial and axial slot exits as well as at the outer boundary of the bearing. 

A representative streamline and pressure plots for the seal flow are shown in figures 3-4 and 3-5. The 

streamlines show the fluid movement through the seal. The flow from the aspirating tooth enters the dam, 

accelerates and is dumped into the circumferential vent slot and eventually exits through the axial and 

radial slots. Nearly half of the bearing flow, fed from the high-pressure air through the bearing feed holes, 

exits radially outwards. The remaining flow enters the circumferential vent slot, mixes with the flow from 

the dam and exits through the axial slot. 

The seal total leakage and the bearing and dam loads are several different clearance and pressure 

conditions were calculated, and compared with the design code calculations. In general, the comparison 

with the design code results was good at small clearances (below 0.004 inches). At large clearances the 

design code results become somewhat inaccurate. The seal showed very high film stiffness at small 

clearances. As designed, the pressurized air bearing provided a large fraction of the seal restoring force at 

 

NASA/CR—2005-212716 19
 

these small clearances. At larger clearances, the bearing film stiffness dropped rather sharply with much 

smaller load capacity generated by the bearing. This exercise proved that the scientific code SCISEAL 

could be successfully applied to complex seal geometries without any special treatment and produce 

reasonable results. 

3.4 3–D Simulations 

3–D simulations on the seal were performed during the testing phase of a full-scale model. It was 

observed during testing that the test seal showed a very stable, repeatable operating clearance of 

0.016 inches (at a seal pressurization of 7 psid) as against 0.0015 inches, the design value. In the absence 

of any empirical or analytical data from the design codes that explained this behavior, the only possible 

solution was to simulate the flow in the seal in full configuration using 3–D CFD codes, and then to 

identify the possible causes for the observed behavior. Earlier results on this seal with the SCISEAL code 

had provided sufficient confidence in the code capabilities, and SCISEAL was again used to simulate the 

full 3–D seal flow at the observed test rig condition in order to analyze the flow. 

3.4.1 Geometry and Flow Conditions.—In order to reproduce the actual flow phenomena as 

accurately as possible, the actual test seal dimensions were used (as against the design geometry) to build 

a 21 domain structured grid on the aspirating face seal. The test seal geometry has a large number of 

radial and axial vent slots that connect to the vent trench, and a representative PI sector of the seal was 

used to perform the simulations. In the present case, a PI angle of 2.5 degrees was used which included 

one set of axial and radial vent slots and one bearing feed hole. All other features in the seal are 

axisymmetric (aspirating tooth, vent trench, rotor, labyrinth cavity). A wire frame model of the 

computational domain is shown in figure 3-6; also shown in this figure are the flow boundary conditions. 

A solids model of the seal with all of the working surfaces is shown in figure 3-7. 

NASA/CR—2005-212716 20
Steady-state simulations were performed at a number of different seal clearance values and 

pressurizations that were either tried out in the seal rig or were planned for testing. The rotor was kept 

stationary for both the experiments and simulations. One possible way to simulate the seal is to fix the 

seal pressure and let the seal clearance change using a force balance model. The other approach was to fix 

the seal clearance and pressurization at different values and calculate the seal balancing forces to assess 

the tendency of the seal at that point (closing, opening or in equilibrium). The second approach was used 

in the present calculations. Similar to the 2–D runs, air was use as the compressible working fluid with 

variable properties. The standard k-ε model, however, was used for turbulence to keep the grid sizes small 

and economical. All of the walls were assumed adiabatic for these runs. 

3.4.2 Simulation Results.—The first simulation run was performed for a seal gap of 0.016 inches and 

an inlet pressure of 7.1 psid, which was the experimentally observed stable seal configuration. The 

reaction force values F1 and F2, on the dam and the bearing portions of the seal were evaluated by 

integrating the computed pressure forces on the respective surfaces. The seal opening forces (F1+F2+Fs) 

were then compared with the seal closing force Fc. The computed values of F1 and F2 showed that the seal 

closing and opening forces were balanced well at the 0.0016 inch setting. This was the exactly the 

behavior seen in the experiments. The calculated seal leakage rate of 0.98 lb/s also compared well with 

the experimental value of 1.01 lb/s. This case thus provided a measure of validation and confidence in the 

computational model. Additional runs then were taken at different clearance values, above and below the 

stable 0.0016 inch gap. At higher seal gaps, the bearing force (opening) was found to be too small to 

counteract the closing force Fc and seal showed a tendency to close. At smaller clearances, the seal 

opening forces F1+F2 were found to be higher than the seal closing force, and hence the seal had a 

tendency to open. This corroborates very well the experimental observations that the seal had a very 

stable operating point at 0.016 inches gap, and would return to this position when perturbed to higher as 

well as lower seal gaps. 

Flow-field details at the stable configuration are shown in figures 3-8 through 3-11. Velocity vectors 

in the r-X plane containing the centerline of the bearing feed hole are shown in figure 3-8. Distinct flow 

NASA/CR—2005-212716 21
threads are clearly seen in the plot. High-pressure air enters the aspirating tooth cavity and then the dam, 

while the feed holes also supply the high-pressure air to the bearing. The flow exiting the dam into the 

circumferential vent slot/trench has a high velocity, and this air enters into the lower exit of the bearing 

instead of going out to the low-pressure region through the axial and radial slots. The air coming into the 

bearing from the feed hole is also swept up by the flow from the dam. A similar r-z section, but midway 

between the bearing feed holes (figure 3-9) shows that the fast flow from the dam enters the lower bearing 

exit, and continues uninterrupted till it goes out the outer exit of the bearing. A view of the velocities in 

the r-θ plane, placed near the seal surface is shown in figure 3-10 and shows the flow from the dam 

entering the bearing, and interfering with the flow from the bearing feed hole. The characteristic pattern 

of the interaction between the bearing feed flow and dam flow was also confirmed by oil trace patterns 

observed on the rotor surface during seal testing. (Personal communication from Mr. Turnquist, GE 

CR&D) 

A pressure plot in the seal gap is shown in figure 3-11 and indicates that the overall pressure level in 

the bearing is higher than the exit pressure (lower seal pressure), as a result of the dam flow coming into 

the bearing. This bearing pressurization from the dam flow generated sufficient pressure load in the 

bearing seal to equilibrate at a gap of 0.016 inches rather than the design value of 0.0015 to 0.002 inches. 

During the seal design stages, all of the design calculations were performed under two assumptions: 

(1) The flow from the bearing and the seal dam do not interfere with each other, and these two elements 

essentially operate independently, and (2) The seal calculations were done at a given clearance, without 

consideration to the process of bringing the seal to this gap from a ‘wide open’ initial seal gap. It is the 

interaction between the dam flow and the bearing at relatively larger clearances that was found to be the 

cause of the anomalous seal behavior. 

NASA/CR—2005-212716 22
NASA/CR—2005-212716 23

Figure 3–10.—Velocity vectors in a r- plane near the rotor wall.

Jet from the

axial hole

Nearly undisturbed

flow from the dam

Flow in

the dam

This pattern

is seen in

oil streaks

Bottom edge

of the bearing

Velocity vectors near the rotor wall,

16 mil clearance
To test the interference hypothesis, ways to prevent the dam flow from entering the bearing were 

considered. The simplest was to consider a small ledge wall on the rotor surface located such that it 

protruded in the circumferential vent slot/trench, at the radial midpoint of the trench. Since the ledge was 

only to act as a flow diverter, the axial extent of the ledge/protrusion was not thought to be critical, and a 

small axial width (3 mm) was assumed. A solids model showing the placement and extent of the ledge in 

the seal model in shown in figure 3-12. Simulations were then performed for a seal clearance of 

0.016 inches. This ledge/flow diverter was found to be very effective in diverting the dam flow away 

from the bearing. This is clearly seen from the velocity plots in figures 3-13, 3-14 and 3-15. The cutting 

planes for these plots are the same as used in figures 3-8 through 3-10 respectively. The dam flow is seen 

to make a near 90 degree turn at the ledge (figure 3-13, 3-14) and exit via the axial slot to the seal low 

pressure region. As a consequence of the flow diversion, the static pressure at the inner radius of the 

bearing is much lower than before, and the flow from the bearing feed hole now exits both at the inner 

and outer radii. This is clearly seen in figure 3-15, where the flow velocities at the feed hole are 

symmetric (compare with figure 3-10). The pressure plot in the seal gap, figure 3-16, shows dramatic 

changes in bearing static pressures which are now much closer to the vent pressure. This reduction in the 

computed bearing pressure levels results in a much smaller bearing film force F2, and eventually produces 

a force balance on the seal that closes the seal gap at this setting. 

Subsequent to this analysis the test seal was modified to build a small ledge on the rotor and was 

tested for stationary and spinning rotor and the initial closing performance of the seal now followed the 

design predictions exactly. This test seal has also been tested at different speeds and pressurization levels 

and stable, predictable performance has been obtained from the seal over the entire operating envelope. 

For details, see [8,9] also included in appendix B. 

 

NASA/CR—2005-212716 24
 

NASA/CR—2005-212716 25
3.5 Summary 

The complex flow field in an aspirated face seal was computed both in 2–D and 3–D configurations. 

The 2–D simulations matched well with the design calculations. However, the 3–D simulations proved of 

significance in analyzing a test seal that showed considerable deviations in behavior from the designed 

values. 3–D flow analyses showed the interference of flows in two different components of the seal at 

large gaps, and pointed to a possible fix. The design codes could not consider these interactions at larger 

clearances and hence could not predict the anomalous behavior. 

This example illustrates the utility of the full 3–D CFD calculations with SCISEAL on this complex 

problem. The details of the flow field and pressures were reproduced accurately by the code, and provided 

first the cause of the anomalous behavior, and then suggested a fix which could be tried out in 

computations to assess its effectiveness. Although the 3–D calculations take much longer to perform than 

the design calculations with simpler codes, the design codes often can not account for all of the flow 

phenomena that may take place in a seal. As new and more complex shaped seals are designed and tested, 

the 3–D CFD calculations definitely have a place in the design procedures. These calculations can provide 

details of the flow fields as well as seal component performance, point out problem areas and reasons, and 

aid in the design process to ensure a successful design. 

4. Flow and Heat Transfer in Disk Cavities 

Rotating cavities with or without throughflow occur in a number of different places in a typical 

engine. A number of different configurations are possible depending on the location of the cavity. 

Cavities near the rim seal typically have a combination of a rotating and stationary walls, while the 

cavities nearer the centerline can have all rotating walls. In the turbine section, the cavity throughflow is 

typically the coolant air that purges the cavity and cools the rotor disk temperatures. To effectively 

estimate the cooling performance in the disk cavities one needs to assess the accuracy of the numerical 

codes that are being used. This chapter deals with two studies of flow and flow+heat transfer in typical 

disk cavities found in the turbine sections. Experimental data was available for the two studies, and the 

NASA/CR—2005-212716 26
SCISEAL code was used to simulate the flow problems at different operating conditions and the 

numerical results compared with the experiments to assess the accuracy of the predictions. 

Of the different turbulence models that are available in SCISEAL, the standard k-ε model and the 

low-Re k-ε models are two models that are widely used. Part of the efforts in this task were devoted to 

assess the results from these two models on the same flow problems, in order to evaluate the accuracy of 

the predictions and to assess the efficacy of using these models to handle the typical disk-cavity problems 

encountered in gas turbines. 

Of the two sets of calculations considered here, one dealt with the flow in a cavity formed by two 

contra-rotating walls and the experimental details and data are presented by Kilic et al,[10] and Gan et al 

[11]. The cavity flows were run at different relative disk speeds and throughflow rates. This type of 

cavities are encountered in turbines with contra-rotating shafts. 

The second set of calculations included flow and heat transfer in a cavity with co-rotating walls, with 

a coolant throughflow. The experimental details and data are given by Northrop et al [12]. Heat transfer 

characteristics on the cavity walls were compared with experimental data. 

Details of the calculations and computations are given in the following sections. 

4.1 Flow in Contra-Rotating Disk Cavity

This Section summarizes the flow simulations performed in a cavity formed by a pair of rotating 

disks. A schematic of this configuration is shown in figure 4-1. 

As shown in the figure, the cavity is formed of two disks with outer radii R of 391 mm. Each of the 

disks carries a shroud along the outer periphery which rotates with the disk. A gap of width sc exists 

between the two shrouds which allows radial egress of air as shown. When a ‘purge’ air flow is used, it is 

introduced through a central hole of radius a in the left disk, and then passes up radially through the two 

‘gauze’ tubes shown which are attached to the two disks and rotate with them. The tubes even out the 

variation in the radial velocity as the flow enters the cavity, but only partially, especially at higher purge 

flow rates. The overall geometry is described in terms of three aspect ratios whose values are: the gap 

ratio G = s/R = 0.12, the clearance ration Gc = sc/R = 0.016 and the inner-to-outer radius ratio a/R = 0.128. 

NASA/CR—2005-212716 27
Two series of experiments were reported in Kilick et al.[10] and Gan et al..[11]. In one case the disk 

speeds were varied with no purge flow, and in the second series, the disk speeds were fixed, and purge 

flow rates were varied. In both cases, velocity measurements were taken at different radial locations, and 

the radial and tangential velocities were measured across the gap in the disks along the X direction. The 

two velocity components were normalized with the local wall swirl velocity Wl = Ωl r and plotted as a 

function of the axial distance normalized with the cavity gap Xmax. Details of the two computational series 

are described below. 

4.1.1 No Purge Flow, Varying Disk Speeds.—In the first series, the left disk was rotated at a constant 

angular speed at a nominal Reθ = 1.25e6. The right side disk was rotated in the opposite direction at 

varying speeds, to get different angular speed ratio (Γ = Ωr/Ωl) values from 0 to –1.0. No purge flow was 

used in this series. Simulations were carried out for five Γ values of 0.0, –0.4, –0.6, –0.8 and –1.0. Of 

these, shown in this note are results for Γ = 0.0, –0.4 and –0.8. 

A 2–D axisymmetric grid with 67 cells in the axial direction and 110 cells in the radial direction was 

generated for this series. The flow domain covered the entire cavity from r = 0 to r = R. The shroud gap 

was blocked with a linear imposed tangential velocity to account for the variation from one shroud to the 

other. The flow was taken as constant property and incompressible, with no-slip walls on disk and shroud 

surfaces with the appropriate angular speeds. The low-Re k-ε model was used for turbulence treatment 

and the grid spacing near the walls was close enough to get nondimensional wall distances y + < 0.3 in 

most cases. 

As mentioned above, the experimental results were in the form of plots of normalized velocity 

components Vs. axial distance, plotted at normalized radial distances of r/R = 0.6, 0.7, 0.8 and 0.85 and 

at Γ = 0.0, –0.4 and –0.8. These are shown in figures 4-2 through 4-4. Also shown in the plots are the 

experimental data for comparison. In general the comparison between the numerical and experimental 

data is good to very good, and the changes in the flow due to the varying right-disk-rotation are picked up 

correctly. A description of the flow structure changes (in terms of the streamlines) with the right-hand 

disk speed is given in [10] and the streamline patterns calculated in the present simulations match well 

with the computations reported in [10]. 

4.1.2 Constant Disk Speeds, Varying Purge Flow Rates.—The disk rotation speeds ratio was fixed at 

Γ = –1.0, and the radial throughflow rate was varied (see Gan et al.. [11]). The purge flow rate was 

specified in terms of a flow coefficient Cw, defined as Cw = Q/Rν where Q was the volume flow rate and 

ν the kinematic viscosity. Four flow coefficient values were analyzed: Cw = 0.0, 2320, 6310 and 9280. 

For the zero purge case (Case 1), the grid used was similar to that used in previous Section. For the 

nonzero purge flow cases, the computational domain was changed from Case 1 by moving up the lower 

boundary to coincide with the gauze tubes. A uniform radial velocity was imposed at the inlet boundary to 

generate the purge flow, and a tangential velocity corresponding to the surface speed of the gauze tube 

was also imposed. 

The nonzero purge flow cases were simulated using both the low-Re turbulence model as well as the 

standard k-ε model to assess the differences in the solutions obtained with these models. The grids used in 

the low-Re case had 67 and 95 cells in the axial and radial directions respectively, and yielded a 

nondimensional wall distance y+

 of < 0.3 at all cells near the walls. For the standard k-ε model, the grid 

size was reduced to 47 and 88 cells in the axial and radial directions, to ensure that the first cell away 

from the wall stayed in the proper y+

 range (y+ > 11.5 for the first cell) for the wall functions. 

As in the previous series, the tangential and radial velocities were measured in the experiments at 

several radial locations across the cavity gap. Plots of the calculated normalized velocities (with the lowRe k-ε turbulence model) as a function of the axial distance at different radial heights are shown in figures 

4-5 through 4-8. Also shown are the experimental data for comparison. As in the previous Section, the 

agreement between the two data sets is good to very good. Computations presented in 

Gan et al. [11] also show similar agreement with the experimental data, albeit their treatment of the inlet 

boundary condition for the nonzero purge flow cases is somewhat arbitrary. Under the conditions 

described, the inflow condition used in the present study appears to be more reasonable. In actuality, the 

NASA/CR—2005-212716 28
NASA/CR—2005-212716 29
NASA/CR—2005-212716 30
NASA/CR—2005-212716 31
NASA/CR—2005-212716 32
NASA/CR—2005-212716 33
NASA/CR—2005-212716 34
NASA/CR—2005-212716 35
axially entering flow impinges on the right side disk, and then moves along the radial direction, and this 

creates a stronger radial flow near the right side, especially for smaller radii as seen in figures 4-8a and 

4-8b. As expected, the discrepancy is larger at lower radii and higher purge flows, but towards the shroud 

regions, the flow tends to even out. 

These runs were also repeated with the standard k-ε model and the results compared with 

experimental data as well as the low-Re k-ε model results. As an example, the velocity profiles for 

Cw = 6320 at various radial stations for the two turbulence models and experimental data are shown in 

figure 4-9. As seen in these plots, the results from the standard and low-Re k-ε (Chien, 1982, [21]) models 

are very close to each other, and agree well with the experimental data. Similar agreement between the 

two turbulence models was seen at all other purge flow rates. 

Finally, the changes in the flow structure with increasing purge flow rates is illustrated in 

figure 4-10 where the streamlines of the flow at Cw=2310 and 6320 are plotted. As described in Gan et al. 

[11], the flow structure consists of a source region exists near the inlet where the radial velocity is 

positive, boundary layers on the rotating walls with radially outward flow and a pair of contrarotating 

vortices from the boundary layers to the central midplane. The flow at the axial midplane is radially 

inwards due to the counterrotating vortices. At the lower purge flow rates, a secondary contrarotating pair 

of vortices near the inlet plane is seen, and this is a results of the lower purge velocities. At higher purge 

flow rates the inlet radial momentum is sufficiently large to eliminate the secondary vortex pair. 

NASA/CR—2005-212716 36
4.2 Simulation of Heat-Transfer in Rotating Cavities 

This series of runs involved the flow and heat-transfer calculations in a cavity with co-rotating walls 

at fixed, equal wall rotational speeds. The flow configuration is shown in figure 4-11. Experiments were 

carried out and reported by Northrop and Owen [12]. The flow domain consists of two rotating disks 

0.428 m in diameter with a separation of 0.059 m. The disks are joined at the top with an insulated rim 

that has several holes along the centerline on the periphery that act as the flow exit passage. Cooling air 

flow was introduced through a central hole in one of the disks (called as upstream disk) and exits through 

the holes in the rim. Both the disks were heated using electric heaters, and the disks have thermocouples 

and flux meters for temperature and heat flux measurements. The experiments involved heating the disks 

to get different radial distributions of wall temperatures and to measure the local Nusselt numbers at 

different flow and disk rotation conditions. 

The simulations assumed the flow to be 2–D axisymmetric, and incompressible. The flow was 

assumed to enter radially at inner radius r/R = 0.1, and a uniform radial velocity was assumed. For the 

present range of temperature variations, constant fluid properties were assumed. Measured profiles of 

wall temperatures were used as thermal boundary conditions on the walls. Three different types of 

temperature profiles were considered in the experiments: increasing, constant or decreasing as a function 

of the radial distance. Such temperature data for one coolant flow rate and three rotational Reynolds 

numbers was presented in the paper and these correspond to a total of nine different flow cases 

(3 rotational speeds X 3 types of temperature profiles). The temperature plots from the paper were 

scanned to generate the profiles which then were used for wallboundary values. Some extrapolation was 

needed for the smaller radial distances (r/R < 0.3) where data was not available, and a linear extension 

based on the last two points was used. The experimental profiles of the wall temperatures are shown in 

figure 4-12 for a non-dimensional coolant flow of Cw = 7000. 

NASA/CR—2005-212716 37
Simulations were carried out using two different turbulence models: 1) standard k-ε model with wall 

functions, and 2) low-Re k-ε model. Two different computational grids were generated for the two 

models to satisfy the wall y+

 conditions. For the low-Re model, a grid with 84 cells in the axial direction 

and 137 in the radial direction was used. The computed y+

 distances were < 0.3 at all walls. For the 

standard k-ε model the first-cell wall distances are much larger, and a grid with 52 cells in the axial 

direction and 120 in the radial direction was used (with y+

 values at the first cell ranging from approx. 

13 to 100). 

Flow and heat-transfer solutions were obtained at one nondimensional coolant flow rate Cw = 7000, 

for which the measured wall temperatures were published (see figure 4-12). Three rotational Reynolds 

numbers Reθ were considered: 6.6 x 105

, 2.0 x 106 and 3.3 x 106. Calculated wall heat fluxes were 

converted into local Nusselt numbers using the local wall and gas inlet temperatures, and the distribution 

of the Nusselt numbers as a function of normalized radial distance r/R for different flow conditions are 

plotted in figures 4-13 through 4-21. In general the comparison is fair to good except the results for the 

“positive” wall temperature profile at Reθ = 3.3 x106

. Some discrepancy in the results for the positive wall 

temperature profile at Reθ = 2.0 x106

 is also noted. Further studies for the source of this discrepancy are 

needed. 

Results of these series of numerical simulations and the comparison with experimental as well as 

published numerical results clearly indicate that the presently available flow and turbulence models 

(standard and low-Re k-ε models) in SCISEAL provide flow and heat-transfer solutions in disk cavity 

flows that are of adequate accuracy [see also ref. 13]. A number of different turbulence models have 

been used for cavity flows including the k-ω model, and k-ε models with corrections for the rotational 

effects near the wall. This aspect has not been explored in the present work. A comparative study of the 

standard k-ε and low-Re k-ε models with the ‘improved’ models in terms of accuracy, ease of use, 

convergence characteristics should be performed to assess the relative merits of these models and to come 

arrive at the ‘best’ model that describes the rotating cavity flow and heat transfer phenomena optimally. 

NASA/CR—2005-212716 38
NASA/CR—2005-212716 39
 

 

 

NASA/CR—2005-212716 40
 

5. 3–D Secondary and Power Stream Coupling Methodology 

The 2–D, axisymmetric solutions of coupled primary and secondary flows in turbine section were 

presented in Chapter 2. They provided a great deal of important information and insight into the flow and 

heat transfer processes in the secondary flow elements as well as the interaction between the two flow 

streams. Such an analysis capability is essential, and provides relatively fast and detailed solutions. These 

solutions assume steady-state interaction and no circumferential variations in the flow fields. In reality the 

rotor and stator blade wakes produce circumferential variations in the powerstream flow and consequently 

can affect the rim seal flows. In addition, motion of the rotor blades makes the flow inherently unsteady 

due to interaction of the blade wakes from one stage with the flow in the next stage. This also produces a 

transient flow field near the rim seal, which can affect the secondary flow in the cavity. With the current 

drive for optimization of the coolant flow rates, this time-unsteadiness of the powerstream and its 

interaction with the secondary flow stream also may need to be resolved in much more detail. Such an 

analysis ensures a much more detailed picture of the flow at the rim seals, and the interaction between the 

powerstream and the cavity flow. 

NASA/CR—2005-212716 41
The effects of the interaction are present in both the compressor section and the turbine section of a 

typical gas turbine engine. Figure 5.1 shows a schematic of a typical disk cavity pair that is used in the 

inner rows of a multi-stage compressor/turbine. Different requirements and considerations go with disk 

cavity flows in a compressor section and a turbine section, as outlined below: 

Compressor Section: In a compressor section, the ‘downstream’ rim seal is at a higher pressure than 

the upstream rim seal. This drives a flow in the cavity pair such that there is ingress of flow in the 

downstream rim seal and cavity. This flow moves to the upstream cavity through the labyrinth seal, and 

exhausts in the powerstream at the upstream rim seal. The leakage flow affects the engine performance in 

two ways. It represents a net loss because a portion of the compressed air is being expanded through the 

cavity/labyrinth seal and the flow energy eventually is converted to heat. Secondly, the flow coming out 

of the upstream rim seal has tangential velocities that are different than the powerstream flow near the rim 

seal [2]. This changes the inlet velocity vectors near the stator row hub and can affect the stator row 

efficiency. In a compressor section, such alterations in the flow can also impact the stall performance. Of 

interest in a compressor section is the time variation of the leakage flows, the velocity distribution of the 

leakage flow as it gets injected in the powerstream and the resulting interaction with powerstream flow. 

Turbine Section: Flow dynamics in the turbine section is different, with the upstream cavity/rim seal 

at a higher pressure (and temperature) than the downstream cavity/rim seal. This would, normally, result 

in flow ingestion at the upstream rim seal, and exhaust at the downstream rim seal. However, ingestion of 

the hot powerstream gas into the cavities will increase component temperatures and will adversely affect 

life. For this reason, hot gas ingestion into the cavities is usually avoided. This is achieved by injecting 

high-pressure compressor air into the cavities and using it to prevent hot gas ingestion as well as 

providing cooling for the components. Since the coolant flow represents a parasitic loss, current focus is 

on optimization of the coolant flow rates, which would provide adequate cooling capacity at the minimum 

possible flowrates. Of particular interest in the turbine section is the flow dynamics at the rim seal, effects 

of circumferential pressure variations (due to blade wakes) on rim seal flow and the cooling of 

components as the coolant flow is optimized. 

When selecting the numerical tools to attack this very complex problem several issues need to be 

resolved, in order to assure that the flow physics is treated properly and physically plausible solutions are 

generated for the powerstream, disk cavity flow and the interaction between the two. A number of issues 

NASA/CR—2005-212716 42
related to the computational and physical aspects of the solution procedure were considered during the 

development of the coupled code methodology. These were: 

1. Flow codes and solver selection 

2. Methodology for coupling the codes: Physics and numerics, type of data transfer, level of 

coupling 

3. Interface interpolation routines, changes in the flow solvers 

4. Synchronization of the codes 

Description of these issues and the methods adopted in each are described in the following 

subsections. The flowcharts for the overall execution procedure as well as other related procedures are 

also discussed. It should be noted here that there are now, possibly, ‘better’ methods to treat some of these 

issues; the methods adopted and used herein were the best available at the time this work was performed 

and represented the state-of-the-art at that time. Obviously, as flow solvers evolve, other methods may 

become attractive for solutions of this type of flows. 

5.1 Flow Codes 

Flow physics in the two flow streams are widely different. The powerstream flow is compressible, 

transonic and inertia dominated, while the cavity/seal flow is slower, with narrow flow passages, has 

dominant heat-transfer, turbulence and viscous effects. The powerstream flows are usually handled using 

the density-based codes, while the slower flows can be better handled using the pressure-based 

methodology. At a minimum, the solver capabilities needed for treatment of the two flow streams are: 

1. Powerstream: transonic flow, turbulence, resolution of time-accurate interaction between 

successive blade rows in a multi-row machine. 

2. Secondary flow stream: solution of slower compressible flows, turbulence modeling, conjugate 

heat transfer, complex geometry handling. 

Although it may be possible to use a single code to treat both flow regimes, the code performance in 

terms of speed and accuracy may not be optimal. In addition, any single code developed specifically for 

one flow regime could need extensive modifications and validation efforts to be able to handle the 

coupled flows. For these reasons, we decided to use two separate codes, specifically developed for the 

two flow streams, in the project. One can then select mature codes that have been validated and 

demonstrated on the respective flow streams, and the thrust of the research would then be on development 

of the coupling interface only. The codes selected were: MS-TURBO for the powerstream solutions and 

SCISEAL for the secondary flows. Both these codes were developed under different NASA contracts, 

and have been validated and applied to a variety of problems. A brief description of the codes and the 

salient features that are relevant to the present research are given below: 

5.1.1 SCISEAL Code.—This code was developed for flow+heat transfer+dynamics simulations in 

turbomachinery seals and secondary flow elements [3]. It uses a finite-volume formulation for integrating 

Navier-Stokes equations. The velocity-pressure coupling is done through a modified SIMPLEC 

algorithm. Structured multi-block grids are used to discretize the computational domain. Details of the 

governing equations, flux calculations, boundary condition treatment and physical models are given 

elsewhere [3]. Presented here are the salient features of the code: 

1. Treatment of incompressible and compressible flows due to pressure-based formulation, timedependent and steady-state solutions 

2. High order spatial and temporal discretization, body-fitted coordinate (BFC) grids 

3. A variety of turbulence models, including Baldwin Lomax, standard and low-Re k-ε models, k-ω

model, and a 2-layer model. 

4. Implicit multi-media conjugate heat transfer 

5. Stationary and rotating coordinate frames, moving/deforming grid treatment 

6. A comprehensive set of boundary condition types, for treatment of all secondary flow conditions. 

7. Procedures for calculation of rotordynamic coefficients. 

NASA/CR—2005-212716 43
SCISEAL has been validated and demonstrated on a number of benchmark and demonstration 

problems in turbomachinery seals, disk cavities and secondary flow systems. The solutions presented in 

Chapters 2-4 in this report were calculated using this code, and amply prove the capabilities and accuracy 

of the code on relevant disk cavity problems. 

5.1.2 MS-TURBO Code.—MS-TURBO was developed at Mississippi State University for the 

computations of time-accurate flows in multi-row turbomachines [14-17]. It uses a density-based 

formulation to integrate 3–D unsteady Euler/N-S equations on structured, multi-block grids. The flow 

equations are non-dimensionalized and written in generalized coordinates to be able to treat body-fitted 

grids. The convective fluxes are discretized using flux difference splitting and up to third order accuracy 

are possible using Osher-Chakravarthy method. The first-order convective fluxes at a cell face ⎟

⎠

⎞ ⎜

⎝

⎛ +

2

1 i

are written as: 

⎥

⎥

⎥

⎦

⎤

⎢

⎢

⎢

⎣

⎡

= + − ∆ + ∆ −

+

+

+ + + 2

1

2

1

2

1

2

1

~ ~ ~ ~

2

~ 1

i i i i

i

F F F F F (5.1) 

where ±

+

∆

2

1 i

F are the flux differences along the right and left running characteristics. Higher order 

differencing is achieved by adding correction terms to the first-order fluxes. Diffusive terms are 

discretized using central differencing. Fluxes near sharp gradients are limited using Van-Leer flux 

limiting method. Typical turbomachine flows are inertia dominated, and viscous effects in flow-wise 

direction are small and are ignored in MS-TURBO (thin layer N-S equations). An eddy-viscosity based 

turbulence model is available for treatment of turbulent flows. Boundary condition formulation is 

characteristics-based for robustness and accuracy. [14,16] 

For handing time-accurate solutions in multiple rows with relative motion, an algorithm is needed to 

resolve the sliding interfaces between successive rows. In MS-TURBO, a grid deformation/clicking 

algorithm is used to treat the relative motion. Each blade row has structured multiblock grids, and 

successive rows are connected through the sliding/clicking interface. A one-to-one match is maintained 

between the grids at the interface. A deformation zone is associated with each interface. As one blade row 

moves with respect to the next one, the relative motion is in the circumferential direction, and the cells in 

the deformation zone are allowed to distort up to a point and then are snapped/clicked to the next cell in 

tangential direction. The number of time-steps for grid clicking is controlled from outside. When the grid 

coordinates on the end faces of the deformation zone are known, a linear interpolation scheme is used to 

regenerate the grids inside the deformation zone. Grid distortion and clicking implies moving/ deforming 

grids, and a space-conserving moving grid algorithm is used where the grid motion is included in the 

convective fluxes through a coordinate transformation. All of the blade rows are treated in absolute frame 

of reference. 

Each blade row can be separated into several radial zones as needed. The code treats one blade row at 

a time, so that the in-core storage requirement is for one blade row only. This reduces the working 

memory size, and allows treatment of a large number of blade rows. The data related to blade rows other 

than the working row are stored on disk and loaded into the core as needed. 

5.2 Functions of the Interface Routines 

During a typical run, the two codes will run in parallel, each working on separate flow streams, and 

exchanging data at certain times to keep the powerstream and secondary flow linked. The overall 

flowchart for the coupled, transient simulation procedure is shown in figure 5-2. The schematic of the 

NASA/CR—2005-212716 44
typical powerstream-secondary flow cavity shown in figure 5-1 is also modified and shown in figure 5-3 

to denote the various codes and expected interface placements which are used in the coupled codes. The 

interface algorithm between the two codes is invoked frequently during the execution, and has to perform 

different functions. Some of the capabilities that were considered during this development are: 

NASA/CR—2005-212716 45
1. Initial data preparation for each code: this involves identification of the interface boundaries, 

check on the location, size of the domains and initial flow variables and flux preparation. 

2. Code run status: Interface routines check the execution status of each code during a coupled run 

to determine whether the codes are at a proper point for data exchange 

3. Data preparation for exchange: appropriate data from each of the codes at all interfaces is 

collected, sorted and stored for interpolation procedure. 

4. Interpolation of data from one code to another: This is a key step in the interface linking and 

requires a lot of careful attention. Due to the motion of the rotor stages, the interface grids are at 

different physical locations. The data on these have to be ‘rotated’ to match the grid locations 

prior to interpolation. Interpolation scheme is general enough to treat any type of grids 

(structured, unstructured). 

5. Exchange of data: After interpolation of appropriate data from one code to another, the data is 

made available to the other code. Currently the interface data sets are written out to disk files, 

which are accessed by both codes. Appropriate interlocking mechanisms are provided in each 

code to synchronize the data input/output processes in the two codes. 

6. Placement of the data: The data read in from the disk files and placed into appropriate locations in 

each code for use in subsequent iterations/time steps. Different boundary data structures are used 

in the two codes, and this has to be taken into account. 

The interface at present consists of three sets of routines in addition to the modifications made to the 

individual flow solvers. One set is in SCISEAL for data collection, exchange and transfer. The second set 

is in MS-TURBO for similar functions. The third set is outside of the two flow solvers, and is used to 

perform the interpolation of data from one code to another and this set of routines is called from both 

codes. 

NASA/CR—2005-212716 46
5.3 Issues in Formulation of Interface Methodology 

The basis for interface algorithm is discussed in this section. Several different items were taken into 

account during the interface development. Specifically, the items that impacted the coupling procedure 

and methods used to resolve these are described below. 

Code solution methodologies: The two codes, SCISEAL and MS-TURBO, although solve the same 

N-S equations, their solution procedures are very different. The so-called density based formulation used 

in MS-TURBO uses a time-dependent form of compressible flow equations. MS-TURBO uses an implicit 

coupled equation solution method that is geared for time-accurate solutions. It does allow for Newton 

subiterations within each time step, which may not be necessary when the code is running singly. 

SCISEAL, on the other hand, uses a sequential method for solution of N-S equations, and needs several 

subiterations at each time-step. This has bearing on code synchronization as well as the level at which the 

data transfer can take place during execution. 

Flow variables: The primitive variables in MS-TURBO, [density, momentum, total internal energy] 

(ρ, ρu, ρv, ρw, e), are nondimensionalized as compared to those used in SCISEAL [pressure, velocity, 

total enthalpy] (p, u, v, w, H). This means additional data inputs are needed for reference values used in 

MS-TURBO, and additional operations are needed to convert data sets from non-dimensional to 

dimensional form. Conversions such as from total internal energy e used in MS-TURBO to total enthalpy 

H in SCISEAL need to be considered. MS-TURBO uses the ideal gas law for the working fluid, with 

constant specific heats, and a similar specification was used in SCISEAL. 

Flux calculations: Both codes use a finite volume treatment, and evaluation of fluxes at the interface 

is a key consideration when transferring data across this interface. MS-TURBO uses a flux-difference 

splitting method with the density-based, coupled form of N-S equations (conservative form), while 

SCISEAL uses products of convective fluxes and primary variables (strong-conservative form) to 

evaluate the fluxes. The interface algorithm should be worked in such a way that the interface fluxes from 

the two codes match, so that conservation of fluxes across the interface is ensured. 

Boundary condition treatment: The methodology used to treat boundaries and to calculate 

boundary fluxes has direct relevance to the interface treatment. Characteristics-based boundary condition 

treatment is used in MS-TURBO. A phantom layer of cells is stored next to each boundary, and this 

information is used for boundary flux calculations. SCISEAL code uses local flow conditions at a 

boundary and the type of boundary condition to come up with a treatment for flux computations. In 

SCISEAL, a phantom cell layer is assumed, but never used explicitly. Instead, equivalent expressions for 

boundary values of variables are calculated and directly used. 

Placement of interface: This can affect the solution accuracy as well as the stability of the solution 

procedure. A number of different constraints on the location and shape of the interface can be considered 

based on code methodologies and flow. The location should be compatible with the requirements for the 

sliding/clicking interface needed for MS-TURBO; local geometry features at the rim seal need to be 

considered, and the location should be in relatively benign flow regions, e.g., avoid recirculation zones as 

much as possible. The typical rim seal geometry has the upstream blade platform lip overlapping the lip 

of the next row blade platform as shown in figure 5-3. This geometry, coupled with the powerstream flow 

generates a recirculation zone at the rim seal (backward-face-step type flow). 

The obvious location of the interface is shown in figure 5-4a. This allows simpler domain geometry 

definitions and cleaner shapes for sliding interfaces. The interface, however, is almost certain to intersect 

the recirculation zone expected in the rim seal. The interface could be moved back in the neck of the rim 

seal as shown in figure 5-4b, which will probably avoid the rim recirculation, but this now poses 

problems with geometry definition and the placement of the clicking interface for MS-TURBO. Such a 

placement would require treatment of different of boundary types at different i/j/k planes. The MSTURBO code had a limited range of boundary type and i/j/k face combinations and placement of the 

interface in the rim seal neck would have required implementation of several additional boundary types. 

For example, on a ‘west’ or ‘east’ face boundary in MS-TURBO, currently only an inlet boundary is 

NASA/CR—2005-212716 47
supported, while a wall boundary specification would be needed if we decide to extend the interface into 

the rim seal gap. For these reasons, the interface location as shown in figure 5-4a was finalized. 

Interface shape: The interface strategy should be independent of the geometry of the interface. Two 

geometrical constraints were placed on the interface shapes due to the type of the flow and ease of grid 

generation. The edges of the interfaces in θ direction have to be circular arcs and this restriction comes 

from sliding interface (the circumferential boundary lines can not be wavy). The interface should be 

generated by revolving a curve in the r-x plane, and this curve should preferably be a straight line in the rx plane whenever possible, where x is the axial coordinate. 

5.4 Flow Treatment at the Interface 

All of the items mentioned in the previous section were taken into account during the building of the 

flow solution methodology at the interfaces. The actual steps and methods that were used to resolve these 

issues are discussed below. 

Conservation of fluxes at interface: As remarked above, MS-TURBO uses a phantom layer of cells 

next to a boundary surface to calculate the fluxes at the boundary, while a specified flux value at a 

boundary can be used directly in SCISEAL. This allowed a way to calculate the fluxes, which would 

ensure conservation at the interface. The basic methodology is: 

(a) Primitive flow variable values from the cell layer next to the interface in SCISEAL are 

interpolated from SCISEAL to MS-TURBO interface grid. This step accounts for the differences 

in relative locations of the individual surface grid sets for each code. The interpolated primitive 

variables are nondimensionalized and used directly in the phantom layer of cells next to the 

interface boundaries in MS-TURBO code. The boundary fluxes are then calculated in MSTURBO using the normally used flux-difference splitting algorithm. 

(b) The boundary fluxes in MS-TURBO are then transferred to the interface routines, 

dimensionalized, rotated appropriately, and then interpolated from the MS-TURBO to SCISEAL 

interface grid. Care is taken to ensure flux conservation during the interpolation procedure. 

(c) The interpolated fluxes are used to enforce boundary conditions in SCISEAL at the interface. 

Since the flux direction can be into or out of the boundary, care is taken during boundary 

condition implementation. 

(d) The fluxes for k and ε equations from SCISEAL at present can not be calculated from the 

MS-TURBO code version used in this project. Instead, values of k and ε are calculated locally at 

each interface boundary cell in SCISEAL and then mass fluxes at the interface are used to 

calculate the convective flux of k and ε at the interface boundary. 

NASA/CR—2005-212716 48
A schematic of this variable/flux transfer methodology is shown in figure 5-5. 

The above procedure ensures that both codes use the same fluxes at the interface, and thus flux 

conservation is enforced. The approach uses existing code methodologies at boundaries and provides a 

consistent way to handle this important and difficult step. This approach has been coded and tried out and 

performs very well as will be shown in the next chapter. 

Level of linking of the two codes: This refers to the how frequently the two codes exchange data 

during execution, and at which level the exchanged data is used. One possibility was to exchange the data 

at the end of each time step. This would make the procedure completely explicit, reduce the algorithm 

stability, and put restrictions on the size of a stable time step. The next level was to exchange data several 

times during a time step. This method requires that the codes perform subiterations during each time step. 

SCISEAL code performs subiterations due to the pressure-based formulation. The equivalent in 

MS-TURBO was the Newton subiterations, where this capability is typically used for enhancing the 

temporal accuracy of the solution. However, in the present case, it was also used for allowing a much 

tighter coupling between the two codes. Typically the number of iterations needed for SCISEAL were 

much higher than the Newton iterations needed in MS-TURBO. The number of subiterations between 

each data transfer for each code is flexible, and is a part of the input data. With this tighter coupling, the 

stability of the coupled execution procedure was enhanced. This was tested on simple problems where the 

data exchange was done once a time step, and several times during a time step, and the stability of the 

solution procedure was seen to be better with multiple data transfers. 

Synchronization of the codes: The two codes use different solution methodologies and also will 

operate on different flow domain sizes. For these reasons, the execution times per time step/subiteration 

for the two codes usually are quite different. Synchronization of the execution of the two codes and data 

exchange at appropriate times can become a problem. In the present algorithm the data exchange is done 

through data files that are written to a disk. The readiness check of each code for data exchange is done 

through two sets of files. A flag marker file is written out by each code when it writes out a data set to the 

disk. The other code then checks for the existence of the flag file and reads in the data set from the other 

code. After the reading is complete, the flag file and the data file are deleted from the disk. When writing 

out data sets, the existence of this flag and data files is checked, and if they exist, the codes go into a 

timed sleep mode and check the files periodically. To avoid indefinite execution of one code in case if the 

other code stops execution for some reason, an upper limit on the total wait time is enforced. If the other 

code does not read the older data sets in this time span, then the execution of the first code is stopped with 

an error message. 

NASA/CR—2005-212716 49
The data exchange can be done through more sophisticated methods such as MPI or internet sockets. 

However, three reasons are found compelling for using data transfer through disk files: 

1. Interface data sets are not expected to be very large because the sizes of interfaces are usually not 

very large, and file data transfer is acceptably fast. 

2. During execution, one can look at the data sets if they are written out in ASCII format to check on 

the time stamps, values etc. This can give an indication of the state of health of the coupled 

execution run. 

3. In case of abnormal termination of any one of the codes, the last data sets will stay on the disk 

and perhaps provide clues to the reasons for termination, and provide an intermediate point for 

restarting the run. 

5.5 Interface Data Interpolation Methodology 

One of the key issues in the interface treatment is the way the data are interpolated from one code to 

another. The complexity of this procedure naturally depends on the complexity of the interface 

geometries, computational grid topology at the interface, relative locations of the interface and the degree 

of accuracy needed (in terms of conservative properties). Additionally, the procedure for collecting the 

interface data before interpolation is also a consideration. Multiple steady/stationary powerstream blade 

stages interacting with stationary cavities/rim seals present a very challenging problem at the interface of 

the two flow streams, and given below are some details of the strategy used to handle this. The important 

considerations are: interface geometry and location; grids used on the interfaces; collection of needed data 

at the interface from the two codes; methods used for interpolation of data across the interfaces; placing 

the interpolated data back to the two codes for use in computations. 

Interface geometry and location: In a typical coupled powerstream-secondary stream problem, the 

flow domains associated with the disk cavities are completely stationary in time. Grids associated with the 

stator rows are stationary in the main, except the deforming zones at sliding interfaces. The domains 

associated with the rotor stage(s), however, move with the rotor blades and also change shapes in the 

deforming zones. The interface patches between MS-TURBO and SCISEAL, thus can be physically 

located far apart from each other, or may be partially overlapping. A typical example of this is shown in 

figure 5-6, where interfaces for the three components from a rotor-stator-cavity combination are shown. 

In order to interpolate and transfer the data across the interfaces, the procedure established was: 

1. Angular locations of a reference point on each interface are tracked in time, to get the relative 

positions of the interface pairs. 

2. Before the interpolation procedure, the data donor surface/patch from SCISEAL or MS-TURBO 

is imaged to the data receiver surface/patch of the other code. Two consecutive images of the 

donor surface are generated, in order to ensure that the receiver surface is completely ‘covered’ 

by the donor surface images (figure 5-6). 

The interpolation subroutines are now fed the geometrical details of the double-imaged donor surface 

and the single receiver surface for data processing. 

The interpolation subroutines are now fed the geometrical details of the double-imaged donor surface 

and the single receiver surface for data processing. 

Surface grids on interface boundaries: The grids associated with SCISEAL flow domains are 

stationary in time and the surface grids usually consist of structured quadrilaterals. The grids on the MSTURBO interfaces will also be structured quads. However, the interface boundary shapes as well as the 

grids change shapes at each time step. The reason for this is the deforming zones associated with the 

deforming/clicking algorithm. The interpolation algorithm thus needs to account for the geometry and 

grid changes at each time step. 

NASA/CR—2005-212716 50
Collection of interface data: Has to follow the solution methodology of each code and the type of 

data to be transferred across. The primary flow variables are transferred from SCISEAL. These are 

updated at the end of each iteration, and are available easily from their respective storage locations. The 

data from MS-TURBO are the boundary fluxes for the five governing equations (continuity, 3 momentum 

equations, and energy,) and retrieving this information is more involved. As remarked in a previous 

section, MS-TURBO accesses information one blade row at a time. The linear implicit set of discretized 

flow equations is inverted at each Newton subiteration, and the flux information in overwritten during the 

inversion procedure. For this reason, the fluxes have to be stored during the ‘forward sweep’ of the 

solution algorithm, one blade row at a time. The MS-TURBO code needed modifications at a much 

deeper level in the algorithm than the SCISEAL code. Both convective and diffusive fluxes are collected 

in MS-TURBO. 

Data preparation for interpolation: This is a two step process. In the first step the raw data from 

each code is first brought into dimensional form. SCISEAL code works on dimensional flow variables, 

and thus the first step is not required. MS-TURBO code, however, uses nondimensional flow equations, 

and both the convective and diffusive fluxes have to be dimensionalized separately before transfer to the 

interpolation algorithm. 

The second step involves conversion of this data for rotation/imaging needed during interface match. 

Both codes use Cartesian velocity components as the primary variables and body-fitted generalized 

coordinate systems. For interface rotation, however, the fluxes and the variables in the flow equations in 

Cartesian system can not be used directly. Instead these are first converted locally into the equivalent 

r-θ-x coordinates, (i.e., a cylindrical coordinate system). This is accomplished by using a simple 

transformation of the type: 

⎥

⎦

⎤ ⎢

⎣

⎡

φ

φ

⎥

⎦

⎤ ⎢

⎣

⎡

− θ θ

θ + θ

⎥ =

⎦

⎤ ⎢

⎣

⎡

φ

φ

θ k

r j

sin cos

cos sin

 (5.2) 

for the radial and tangential velocities, ur and uθ as well as for the fluxes along the radial and tangential 

grid lines. Imaging this converted data set now essentially means keeping the same flux/variable values, 

but changing the θ coordinate appropriately. The values of the new θ coordinates for each interface data 

set are determined from the relative locations of the interfaces. Once the new θ values are known, the 

fluxes/variables in the r-θ-x coordinate system are converted back to the Cartesian system via a reverse 

transformation: 

NASA/CR—2005-212716 51
⎥

⎦

⎤ ⎢

⎣

⎡

φ

φ

⎥

⎦

⎤ ⎢

⎣

⎡

+ θ θ

θ − θ

⎥ =

⎦

⎤ ⎢

⎣

⎡

φ

φ

θ

r

k

j

sin cos

cos sin

 (5.3) 

The fluxes/variables are then ready for interpolation from the donor face sets to the receiver face sets. 

Interpolation procedure: This is another key aspect of the interface methodology. It is a very 

complex problem due to: 

(a) cylindrical interface shapes; 

(b) surface grids which change continually and are usually skewed; 

(c) partially overlapping surface sets, where the receiver surfaces will cover only 50 percent of the 

area of the donor surface image pair; 

(d) need for fast procedures because the interpolation routines will be used a number of times by both 

codes during each single time step. 

Note is also made of the fact that the donor data of fluxes/variables are not available at the grid nodes, 

but at the centroids of the faces or cells, and these values have to be interpolated to the centroids of the 

receiver surface. 

An algorithm was developed at CFDRC to treat such a problem of interpolation and the method is very briefly 

described here. Additional formulation is given in appendix B. The method uses the following key steps: 

1. Normal vectors at each grid face on the donor surface are calculated first. Any type of surface 

element can be treated, including triangles, quads and arbitrary polyhedra. For faces with more 

than three sides, the normal direction may not be unique, and a weighted average procedure is 

then used. 

2. The face-center data (fluxes, variables) available on the donor grid is then transferred to the face 

corners using a Laplacian interpolation algorithm. 

3. Gradients of the variable data at the face centers of donor grid are calculated using the corner 

values found in step 2. 

4. For each of the face centroid from the receiver grid, the closest face centroid from the donor grid 

is found next. This is needed for the final interpolation procedure 

5. Each receiver face centroid is projected in the face-normal plane of the closest face/centroid in 

the donor face. Variable value at the receiver centroid is then found by using the corresponding 

value at the donor face centroid, gradient at the donor face centroid and the distance between the 

donor and receiver face centers. 

The interpolation procedure is used several times during a typical time step and speeding up the 

process is of help. Some speedup was achieved by storing the information related with donor face 

normals and the centroid neigbors in step 4. This information is calculated once at the beginning of each 

time step and used subsequently. Steps 2, 3, and 5 deal with variables to be interpolated, and have to be 

repeated at each data exchange. 

The procedure described above is not guaranteed to be flux conserving in the global sense, i.e., if the 

variables/fluxes were integrated over the donor and receiver surfaces, the two may not match. This is not 

very crucial for variable transfer from SCISEAL to MS-TURBO, but the reverse transfer of fluxes from 

MS-TURBO to SCISEAL must be conservative. To achieve this, an additional integration step was added 

in MS-TURBO. The fluxes from the donor and receiver surfaces are integrated and the two values 

compared. The interpolated fluxes on the receiver surface are then adjusted using a simple constant 

multiplication factor to equalize the integrated/global values from the donor and receiver. 

One further improvement to the interpolation procedure could involve the use of a flux conserving 

methodology where the faces from receiver grids are projected into the donor faces. A surface cutting 

NASA/CR—2005-212716 52
algorithm is then used to find out the intersection and overlaps of the donor and receiver surfaces. The 

fluxes are then interpolated from the donor surface to receiver surface grids using weighted area averages 

of the overlapping areas, and finally the contributions to each of the receiver grid faces are summed up. 

Such a procedure can be exactly flux conserving for donor-receiver surfaces which are planar. For 

cylindrical donor-receiver surface pairs, however, the accuracy of flux conservation will depend on the 

grid distribution, grid coarseness and other factors, and the overall effort may be only as accurate as the 

method currently being used. 

Placement of interpolated data: This is the last step in the interface treatment procedure. As 

mentioned above, the interpolated data is written out to disk files for the other code to read in. On the 

MS-TURBO side, the input data consists of the variable values for the phantom layer. The input variable 

data is nondimensionalized first, and then stored at the appropriate boundary region phantom layer for 

use. On the SCISEAL side, the input data are fluxes from MS-TURBO. These are stored in the 

appropriate boundary storage array associated with the SCISEAL boundaries. 

5.6 Summary 

The methodology for a coupled, transient, 3–D solution procedure using two different codes for two 

different flow streams in a turbomachine, e.g., gas turbine engine, was described in this chapter. The 

rationale for the procedures and choice of the codes used, SCISEAL and MS-TURBO was described, 

followed by the various issues associated with the coupling procedure and the methods used in the present 

work to address these issues. The procedure for interpolation of data needed for coupled execution was 

described next to complete all aspects of the coupled execution. This methodology has been coded, 

debugged, and used on two test problems, a turbine rig problem and to a compressor rig. Description of 

these cases, solution methodology and sample results are described in the next Chapter. 

6. Coupled, Transient Analyses of Power Stream-Secondary Flows

The codes and methodology described in the previous chapter was utilized to compute several 3–D, 

coupled, powerstream and secondary flows in gas turbines. Specifically, the codes were tried out on a 

simple case to validate/checkout the codes and coupling procedure. Second case was the high-pressure 

turbine rig developed by UTRC to test a high-work turbine stage. Third case that was attempted was a 

section from the NASA Glenn Research Center’s Large Low-speed Compressor Rig (LSAC) that was 

built for generating flow data for code validation. These simulations comprised the validation and 

demonstrations problems. Details of these simulations are presented in this Chapter. 

6.1 Bladeless Rotor+Stator+Cavity in a Turbine Section 

This was the first case tried out and also served to debug the codes as well as validate the numerical 

models and the interface treatment. As would be appreciated, testing the time-accurate, coupled code 

methodology is not very easy for lack of suitable benchmark problems. A simplified case was therefore 

developed that could be solved by one of the two codes (SCISEAL or MS-TURBO) on its own, and this 

solution taken as the benchmark. The coupled codes were then tried next and the simulation results 

compared with the single-code simulations for validation and sanity checks. The MS-TURBO code was 

hardwired to handle only the powerstream flow and could not be used to treat the cavity portion as well. 

SCISEAL did have the flexibility to handle both flow streams, except the sliding interface between the 

stator and the rotor stages. The one way out was to consider a rotor+stator+cavity problem where the 

blades in the powerstream were taken out. This reduced the problem to a steady-state, axisymmetric flow 

NASA/CR—2005-212716 53
which could be handled by SCISEAL alone. A number of variations on this bladeless powerstream 

problem were tried and duplicated with the single code as well as the coupled codes. 

6.1.1 Flow Geometry and Boundary Conditions.—The flow geometry consisted of a bladeless rotor 

stage followed by a bladeless stator stage, with an intermediate rim seal attached to a disk cavity with a 

very simple geometry. A solids model (solid surfaces with computational grids) is shown in figure 6-1 

along with the boundary conditions and flow conditions that were used. The powerstream flow inlet 

boundary was at 300K, Mach 0.25 and the exit pressure was set at 100 kPa. The upstream stage was the 

rotor, and the hub wall was rotating at 1000 rpm. The rim seal gap was attached to an L shaped disk 

cavity, and the pressure conditions at the disk cavity inlet were specified as a boundary condition. All disk 

cavity walls attached to the rotor section were also treated as rotating walls. The powerstream conditions 

were held fixed, while the cavity inlet pressure were varied. With a sufficiently low inlet pressure the 

powerstream flow could be ingested into the cavity and by raising it the cavity flow could be forced into 

the powerstream at the rim seal. These cases were tried out with both cavity flow ingress and egress at the 

rim seal and the coupled code methodology checked out under both conditions. 

The steady-state simulations were carried out with SCISEAL on a multi-block (1 block in 

powerstream and 2 blocks in the disk cavity) structured grid that was also used in the coupled code 

simulations. The grid was kept fairly coarse for fast execution and debugging. Two main cases were 

considered: one with definite flow ingress into the cavity and the other with a clear flow egress into the 

powerstream. Simulations and results of these cases are described next. 

6.1.2 Flow Ingress in Cavity.—The cavity pressures were set to a low value of 98 kPa and the 

SCISEAL code was first used to obtain the steady-state simulations of the coupled powerstream-cavity 

flows. The same problem was then run in time-transient mode with the coupled codes and this was 

continued till a time-invariant solution was obtained. The mass flow rates at the cavity inlet/outlet plane 

were compared from the two sets of simulations and these were: 1.92 x 10–3 kg/s for the run with 

SCISEAL code alone and 1.83 x 10–3 kg/s for the coupled code run, and the two sets correlate well. 

NASA/CR—2005-212716 54
The structure of the flow near the rim seal is of interest and was checked for major flow features as 

well as pressure field. Combined velocity + pressure field plots from the single code run and the coupled 

code run are shown in figure 6-2a and 6-2b. Plotted here are the flowfields below the rim seal, i.e., the 

region handled by SCISEAL in the coupled runs. 

Due to the fast powerstream flow, a recirculation zone is created at the rim seal interface. The cavity 

wall attached to the rotor spins and produces disk-pumping action, so that the flow near this wall always 

moves up radially. This flow gets turned at the rim seal interface, and again at the opposite stationary wall 

of the disk cavity. Due to the recirculation zone at the seal, the ingested powerstream flow enters the rim 

seal near the stationary wall of the cavity. As seen from the plots in Figs 6-2a and b, the velocity pattern 

associated with the recirculation zone as well as the stagnation pressure near the rim seal on the stationary 

side is very similar in both runs. This shows that in this case, when there is a net ingress into the cavity 

the coupled codes produce similar results to the single code run. 

6.1.3 Flow Egress from the Cavity.—For this run, the cavity inlet pressure was set to 102 kPa with 

the powerstream conditions left unchanged. The single code results from SCISEAL produce a net flow 

into the cavity (and out of the rim seal to powerstream) of 2.388326e–3kg/s, and this compares very well 

with a computed flow egress from the rim seal of 2.256348E–03 kg/s for the coupled code run. 

The velocity + pressure field plots for an r–x plane for the single code and coupled code runs are 

shown in figures 6-3a and 6-3a. As before, the gross flow features as well as the pressure field distribution 

is very similar in the two runs. 

Due to the flow egress condition at the rim seal, the flow features are different from the earlier case, 

with the rim seal region showing almost no recirculation. The disk pumping on the rotor wall augments 

the exiting flow and the radial momentum of this flow carries it in the powerstream in a near-radial 

direction. However, away from the rotor side cavity wall, the rim seal velocity shows the effects of the 

axial momentum of the powerstream flow, which tends to force the rim seal flow in the axial direction. A 

recirculation bubble forms near the cavity stator wall in this case, and the two sets of results show very 

similar velocity distribution near this recirculation zone. 

This example served to show that the mass and momentum flux calculation as well as the data 

exchange at the interface is taking place properly, including the geometry manipulation and interpolation 

algorithm. Relative pressures in the cavity and powerstream decide the flow direction at the rim seal, and 

this example showed that the pressure information in the individual flow domains as well as across the 

interface is being transmitted properly. Although not shown here, the pressures are continuous across the 

interface, as will be shown in the next example where the two flow streams were plotted together. 

NASA/CR—2005-212716 55
6.2 UTRC High-Pressure Rig Simulations 

A test rig was built at UTRC to test a single rotor+stator+cavity configuration of a high-work turbine 

stage. Although not run at the actual engine conditions, the rig was built to provide detailed pressure, 

temperature and velocity information in all regions in time-averaged form and more importantly, in 

unsteady form. With this data the understanding of the dynamics between the powerstream flow and the 

disk cavity flows would be enhanced, and the unsteady data generated by the rig could be used for CFD 

code validation. This flow problem was simulated using the coupled code methodology developed here. 

The time-accurate results generated in the simulations are to be validated against the data from the H.P 

Rig, and also provide flow details to UTRC for better instrumentation in the rig [19].

6.2.1 Geometry and Flow Information.—A cross section of the H.P. Rig is shown in figure 6-4 and 

shows the major components and flow directions. The circled area is the flow domain of interest and 

details of the geometry in this area is shown in figure 6-5. The powerstream flow domain consists of a 

stator vane that guides the incoming flow, followed by a single rotor stage. Two disk cavities are present 

on either side of the rotor stage, and the disk cavity upstream of the rotor stage is the cavity of interest. 

This interstage cavity interfaces with the powerstream at the rim seal. As shown, the rim seal has a 

‘tongue and groove’ form and the overlap of the stator platform over rotor platform generates a backward 

facing step configuration. The powerstream flow will generate a recirculation zone at the rim seal as a 

result of this overlap. A three knife stepped labyrinth seal is present at the entrance of the cavity. 

Blade counts on the stator vane and rotor stages were 48 and 58 respectively. If treated exactly, the 

representative PI sector would be 180 degrees, and would lead to a very large computational grid. For this 

reason, the blade count ratio was adjusted to 48 and 60 blades in the stator and rotor stage respectively, 

and the rotor blade thickness was adjusted to maintain the blocking factor. With this adjustment, the 

representative PI sector was set at 30 degrees, with 4 blades in the stator stage and 5 blades in the rotor 

included in the calculation domain. 

Multi-domain structured grids were built in the powerstream domains, with one domain in each 

blade-to-blade block of the stator and rotor stages. Grids in the radial directions were matched exactly at 

the rotor-stator sliding/clicking interface. Grids in the θ direction were also matched one-to-one at the 

rotor-stator clicking interface. In θ direction, however, this match is over the entire flow problem, and this 

puts some restrictions on how the θ direction grid can be distributed in the individual blade-to-blade 

blocks (the θ direction cell counts in stator and rotor blade-to-blade blocks must be in inverse ratio to the 

blade count ratio). In the present case, the grids in each of the blade-to-blade block in the stator vane had 

NASA/CR—2005-212716 56
49 by 12 by 15 cells in the axial, radial and θ direction. The corresponding distribution in the rotor stage 

was 36 by 12 by 12 cells in each blade-to-blade block. This yielded a total of 61200 cells in the 

powerstream. The deformation zones ahead and after the rotor-stator clicking interface each had 4 cells in 

the axial direction. This is a relatively coarse grid, and should be refined. The tip clearance for the rotor 

stage was ignored for this computation. For the disk cavity and the labyrinth seal (SCISEAL flow 

domain), a multiblock, structured grid with 16 blocks was built and was generated by revolving a set of 

faces that define the r–x cross-section of the cavity. The computational grid for cavity+rim seal had 

approximately 33000 cells and used 30 cells in the θ direction to interface with 60 cells from the 

powerstream grid. figure 6-6 shows a solids model of the cavity and rim seal grids. The grids in the 

powerstream blocks were relatively straightforward, with H grid topology in each blade-to-blade block. 

The grids in the rotor move with the rotating blades, and could be physically located anywhere in the 

circle. These have to be rotated and imaged for interpolation to the stationary grids, as was outlined in the 

previous chapter. Figure 6-7 shows the relative locations of the three grids at a given time during the 

computations. 

NASA/CR—2005-212716 57
NASA/CR—2005-212716 58
Air was used as the working fluid. In the powerstream, it was treated as a constant viscosity fluid and 

an eddy viscosity based model was used to treat turbulence. The upstream boundary for the stator row is 

an inlet Mach number and stagnation quantities (pressure and temperature). The incoming flow was taken 

as axial. The inlet Mach numbers is rather low at 0.09. At the exit of the rotor stage, static pressure with 

inertial radial correction was specified (the radial pressure gradient is matched to the centrifugal gradient 

generated by the tangential/swirl velocity at the exit). The shroud was a stationary wall. All the walls on 

the stator stage were stationary adiabatic walls, and the rotating, adiabatic walls were imposed on the 

rotor surfaces. The rotor speed was 3600 rpm. The inlet flow temperature was at room condition, 302.6 K. 

The powerstream inlet total pressure was set at 155 kPa/22.4 psia and the nominal exit pressure was 

122 kPa/17.8 psia. The nominal exit pressure was imposed at the shroud of the powerstream exit, with 

decreasing pressure towards the hub as a result of the radial inertial balance. 

The cavity and rim seal flow was treated as a compressible, variable property flow and the turbulence 

was handled with the standard k–ε model. The cavity inlet condition was specified in terms of the 

stagnation pressure and temperature. The stagnation temperature was set at room conditions/ 302.6 K and 

the stagnation inlet pressure was specified in terms of a fraction of the powerstream inlet total pressure. 

Several runs at different inlet pressure ratios (cavity total pressure/powerstream inlet total pressure) were 

completed: 0.97, 0.88 and 0.8. 

Time step to be used in the coupled execution is determined by the powerstream code, MS-TURBO. 

The time step is specified in terms of the number of distortion steps to be taken before the grids in 

θ direction are clicked to the next grid. Once the circumferential grid-count in the powerstream and the 

rotor speed are known, the physical time step size is fixed. In the present solutions, the time step was set 

so that 16 deformation steps were taken in-between each grid click. This yielded 640 time steps per 

30 degrees of rotor travel. The corresponding maximum CFL in MS-TURBO was approx. 8. For the 

present runs, first order time and space discretization in powerstream were used, while first-order time 

and second order central differencing were used in the cavity flow. 

6.2.2 Results and Discussion.—Steady-state simulations of the cavity and powerstream were also 

performed to quantify the rim seal flow rates, which provided an anchoring point for the flow in a 2–D 

axisymmetric mode, where the blade wakes are ignored. Once the time-accurate simulations were done, 

these could than be compared and contrasted with the 2–D runs to assess the size of changes caused by 

the axisymmetric flow assumption. Representative 2–D velocity vectors in the cavity for an inlet pressure 

ratio of 0.97 are shown in figure 6-8 and clearly show the recirculation dominated cavity flow, as well as 

the recirculation zone at the rim seal. Location of the interface for the coupled MS-TURBO and 

SCISEAL run is also shown in this figure for reference and the interface could be expected to intersect the 

rim seal recirculation zone. The mass flow rate in the rim seal for this configuration was 

0.278x10–3 kg/sec for a 30 degree PI sector. 

The time-accurate, coupled solution runs were started with initial runs on both TURBO and 

SCISEAL codes, with the interaction turned off. The disk cavity solution was obtained with SCISEAL, 

and for this run constant flux values were specified at the interface boundary at the rim seal; the 2–D 

solution data was used to estimate these flux values. The initial run on the powerstream flow was done 

with MS-TURBO running in single code mode, with wall conditions in place of the rim seal interface. All 

of the other flow and boundary conditions were maintained at the desired values. Since the aim of the 

initial run was to wash out the initial condition, the time step in TURBO run was increased to 4 times the 

coupled execution time step, and the code was run for 600 time steps. 

After the initial runs were completed, the parallel execution was started, and at a preset time step, the 

interface boundaries in both were ‘opened’ by starting the data exchange; this was similar to breaking 

open a membrane in-between the two codes. The exchanged data was underrelaxed for a prespecified 

number of initial time steps and then the underrelaxation was removed. The coupled execution procedure 

was continued for at least two PI sector rotations, i.e., for at least 60 degrees of rotor turn. At this point 

the flow was nearly time-periodic and then the solutions for the next 30 degrees of rotor turn were 

collected for processing. 

NASA/CR—2005-212716 59
As remarked earlier, three runs with cavity inlet stagnation pressure at 0.97, 0.88 and 0.8 times the 

powerstream inlet stagnation pressure were completed. 3–D time accurate solutions generate voluminous 

data and it is difficult to show it in detail. Only representative plots are shown here and discussed. The 

results have also been used to prepare slides of results at different times steps and these have been 

combined to produce animated plots. See CD attached to this report. 

A representative pressure surface plot in the powerstream domain (MS-TURBO solution) is shown in 

figure 6-9, showing the pressure distribution along the hub surface which also contains the interface 

between MS-TURBO and SCISEAL. The stator blade wakes are clearly visible (although not very 

dramatic for the test rig conditions). The wakes then interact with the cavity flow and affect the interface 

pressure distribution, and exert some influence near the entrance of the rotor blade row. The flow is 

expanding along the powerstream and the continually decreasing pressure along the powerstream flow 

direction reflects this. 

One of the assumptions in the powerstream-cavity flow interaction was that the blade-wake 

interaction in such problems could be strong, providing substantial changes in the rim seal flow field. In 

the present case, however, such changes were not seen. In fact, the serpentine passage in the rim seal and 

cavity seemed to produce a large amount of flow damping, so that the flows near the labyrinth seal were 

perturbed to a very small degree. 

Two representative velocity plots are shown here to explain the calculated flow fields. The location of 

the cutting planes was fixed based on the location of the rim seal with respect to the stator blade wakes. 

Figure 6-10 shows the “wake” cross-section and “midplane” cross-sections used in the plots. Figure 6-11 

shows the “complete” cross-sectional surface that includes the cavity and the powerstream and illustrates 

the complexity of the flow domain. All of the vector plots shown here used combined cutting planes as 

shown in figure 6-11. 

Two velocity vector plots in the r–x cross section of the cavity+powerstream are shown in 

figures 6-12a and b. The rim seal in figure 6-12a is in the blade wake, and it is midway between two 

wakes for figures 6-12b. The recirculation zone in the rim seal area is clearly seen. When the cutting 

plane is in the wake region this recirculation zone is somewhat weaker than for the cutting plane in 

midway plane where the pressure levels are lower. There are also some differences in the velocity plots 

and pressure values in the neck region and cavity below, but it is too small to be seen in these plots. Some 

NASA/CR—2005-212716 60
NASA/CR—2005-212716 61
preliminary experimental data from the rig suggests that the pressure changes in the cavity, induced by 

the blade passing, are very small, of the order of a few percent of the powerstream pressures, and this 

correlates well with the plots shown here. 

The velocities in the cavity cross section show a torturous flow path, flow threads and numerous 

recirculation zones. The right side wall and bottom labyrinth wall are rotating. This produces pumping 

action along all vertical walls and generates a large recirculation zone in the vertical open area of the 

cavity. The flow moves into the rim seal neck along the top surface, goes around the rotor ledge and then 

is slung out towards the stator ledge. The recirculation zone near the rim seal also helps this motion. The 

cavity flow then moves along under the stator ledge till it mixes in the mainpath flow. The stepped 

labyrinth seal shows the usual recirculation zones, the main one in the labyrinth cavity and another in the 

step region. 

The velocity plots in figure 6-12a or b can also be compared with the 2–D solution shown in 

figure 6-8. The main flow features are similar except the recirculation zone in the rim seal area, which is 

much flatter in the 2–D solutions as compared to the coupled run. One reason is that the blades in the 

NASA/CR—2005-212716 62
rotor stage were ignored in the 2–D run, and these produce flow disturbances which would tend to reduce 

the recirculation zone in axial direction. The mass flow through the rim seal in the 3–D run varied from 

0.22–0.26 kg/s as compared to 0.278 kg/s seen in the 2–D run, which are in fairly good agreement. Such 

comparisons in flow structure and flow rates will be ultimately useful in assessing the 2–D results with 

the ‘correct’ 3–D time accurate solutions as more flow cases are analyzed. 

Reducing the cavity inlet pressure ratio from 0.97 to 0.88 reduced the rim flow into the powerstream, 

but the flow structures remained essentially the same. A large reduction to a pressure ratio of 0.8, 

however, produced results that were substantially different in terms of the flowrates at the rim seal which 

went from approx. 0.0146 kg/s into the powerstream at pressure ratio 0.88 to a flowrate of 0.0165 kg/s 

into the cavity at a pressure ratio of 0.8, indicating that the zero flow rate at the rim seal could be inferred 

to be at approx. a pressure ratio of 0.85. UTRC had some experimental data for the average flow rates into 

and out of the cavities and the data indicated that the zero flow rate condition was seen at a pressure ratio 

of 0.84. Thus, good correlation was seen between the numerical and experimental data. 

A representative velocity plot in the midway plane for pressure ratio of 0.8 is shown in figure 6-13a to 

illustrate the changes in the cavity flow when the rim seal ingests the powerstream flow. For comparison, 

the corresponding vector plot for pressure ratio of 0.88 is shown in figure 6-13b. The obvious differences 

are in the labyrinth seal area where the flow vectors on top of the teeth have reversed direction in 

figure 6-13a (flow from right to left). The flow before the rim seal and near the blade platform ledges also 

shows dramatic changes. The recirculation at the interface is still similar, but in figure 6-13a, the flow 

near the rotor ledge is stronger, and a part of this continues on into the gap between the rotor-stator 

ledges. The recirculation neat the rotor ledge tip has reversed direction and this flow then gets added to 

the downward leg of the recirculation in the vertical block of the cavity. Differences are also seen at the 

lower end of the recirculation zone, where a large part of the downward leg of the recirculation flow goes 

into the labyrinth seal in figure 6-13a, while in figure 6-13b it is turned away from the labyrinth seal and 

absorbed in the upward leg of the recirculation zone. 

These runs and representative plots show the detailed information that can be generated using the 

coupled codes. The limited amount of comparison with 2–D runs as well as experimental data has shown 

that to this extent, the physics and numerics in the coupled execution procedure has been done properly 

and produces reasonable results. UTRC is in the process of additional, time-accurate data generation from 

the H.P. Rig and this data will be invaluable into validating and anchoring the coupled code execution 

procedure. 

NASA/CR—2005-212716 63
As remarked earlier, the time step size corresponded to a CFL number of around 8. Some testing has 

shown that CFL numbers of up to 12 can be used. The time step size is determined by the blade motion 

criterion, and so offers a limited amount of control on the possible CFL values. Time dependent runs are 

in general expensive, and the present methodology was no exception. The codes were run on two Silicon 

Graphics R10000 processors, and together, the two codes needed approximately 10 minutes of clock time 

per time step. The total number of time steps usually ran about 2000-2200 for periodic solutions. This 

translates a total clock time of about 360 hours. With the advent of faster machines with clock speeds of 

1 GHz and more, these computational times will reduce substantially, making even the time-accurate runs 

a possibility for design simulations. 

6.3 NASA Low-Speed Air Compressor (LSAC) Rig 

A low-speed air compressor facility was built at NASA Glenn Research Center and used to generate 

flow data in a multi-stage machine, for code validation as one of the purposes. The rig has four rotor 

stages, inlet and exit guide vanes and three intermediate stator rows, see figure 6-14. The interstage 

cavities can be altered to some extent to change labyrinth seal shapes etc. to evaluate their effects on the 

cavity flows. A description of the rig and blade geometries etc. is given in [20]. The authors, Wellborn 

and Okiishi, conducted experiments on the rotor 3-4 interstage cavity and rim seals to analyze the 

coupled, time dependent flow fields. The powerstream flow in their configuration had 3 blade rows: rotor 

No. 3, stator No. 3 and rotor No. 4. The interstage cavity is relatively simple in shape, and the labyrinth 

seal had a single tooth. The experimental data includes velocity profiles in the powerstream, rim seals, 

and partway into the cavities. A schematic of the experimental configuration is shown in figure 6-15. 

6.3.1 Geometry and Flow Conditions.—The blade rows have simpler blade ratios: 39 blades on each 

rotor and 52 blades on the stator vane. This allows the use of 3 blades each in the two rotor stages and 

4 blades in the stator stage, with a PI angle of 360/13 degrees. The operational conditions for the rig are: 

960 rpm, flow rate of 12.3 kg/s and a pressure ratio of 1.04 over the entire rig. The disk cavities in the 

compressor sections typically are not cooled with purge flow. The flow in the two disk cavities and the 

labyrinth seal is driven by the pressure differential between the rim seal after the stator blade and the rim 

seal before the stator. 

NASA/CR—2005-212716 64
A multi-domain grid was built for the powerstream with one block in each of the blade-to-blade 

passages. This yielded 3 blocks each in the two rotor stages and four domains in the stator. The grid sizes 

used were 29 by 12 by12 cells in the axial, radial and tangential directions in each block of the rotor 

stages and 40 by 12 by 9 cells in each block of the stator stage. This yielded a total of approximately 

130K cells in the powerstream flow. A 7-domain, 28K cell grid was generated for the secondary flow 

circuit. A solids view of the flow domains showing the powerstream blades and the disk cavities is shown 

in figure 6-16. 

The external flow boundary conditions are needed only in the powerstream for this configuration 

since the cavity flow is entirely driven by the powerstream. At the inlet of the first rotor stage the inlet 

Mach number, swirl conditions and the total pressure and temperature were available. At the rotor exit a 

static pressure with radial balance condition was imposed. 

NASA/CR—2005-212716 65
6.3.2 Results and Discussion.—As for the H.P. rig, the solutions were started with a steady-state run 

for the cavity flow with some reasonable flux conditions at the inlet of the two rim seals. The TURBO 

code was run on the powerstream with walls at the rim seal interface. At a predetermined time, both the 

rim seal interfaces were then allowed to exchange data. The time step was determined by the grid clicking 

frequency at the stator-rotor interfaces. The circumferential grid count in the powerstream passage was 

36 and 16 time steps were used per grid click to yield 576 steps per PI sector. 

A number of different simulation runs were attempted. Initially, the exact rig conditions were used, 

but the simulations tended to diverge relatively quickly. Changes in the time step size as well as the 

number of subiterations per time step in the two codes usually would change the number of time steps 

before code divergence. 

In consultation with NASA personnel, the rpm of the rotor stages was doubled to 1920 rpm, in order 

to achieve higher flow speeds in the powerstream in an attempt to bring the Mach numbers in the 

applicable range for the MS-TURBO code. However, the pressure ratio across the machine was kept as 

before, which should also have been scaled up. With this reduced pressure increase at a given flow rate, 

the powerstream flow rate was much smaller than that which would correspond to the lower pressure rise. 

A run was completed with these conditions, and revealed that the lower flow rate generated low velocities 

near the hub, and in some places produced reverse flow near the hub (consistent with incipient stall). 

Typical velocity and pressure plots from the coupled procedure are shown in figure 6-17a, where the 

cavity section was placed in the wake of the stator blade and 6-17b where the section was placed halfway 

between the stator blade wakes. As seen, the gross features of the cavity flow include recirculation zones 

in both the rim seals as well as in the vertical sections of both cavities. The expected jetting of flow on top 

of the labyrinth tooth is also seen. Although the main flow features were clearly captured in the simulated 

solution, quantitative comparisons with experimental results could not be performed at the flow 

conditions used in these simulations. An additional run at the proper pressure ratio was started but could 

not be completed because of time and resource limitations. 

6.4 Summary 

The results presented in this chapter indicate that the coupled execution procedure can be successfully 

used to handle the powerstream and cavity flow interaction in the time-accurate mode. The validation test 

case, although simple, served to show that the basic physical and numerical arguments used in the 

algorithm development are correct and coded properly. The H.P. rig simulations showed that the coupled 

codes can handle complex shaped cavity and powerstream flows. Results from the coupled codes matched 

with the 2–D simulations and experiments, and the predicted cavity inlet pressure ratio for a zero rim seal 

flow matched well with the UTRC experimental value. One of the concerns during the simulations was 

the relatively small perturbations seen in the cavity flow as a result of the powerstream disturbances. Part 

of the reason may be that the wakes upstream of the rim seal were fixed in space while rotor blades that 

were downstream of the rim seal produced perturbations in the powerstream. These disturbances are small 

compared to those one would get if the upstream blade wakes were moving. These small disturbances 

were then further damped out in the rim seal. Additional experiments in the H.P. rig, with better 

instrumentation for transient measurements are in progress and results from these tests will be valuable in 

further validation of the codes. The LSAC runs were somewhat less successful, and part of the reason 

may have been the extremely slow powerstream flow that had to be handled by MS-TURBO. The 

compressor cavity simulations are more difficult because the success of the coupled codes will depend on 

the accuracy of the powerstream code. Other compressor cavity cases, where the powerstream flows are 

in a more favorable range need to be simulated to ensure that the coupled execution procedure will work 

in the compressor section of a gas turbine engine. 

NASA/CR—2005-212716 66
NASA/CR—2005-212716 67
7. Summary and Recommendations for Future Work 

With the drive for higher power and efficiencies from gas turbine engines, optimization of secondary 

flow systems has become important because of the potential for improvements. For successful 

optimization of the secondary/seals flows, details of the secondary system flow and thermal behavior, and 

its impact on the other flow systems in a gas turbine engine must be known. Present day numerical tools 

offer a way to provide such details, and the current work was focussed on two aspects: 1. To apply the 

present day advanced CFD tools to different real-life secondary flow applications from different original 

equipment manufacturer, to provide feedback and 2. Develop a computational methodology for coupled, 

time-accurate simulations of the powerstream and secondary flow, with focus on the disk-cavity and rim 

seal flows and interaction with the powerstream. 

The preceding chapters of the report have presented the work performed on both areas of focus. Main 

objectives of the present work were completed successfully. The CFD code, SCISEAL, was used on three 

sets of problems. One was the validation study on flow and heat transfer in disk cavities, and the results 

with two different commonly used models were compared with very good correlation with published 

experimental data. 

One of the OEM problems was the T56 engine turbine drum cavities from Allison Engine Company, 

Rolls Royce Aerospace Group (RRAE). Flow and conjugate heat transfer simulations on the inner disk 

cavities were performed and results compared with RRAE design data, again with good correlation. The 

results with conjugate heat transfer in the solid parts (rotors, seal supports) showed that additional thermal 

loads are placed on the cavity coolant flows by the conduction of heat in the solid parts. This additional 

load must be taken into account when designing and optimizing the secondary flow systems in the turbine 

sections. Additional parametric simulations also revealed interesting information on flow behavior in 

response to variations in coolant flow rates and seal clearances, which will be valuable in design process. 

The second OEM problem was the aspirating face seal being developed by GE and Stein Seal 

Company. Initial 2–D CFD simulations provided results that were similar to those obtained from Stein 

Seals' design codes. However, at flow and geometrical conditions away from the design working 

conditions the predictions from the simpler design codes differed significantly. More importantly, the test 

seal showed unacceptable deviations from the design specifications. In this case the 3–D CFD simulations 

played a crucial role in analyzing this seal and coming up with the reasons for the observed behavior. The 

interaction of flow streams from two different parts of the seal (seal dam and bearing) at larger seal 

clearances (which could not be accounted for in the design codes) was identified as the main reason, and a 

fix suggested. The fix was first tested numerically using the 3–D model, and showed dramatic 

improvements in seal loads. The modification was then implemented on the GE test seal, and the seal 

performance was restored to the design specifications. The test seal design is currently being revised and 

additional simulations will be vital in ensuring that the new seal design will behave properly. 

The second major objective, development of a coupled flow simulation capability was achieved by 

using two codes, MS-TURBO and SCISEAL for the powerstream and secondary flows, and coupling 

these with an interface algorithm. A number of issues such as interface placement, data exchange routines 

etc. were successfully resolved, and flux conservation across the interface was ensured. The coupling 

algorithm was completed, and tested on three different problems. The UTRC H.P. rig simulations 

matched the partial experimental data very well and currently the numerical results are being made 

available to UTRC for better instrumentation. Additional data from the rig, as it becomes available, will 

be valuable in validation of the current algorithm as well as others. 

The coupling algorithm developed during this phase was important in linking the two selected codes 

to work together and provide proper physics during the data exchange. Another important aspect of this 

work is the methodology of the coupling itself. A number of issues were sorted out and proper solutions 

worked out. This experience will prove useful if similar coupling algorithms are to be developed for other 

applications. 

NASA/CR—2005-212716 68
7.1 Recommendations for Future Work 

The work presented here is by no means complete and a number of future improvements and 

extensions can be made to further this work and to perhaps bring some of the numerical technology to the 

design stages of turbine secondary flow circuits. Some of the possible areas for future include, in brief: 

1. Additional work on the 2–D simulations of the turbine drum cavities, including the conjugate heat 

transfer in the solid parts could prove valuable in better estimation of the coolant flow heat loads. 

One of the major problems is the lack of data from actual engines for code validation, and work 

in this area will also be very valuable. 

2. The thermal fields in the solid portions of the secondary flow system can be used in a structures 

module to evaluate the thermal stresses and strains in these parts. Although the 2–D 

representation is not truly representative of the complex shaped solid parts in an actual engine, the 

thermal-structures calculation can provide some idea of the displacements and loads on the solid 

parts. 

3. As remarked earlier, the coupled solutions were obtained with two separate codes, as this was the 

best alternative at the time of this project. In principle, the secondary flow code, SCISEAL, can 

be used in the powerstream if the sliding interface treatment were available in SCISEAL, and 

may provide better solution capabilities. Similar remarks may also be true in case of extending 

the powerstream code into the cavity region. Certainly this aspect should be explored further. 

4. The coupled solution methodology should be tried out on more realistic flow cases, on actual 

engine conditions and geometries to evaluate the performance of the codes as well as to 

understand the coupled flow physics. To this end, additional simulations with flow and geometry 

variations on the H.P. rig would be useful, because the numerical solutions could be used for 

better rig designs and instrumentation. 

8. References 

1. Steinetz, B.M., and Hendricks, R.C., “Engine Seal Technology Requirements to Meet NASA’s 

Advanced Subsonic Technology Program Goals,” NASA-TM-106582, AIAA-94-2698, AIAA Joint 

Propulsion Conference, Indianapolis, IN, 1994. 

2. Heidigger, N.J., Hall, E.J., and Denaley, R.A., “Parameterized Study of High-Speed Compressor Seal 

Cavity Flows,” AIAA-96-2807, AIAA 32nd Joint Propulsion Conference, Lake Buena Vista, FL, July 

1996. 

3. Athavale, M.M., Przekwas, A.J., Hendricks, R.C., and Liang, A.D., “SCISEAL-A Three-Dimensional 

CFD Code for Accurate Analyses of Fluid Flows and Forces in Seals,” Conference on Advanced 

Earth-to-Orbit Propulsion Technology, May 1992. 

4. Athavale, M.M., Ho, Y.H., Forry, J.M., Munson, J.H., Hendricks, R.C., and Steinetz, B.M., 

“Simulation of Secondary Flow in Gas Turbine Disc Cavities and Interaction with the Main Flow 

Path,” AIAA-95-2620, 31st AIAA Joint Propulsion Conference, San Diego, CA, July 1995. 

5. Ho, Y.-H., Athavale, M.M., Forry, J.M., Hendricks, R.C., and Steinetz, B.M., “Simulation of 

Secondary Flow in Gas Turbine Disc Cavities, Including Conjugate Heat Transfer,” ASME-96-GT67, ASME International Gas Turbine and Aeroengine Congress and Exhibition, Birmingham, UK, 

June 1996. 

6. Athavale, M.M., Ho, Y.-H., Forry, J.M., and Hendricks, R.C., “Simulation of Powerstream and 

Turbine Disc Cavity Flow Interaction Under Transient Conditions,” AIAA-96-3305; AIAA 32nd Joint 

Propulsion Conference, Lake Buena Vista, FL July 1996. 

7. Hwang, M-F., Shucktis, B., “Advanced Seals for Engine Secondary Flowpath,” AIAA-95-2618, 

AIAA 31st Joint Propulsion Conference, San Diego, CA, July 1995. 

NASA/CR—2005-212716 69
8. Turnquist, N.A., Bagepalli, B.S., Reluzco, G., Wolfe, C.E., Tseng, T.W., McNickle, A.D., Dierkes, 

J,T., Athavale, M.M., and Steinetz, B.M., “Aspirating Seal Modeling and Full Scale Testing,” AIAA97-2631, 33rd AIAA Joint Propulsion Conference, Seattle, WA, July 1997. 

9. Turnquist, N.A., Tseng, T.W., McNickle, A.D., Dierkes, J.T., Athavale, M.M., and Steinetz, B.M., 

“Analysis and Full Scale Testing of an Aspirating Face Seal with Improved Flow Isolation,” AIAA98-3285, AIAA 34th Joint Propulsion Conference, Cleveland, OH, July 1998. 

10. Kilic, M., Gan., X., and Owen, J.M., “Turbulent Flow Between Two Disks Contrarotating at Different 

Speeds,” J. Turbomachinery, Vol. 119, pp. 408-413, 1996. 

11. Gan, X., Kilic, M., and Owen, J.M., “Flow Between Counterrotating Disks,” J. Turbomachinery, Vol. 

117, pp.298-305, 1995. 

12. Northrop, A., and Owen, J.M., “Heat-Transfer Measurements in Rotating Disc Systems, Part 2: The 

Rotating Cavity with a Radial Outflow of Cooling Air,” Int. J. Heat and Fluid Flow, Vol. 9, pp.27-36, 

1988. 

13. Athavale, M.M., Vaidya, N., Hendricks, R.C., and Steinetz, B.M., “A Computational Study of 

Turbulent Flow and Heat Transfer in a Rotating Disc Cavity, 7th International Symposium on 

Transport Phenomena and Dynamics of Rotating Machinery (ISROMAC-7), Honolulu, HI, 1998. 

14. Janus, J.M., “Advanced 3–D CFD Algorithm for Turbomachinery,” Ph.D. Thesis, Department of 

Aerospace Engineering, Mississippi State University, May 1989. 

15. Janus. J.M., and Whitfield, D.L., “Counterrotating Prop-Fan Simulations which Feature a Relative 

Motion Multiblock Grid Decomposition Enabling Arbitrary Time-Steps, AIAA-90-687, AIAA 

Aerospace Sciences Meeting, Reno, NV, 1990. 

16. Chen, J.P., “Unsteady Three-Dimensional Thin-Layer Navier-Stokes Solutions for Turbomachinery 

in Transonic Flows,” Ph.D. Thesis, Department of Aerospace Engineering, Mississippi State 

University, Dec. 1991. 

17. Janus, J.M., and Horstman, H.Z., “Unsteady Flow-Field Simulation of Ducted Prop-fan 

Configurations,” AIAA-92-0521, AIAA Aerospace Sciences Meeting, Reno, NV, 1992. 

18. Athavale, M.M., Przekwas, A.J., Hendricks, R.C, and Steinetz, B.M., “Development of a Coupled, 

Transient Simulations Methodology for Interaction Between Primary and Secondary Flowpaths in 

Gas Turbine Engines,” AIAA-97-2727, AIAA 33rd Joint Propulsion Conference, Seattle, WA, July 

1997. 

19. Athavale, M.M., Przekwas, A.J., Hendricks, R.C., and Steinetz, B.M., “Coupled, Transient 

Simulations of the Interaction Between Power and Secondary Flowpaths in Gas Turbines,” AIAA-98-

3290, AIAA 34th Joint Propulsion Conference, Cleveland, OH, Jul 1998. 

20. Wellborn, S.R., and Okiishi, T.H., “Effects of Shrouded Stator Cavity Flows on Multistage Axial 

Compressor Aerodynamic Performance,” NASA CR 198536, October 1996. 

21. Chien K.Y., “Prediction of Channel and Boundary-Layer Flows with a Low Reynolds Number 

Turbulence Model.” AIAA Journal 20.1(1982): 33-38. 

NASA/CR—2005-212716 70
Appendix A 

Selected Publications 

NASA/CR—2005-212716 71

NASA/CR—2005-212716 73
NASA/CR—2005-212716 74
NASA/CR—2005-212716 75
NASA/CR—2005-212716 76
NASA/CR—2005-212716 77
NASA/CR—2005-212716 78
NASA/CR—2005-212716 79
NASA/CR—2005-212716 80
NASA/CR—2005-212716 81
NASA/CR—2005-212716 82
NASA/CR—2005-212716 83
NASA/CR—2005-212716 84
NASA/CR—2005-212716 85

NASA/CR—2005-212716 87

Presented at the ASME International Gas Turbine and Aeroengine Congress and Exhibition, Birmingham, UK, June 1996. 

96-GT-67
NASA/CR—2005-212716 88
NASA/CR—2005-212716 89
NASA/CR—2005-212716 90
NASA/CR—2005-212716 91

Figure 1. Flow Model for the Allison T-56/501D Turbine Cavities

Isothermal

wall

Isothermal

wall Isothermal

wall

Isothermal

wall

Isothermal

wall

Rotor

(14 239 rpm)

Rotor

(14 239 rpm)

Adiabatic wall

Adiabatic

wall

Main flow 1 Main flow 2

Main flow 3

Main flow 4

Main flow 5

3 Main flow 6

A

B

C

D

6

4

1 5

2

Isothermal

wall

Purge flow

location

Purge flow location

Isothermal

wall

Isothermal

wall

Stator

support

shaded area: conjugate heat transfer

static pressure is specified

at six main flow exits
NASA/CR—2005-212716 92
NASA/CR—2005-212716 93
NASA/CR—2005-212716 94
NASA/CR—2005-212716 95
NASA/CR—2005-212716 96
NASA/CR—2005-212716 97
NASA/CR—2005-212716 98
NASA/CR—2005-212716 99
NASA/CR—2005-212716 100
NASA/CR—2005-212716 101
NASA/CR—2005-212716 102
NASA/CR—2005-212716 103

AIAA 97-2727

Development of a Coupled, Transient Simulation 

Methodology for Interaction Between Primary and 

Secondary Flowpaths in Gas Turbine Engines

Mahesh M. Athavale and Andrzej J. Przekwas

CFD Research Corporation

Huntsville, AL

and

R.C. Hendricks and B. Steinetz

NASAS Lewis Research Center, OH

33rd AIAA/ASME/SAE/ASEE Joint Propulsion 

Conference & Exhibit

July 6–9, 1997 / Seattle, WA 

NASA/CR—2005-212716 105
1

American Institute of Aeronautics and Astronautics

Development of a Coupled, Transient Simulation Methodology for Interaction

Between Primary and Secondary Flowpaths in Gas Turbine Engines

M. M. Athavale* and A.J. Przekwas†

CFD Research Corp., Huntsville, AL

R.C. Hendricks and B.M. Steinetz

NASA Lewis Research Center, Cleveland, OH

ABSTRACT

Optimization of secondary flows in gas turbine engines

promises significant, efficiency increases. Effects of

such optimization on the interaction with the mainpath

flows need to be thoroughly investigated. The inherent

unsteadiness of flow in the mainpath of a multi-stage

engine coupled with reduced secondary flow rates may

lead to local hot gas ingestion in the turbine disc cavities, with adverse effects on component life. A timeaccurate simulation methodology is being developed to

provide detailed knowledge of these flow-fields. The

method involves use of two codes specially developed

for the two flowpaths, coupled through an interface for

data exchange. The multi-stage transient power stream

flow is handled by the MS-TURBO code with a deforming/clicking grid algorithm, while the turbulent flow

heat-transfer in the secondary path is handled by the

SCISEAL code using an unstructured/Cartesian adaptive grid. Results of adaptive grid algorithm on a typical

turbine disc cavity are shown, and a description of the

methodology and current status of the coupling algorithm is presented.

INTRODUCTION

Demand for higher performance from gas turbine

engines has led to higher operating temperatures and

pressures. Adequate cooling of components, especially

in the turbine section, becomes vital under these conditions for acceptable component life. Cooling is usually

achieved by coolant air bled from the compressor section. This air, although necessary, represents a loss, and

is a prime candidate for optimization in the drive to

increase the engine efficiency through secondary flow

management. Under these conflicting requirements, a

detailed knowledge of the flow and heat-transfer processes in the secondary flow systems such as disc cavities, and their interaction with the main path flows

becomes critical at the design stage to ensure adequate

component life. 

Flow and heat transfer processes in rotating cavities

formed between two rotor disks as well as the cavities

formed in rotor-stator disks have received considerable

attention in the past. Early work on the rotating cavity

flow and heat transfer includes experimental [1-3] as

well as analytical [4,5] studies. Work on the rotor-stator

configuration with a rim seal includes experimental

[6,7] and analytical [e.g. Ref. 8] studies done on simplified geometries. Analytical models for the cavity flows

typically used integral flow equations and often did not

include the interaction with mainpath flow. Such models

are inadequate for generating the flow details that may

be needed for future designs.

Computational fluid dynamics (CFD) techniques are

being increasingly used to provide detailed flow-field

information that the analytical methods could not generate. Several studies, dealing with single cavity configuration with simplified geometry are available in the

literature [9-12]. Ko and Rhode [10] and Athavale et.al.

[11,12] presented 2-D axisymmetric flow and heat transfer results in generic turbine disc cavities. The cavities

considered were of the rotor-stator type with a rim seal

and some measure of interaction with a mainpath flow

was provided. Results for different coolant flow rates,

and geometry changes in the rim seal were presented in

these studies.

A recent study by Heidegger, et al. [13] presented simultaneous, 3-D solutions of the powerstream and seal cavity flow interaction in a typical multistage compressor.

Their results show that the leakage flow out of the seal

cavities can affect the powerstream significantly, mainly

by altering the inlet flow near the stator blade root area,

and can potentially affect the performance of the overall

compressor.

_________________

* Group Leader / Research

† Vice President / Research

_________________

Copyright  1997 by the American Institute of Aeronautics and

Astronautics, Inc. All rights reserved.

NASA/CR—2005-212716 106
In an actual engine, the turbine or compressor has multiple disc cavities, with intra-cavity connections and multiple mainpath flow conditions, and the shapes of the 

cavities are far more complicated than those considered 

in these works. More recently, several studies have been 

performed with CFD to take into account the complex 

cavity shapes as well as multiple cavity configurations 

[14-17]. Virr et al. [15] presented a demonstration case 

for a multiple cavity turbine drum configuration. 

Athavale et al. [16] studied the multiply-connected disc 

cavities and interaction with main-path for the UTRC 

Large Scale Rig. Studies on an actual turbine drum 

geometry were presented for the Allison T-56 turbine 

drum inner disc cavities in refs. 14 and 17. The studies 

included the interaction of disc cavity flows with main 

stream, interstage labyrinth seals as well as the conjugate 

heat transfer between the flow and the solid parts (rotor 

and stator disks) of the turbine drum to generate a 

comprehensive flow and heat transfer picture of the turbine section. 

The majority of the CFD work done so far was based on 

the 2-D axisymmetric model and did not account for the 

circumferential variations that are typically present in a 

multi-stage turbine machine. The flow in the mainpath 

contains blade wakes that move with the rotor blades, 

and generate a time-periodic flow-field in the circumferential direction. The blade wakes, as they pass over the 

rim seals at the blade platforms, generate local flow 

variations that may lead to local flow features that may 

differ considerably from the averaged, 2-D solutions. 

Information on these local, time-varying features 

becomes more important during the design stages, as this 

can lead to performance degradation in the compressor 

section, and, perhaps local ingestion of hot mainpath gas 

in turbine disc cavities that will affect component life. 

The present paper describes a new computational methodology that is being developed by NASA to treat the 

complex, 3-D, time-dependent flow field that exists in 

the turbine mainpath flow and couple it with the secondary flow-fields that exist in the sub-platform regions of 

the secondary flow system (See Figure 1). The flow 

characteristics in the two flow streams differ significantly. The mainpath flow is typically compressible, 

transonic, and the geometries involved are usually simpler, mainly annulus base. The sub-platform flows are 

typically low-subsonic, dominated by recirculating, turbulent flows and the domain geometries are complex 

shaped, and usually contain narrow passages relating to 

the seals. In addition, the secondary flow calculations 

also need to consider conjugate heat transfer to the solid 

parts from the flow. In view of these different require 

ments, it was decided to use two different codes for the 

two different flow paths, such that each code was developed especially for one flow path. Thus, each of the 

codes took into account of the requirements of the corresponding flow stream and physics. The following sections give a brief outline of the two codes that are being 

used, a description of the interface algorithm and issues 

that are involved in coupling the codes. Some examples 

of grid-adaptation for the cavity flows using the secondary path code are also presented 

DESCRIPTION OF THE CODES 

The two codes that were selected are the MS-TURBO 

code [18,19] that was developed for the high speed 

mainpath flows in multi-stage turbomachines. The secondary flow will be treated using SCISEAL [20], a code 

developed for the secondary and turbomachinery seal 

flows. Both of the codes were developed under separate 

NASA contracts. A brief description of the codes follows: 

MS-TURBO code [18,19] 

This code uses the 3-D unsteady Euler/N-S form of the 

flow equations. The code was developed for the multirow turbomachinery transient mainpath flows that result 

from the relative motion between successive blade rows. 

Each blade row is separated in radial zones if needed, 

and treated one at a time. The in-core storage requirement is for one blade row at a time only, which reduces 

the working memory size and allows any number of 

blade rows. Information at the blade row boundary 

faces is stored in separate arrays which are used to provide the linking between successive blade rows. The 

flow equations are written in the generalized form and 

the convective fluxes are discretized using the flux-difference splitting methods with third-order accuracy 

achieved using the Osher-Chakravarthy method. The 

first-rate convective fluxes, e.g., at a cell face are written as: 

±

+

−

+ +

+ + + ∆⎥

⎦

⎤ ⎢

⎣

⎡ = + − ∆ + ∆ 2

1 2

1

2

1 2

1 i i i i i i 1 F

~ F~ F~ F~ F~

2

1 F~ (1)

where are the flux differences along right and left running characteristics. Higher order accuracies are 

achieved by adding corrective flux difference terms to 

this expression. The diffusive terms are discretized 

using the central-differencing method. Flux near sharp 

gradients is limited using a Van Leer flux limiting 

scheme. The code used the thin-layer N-S equations 

2

American Institute of Aeronautics and Astronautics NASA/CR—2005-212716 107
where the diffusive terms in the flow-wise direction are 

neglected. The code has an eddy-viscosity based turbulence model to treat turbulent flows. The boundary conditions are set to fit a typical turbomachine problem, and 

are relatively easy to set up. 

Structured grids are used in each of the blade rows. 

When the blade rows move with respect to each other, 

the flow is resolved in time unlike a class of solvers that 

use circumferential averaging. This time resolution is 

important for the present application as was outlined in 

an earlier section. The interface between a moving row 

and a stationary row consists of an interface zone that is 

allowed to deform as one blade row moves past the next. 

A clicking algorithm is used in conjunction with the 

deformation which allows a cell to ‘click’ to the next 

cell after a certain amount of deformation. When the 

grid on the end faces of the deformation zone is known, 

the grid inside the deformation zone is calculated using 

linear interpolation. This ensures reasonably good grid 

quality in the deformation zone at any time during the 

simulations. Grid distortion and clicking implies moving grids, and motion of the grid is included in the time 

derivative of the flow variables through a transformation. The flow domain that will be used for the present 

application will have an interface boundary on the hub 

surface of the blade rows, at the place where the rim seal 

is present. 

SCISEAL code [20,21] 

This code was developed at CFDRC for simulations of 

flows in the secondary flow elements and turbomachinery seals. The released version of the code uses a pressure based finite volume methodology to integrate the 

Navier-Stokes equations on structured, multi-block 

grids. The pressure-based solution scheme allows treatment of slow and recirculating flows. The code has a 

variety of turbulence models including standard k-e and 

Low-Re k-e models, a comprehensive set of boundary 

condition types, and high-order spatial and temporal discretization schemes. A detailed description of the code 

capabilities is given in Ref. 20. 

As remarked earlier, the shapes of the disc cavities are in 

general very complex and contain large cross-sectional 

areas meeting small gap areas e.g. a labyrinth seal. Generation of a structured multiblock grid on such problem 

can become cumbersome and time consuming. In addition, grid refinements/adjustments may be needed to 

resolve flow features that may not be obvious beforehand. Part of the current work is focussed on making 

grid generation and problem setup/running as easy to the 

user as possible. The items that are under consideration are 

1. Adaptation/incorporation of the unstructured/ 

adaptive Cartesian grid solution methodology [21] 

in SCISEAL: Use of unstructured grids in the complex shapes of the disc cavities will simplify the 

grid generation procedure, and facilitate ease of use 

when coupling the flow solutions with conjugate 

heat transfer and structural mechanics in the solid 

parts. Using the triangular cells in 2-D or tetrahedra 

in 3-D is easiest for grid generation, but can lead to 

accuracy loss and more computational time. To 

avoid this, the code can handle a variety of cell/ 

cell-face types including triangle, quads and polygons in 2-D and tetrahedrons, pyramids, bricks, and 

prisms with arbitrary polygonal cross-sections in 3-

D. 

2. Grid Adaptor: To further simplify the grid generation and solution process, the code is coupled with a 

grid adaptor to adapt the grids to the local flow conditions for optimum use of the grids. Starting with a 

baseline coarse grid, the adaptor can be used to add 

cells (by splitting) in areas of high gradients, or 

coarsen it as needed; success of this process 

depends a great deal on the adaptation criterion 

used. At present, the adaptor uses a combined 

‘deviation’ function outlined below as a criterion to 

split cells: 

32

where c1, c2, c3 are the weights specified by the user such 

that c1+c2+c3=1. The deviation function is a vector, and this allows directional splitting of cells as 

against isotropic splitting. The deviation functions such 

as ∇p are generated by SCISEAL at the end of each run 

which are then fed to the adaptor for the next refinement. The grid can be refined or coarsened by specifying a maximum number of cells desired in the adapted 

grid. Coarsening of the grid can be done at best up to the 

original coarse or root grid. 

To illustrate the use of the adaptor and the grid refinement/clustering process, a pair of turbine disc cavities 

from the Allison T-56 engine was considered (see Ref. 

14) The problem definition and the boundary conditions are shown in Figure 2. The startup grid for the 

problem is shown in Figure 3a. This grid has approximately 1200 cells. An earlier structured grid solu3

American Institute of Aeronautics and Astronautics NASA/CR—2005-212716 108

Deviation = C ∇ × ( ) Ω×V + C ∇p + C ∇T (2) 1
4

American Institute of Aeronautics and Astronautics

tions[14] used about 8000 cells for this 2-D geometry.

Using the above defined error vector with c1 and c3 as

the two major contributors, the original grid was successively refined. This involved running SCISEAL on a

new grid to partially converge the solution, obtaining

the error distribution, and then adapting and refining the

grid based on this error distribution. The demonstration

calculation was arbitrarily stopped at a grid size of 5000

cells. The initial and final grids as well as two intermediate grid are shown in Figures 3a-3d. The resulting

temperature and streamline field on the finest grid are

shown in Figure 4a and 4b. These results are in qualitative agreement with the structured grid solutions

obtained in [13]; quantitative comparisons will be done

by integration of flow quantities at selected locations,

using an appropriate post-processor.

As seen in Figures 3a-3d, the grid refinement takes

place in the areas with high gradients of the flow quantities specified in the Error function. Form of this error

function as well as the actual variables used in its definition can change depending on the problem type and

flow physics encountered. The present error function

may not be the best suited for this problem and may

need to be modified to include gradients of other flow

variables, e.g. density, mach number, which are relevant

to compressible flows.

COUPLING INTERFACE METHODOLOGY

During a typical run the two codes will be running on

one or more machines, while an additional set of routines has been developed that will perform the interfacing of the two codes for the coupling of primary and

secondary streams. The overall execution flow chart for

the parallel, coupled execution is shown in Figure 5. As

seen, the interfacing routines need to perform several

functions outlined below:

1. Initial data preparation in each of the two codes for

exchange with the other code. This preparation

includes information of the grids, flow variables

and fluxes.

2. During the solution process, the interface routine

checks for the execution status of each of the codes

to assess whether the two codes are at appropriate

stage to exchange data.

3. Preparation of the data in both codes for interpolation and exchange. This involves storing appropriate type of data from appropriate grid locations in

each of the codes.

4. Interpolation of the data from grids in one code to

the grids in the other code. The grid data are

exchanged and prepared in format needed for interpolation routines The grid topology and type

(structured, unstructured) are taken into account

during the interpolation.

5. Actual exchange of the interface data: this is done

at present through disk file that are written out from

each of the codes. Writing of the data is keyed to

some flag files that indicate whether the earlier data

sets have been used by the other code or not. If not

the interpolation routine waits till the other code is

ready. The data transfer can be done through direct

exchange of data through message passing rather

than through disk files.

6. Check of the data that has been read in each code,

and placing the data from temporary locations to

the appropriate storage locations for use by the code

in the next iteration. This part becomes important

during boundary condition implementation in each

of the codes where the interfaces are placed

The interface itself consists of three separate units: A

set of routines associated with MS-TURBO that assemble the grids and interface variable information, a set

with SCISEAL to perform the same function in

SCISEAL, and a separate code that is used to perform

interpolation of variables/fluxes from one code to the

other in item 4 above, and which is called from both

codes. 

Formulation of Interface Methodology

Several issues needed to be resolved during the formulation of the interfacing routines. Some of these are discussed below, together with the current formulations

that have been used.

1. Differences in code formulations: This is by far the

most important issue one faces when coupling two

codes. Some of the differences to be noted are:

A. The TURBO code is a density-based code with

an implicit, coupled equation solution method.

The SCISEAL code is pressure-based, and

uses a sequential equation solution method. 

B. Cell face convective fluxes in TURBO are

based on the flux-difference splitting method,

while the fluxes in SCISEAL are calculated as

a product of the convection multiplied by an

appropriate flow variable.

C. Subiterations in each of the time step is a necessary requirement for the SCISEAL code due

to the sequential equation method. TURBO

code, on the other hand, can be used to directly

march in time without subiterations. The code,

NASA/CR—2005-212716 109
5

American Institute of Aeronautics and Astronautics

though, has subiterations to improve time accuracy.

 

Given these differences, it is obvious that the data

exchange had to be in such a way as to avoid conflicting demands from the two codes, e.g. insisting that the

cell face fluxes at the interface be calculated independently from the two codes and somehow be reconciled.

It is essential, however, to ensure that the interface flux

conservation is maintained at all times. To achieve this

the current interface formulation does following

exchange:

a. Variable values from SCISEAL at the cell layer

next to the interface are interpolated from the

SCISEAL grid to the TURBO grid. These

variables are used by the TURBO code in a

phantom layer to calculate the fluxes at the

boundary. 

b. The fluxes calculated by the TURBO code then

are interpolated to the SCISEAL grid and

passed back to SCISEAL where they are

imposed directly on the boundary cell faces as

flux boundary conditions. Thus, the fluxes at

the interfaces are always balanced, without any

conflicts.

c. SCISEAL needs face fluxes of the turbulence

quantities k and e when there is flow from the

TURBO code to SCISEAL code. These are

not available from the TURBO code and need

to be calculated locally in SCISEAL. This is

done using the convective fluxes from TURBO

code and extrapolated values of k and e from

SCISEAL.

2. Level of linking of the data sets: This refers to the

level at which the two codes exchange data. One

possibility is at the end of each time-step. This is a

fairly loose coupling and may not be sufficient. At

present the data exchange is planned to be done

after every subiteration during the time stepping

procedure. With a sufficiently large number of subiterations in each code, this coupling is expected to

be sufficiently implicit to provide a stable algorithm

and maintain accuracy.

3. Matching of the execution times: This is a result of

different methodologies and different grid sizes that

are expected to be employed. The readiness of each

code to receive and write data to the other code is

keyed on existence of several flag and data files.

4. Interpolation algorithm: At each data exchange, the

data from one code have to be interpolated to the

grid from the other code, and an accurate, robust

interpolation algorithm is needed. At present the

algorithm in place uses local cell center values and

gradients to interpolate data from one grid to

another. Global flux conservation is not implicit in

the algotrithm and has to be ensured after the fluxes

from TURBO have been interpolated. This procedure will be replaced with an algorithm based on a

conservative scheme where one grid is projected

onto the other and actual area intersections are

found to facilitate interpolation. This algorithm

conserves fluxes implicitly.

PRESENT STATUS AND PLANS 

 At present all of the coding is completed and debugging

runs are in progress. The completed module will be

validated using steady and unsteady data from the

UTRC high-pressure turbine stage rig which is being

tested at UTRC. A schematic of the overall rig is shown

in Figure 6. The arrangement of the rotor and starter

rows and the associated disc cavity and rim and labyrinth seals in the rig is shown in Figure 7. This rig will

provide high quality experimental data for the timetransient interaction of the mainpath and cavity flows.

The interaction will be simulated using the coupled code

and compared with the experiments. Additional cases

for validation will be sought and used as available.

Near future plans also include development of a graphical user interface (GUI) that will provide capabilities of

easy grid generation and problem setup. The GUI will

also provide controls during code execution and provide

the capability of code coupling through direct information exchange rather than through disc files.

SUMMARY

A method to perform parallel, coupled time-accurate

simulations of the secondary and primary flowpaths has

been proposed and currently being developed. The

methodology involves use of two different codes, developed specially for the two different flowstreams, will be

used to treat the flows in the respective streams. The

mainpath flow will be treated using MS-TURBO,which

uses a deforming/clicking grid zone to couple multiple

blade rows and provide time-accurate solutions of the

mainpath. The secondary flow stream will be treated by

SCISEAL, a code developed for the turbulent flow and

heat transfer in this stream. The code has unstructured/

adaptive Cartesian grid capability which will be particularly useful in treatment of complex cavity shapes. A

grid adaptor has been developed for grid refinement/

redistribution for optimal grid usage in the secondary

path. An interpolation algorithm has been developed to

NASA/CR—2005-212716 110
6

American Institute of Aeronautics and Astronautics

couple the two codes during execution and to provide

the coupling between the two flowpaths. This is the first

time such a comprehensive methodology has been proposed for primary and secondary flow coupling, and

with the drive for ever increasing power and efficiency

from modern gas turbine engines, the developed codes

can be expected to become very useful in the design and

performance evaluation process of modern gas turbines.

ACKNOWLEDMENTS

This work was supported under NASA Contract NAS3-

27392, with R.C. Hendricks and B.M. Steinetz as the

Program Monitors. This support is greatly appreciated.

Thanks are due to Drs. Jayent Sabnis and R. Johnston of

UTRC for providing the UTRC rig figures.

REFERENCES

1. Owen, J.M., and Pincombe, J.R., “Velocity Measurements Inside a Rotating Cylindrical Cavity with

a Radial Outflow of Fluid,” J. Fluid Mechanics,

Vol. 99, p. 111, 1980.

2. Gan, X., Kilic, M., and Owen, J.M., “ Flow

Between Counterrotating Disks,” J. Turbomachinery, Vol. 117, pp.298-305, 1995.

3. Northrop, A., and Owen, J.M., “Heat-Transfer Measurements in Rotating Disc Systems, Part 2: The

Rotating Cavity with a Radial Outflow of Cooling

Air,” Int. J. Heat and Fluid Flow, Vol.9, pp.27-36,

1988.

4. Owen, J.M., Pincombe, J.R., and Rogers, R.H.,

“Source-Sink Flow Inside a Rotating Cylindrical

Cavity,” J. Fluid Mechanics, Vol. 156, pp.233-265,

1985.

5. Chew, J.W., and Rogers, R.H., “An Integral Method

for the Calculation of Turbulent Forced Convection

in a Rotating Cavity with Radial Outflow,” Int. J

Heat and Fluid Flow, Vol. 9, pp.37, 1988.

6. Johnson, B.V., Daniels, W.A., Kaweki, E.J., and

Martin, R.J., “Compressor Drum Aerodynamic

Experiments with Coolant Injected at Selected

Locations,” J. Turbomachinery, Vol. 113, pp.272-

280, 1991.

7. Graber, D.J., Daniels, W.A., and Johnson, B.V.,

“Disk Pumping Test,” AFWAL-TR-87-2050, 1987.

8. Chew, J.W., “A Theoretical Study of Ingress for

Shrouded Disc Systems with Radial Outflow,

ASME-89-GT-178, ASME Gas Turbine and

Aeroengine Expo., Toronto, Canada, 1989.

9. Chew, J.W., “ Predictions of Flow in Rotating Disk

Systems Using the k-e Turbulence Model,” ASME88-GT-229, ASME Gas Turbine and Aeroengine

Expo., Amsterdam, The Netherlands, 1988.

10. Ko, S.H., and Rhode, D.L., “Thermal Details in a

Rotor-Stator Cavity at Engine Conditions with a

Mainstream,” ASME-91-GT-275, ASME Gas Turbine and Aeroengine Expo., Orlando, FL, 1991.

11. Athavale, M.M, Przekwas, A.J., and Hendricks,

R.C., “A Numerical Study of the Flow-Field in

Enclosed Turbine Disk-Cavities in Gas Turbine

Engines,” ISROMAC-4, Honolulu, HI, 1992.

12. Przekwas, A.J., Athavale, M.M., and Hendricks,

R.C., “Progress in Advanced Modeling of Turbine

Engine Seal Flows,” AIAA-94-2803, AIAA Joint

Propulsion Conference, Indianapolis, IN, 1994.

13. Heidegger, N.J., Hall, E.J., and Delaney, R.A.,

“Parameterized Study of High-Speed Compressor

Seal Cavity Flow,” AIAA-96-2807, 32nd AIAA

Joint Propulsion Conference, Lake Buena Vista,

FL, 1996.

14. Athavale, M.M., Ho, Y.H., Forry, J.M., Munson,

J.H., Hendricks, R.C., and Steinetz, B.M., “Simulation of Secondary Flow in Gas Turbine Disc Cavities and Interaction with Main Flow Path,” AIAA95-2620, AIAA Joint Propulsion Conference, July

1995, San Diego, CA.

15. Virr, G.P., Chew, J.W., and Coupland, J., “Application of Computational Fluid Dynamics to Turbine

Disc Cavities,” J. Turbomachinery, Vol.116,

pp.701-708, 1994.

16. Athavale M.M., Przekwas, A.J., Hendricks, R.C.,

and Steinetz, B.M., “Numerical Analysis of IntraCavity and Power-Stream Flow Interaction in Multiple Gas-Turbine Disk-Cavities,” ASME-95-GT325, ASME Gas Turbine and Aeroengine Expo.,

Houston, TX, 1995.

17. Ho, Y.H., Athavale, M.M., Forry, J.M., Hendricks,

R.C., and Steinetz, B.M., “Numerical Simulation

of Secondary Flow in Gas Turbine Disc Cavities,

Including Conjugate Heat Transfer,” ASME Paper

96-GT-67, ASME Gas Turbine and Aeroengine

Expo., June 1996, Birmingham, UK.

18. Janus, J.M., and Horstman, H.Z., “Unsteady Flowfield Simulation of Ducted Prop-fan Configurations,” AIAA-92-0521, AIAA Aerospace Sciences

Meeting, Reno, NV, 1992.

19. Janus, J.M., and Whitfield, D.L., “Counterrotating

Prop-Fan Simulations Which Feature a RelativeMotion Multiblock Grid Decomposition Enabling

Arbitrary Time-Steps,” AIAA-90-687, AIAA Aerospace Sciences Meeting, Reno, NV, 1990.

20. Athavale M.M., Przekwas, A.J., Hendricks, R.C.,

and Liang, A., “ SCISEAL-A Three-Dimensional

CFD Code for Accurate Analyses of Fluid Flows

and Forces in Seals,” Conference on Advanced

Earth-to-Orbit Propulsion Technology, May 1992.

NASA/CR—2005-212716 111
7

American Institute of Aeronautics and Astronautics

21. Athavale, M.M., Jiang, Y., and Przekwas, A.J.,

“Application of an Unstructured Grid Solution

Methodology to Turbomachinery Flows,” AIAA95-0174, AIAA Aerospace Sciences Meeting,

Reno, NV, 1995.

Purge/ coolant

flow Interstage labyrinth

seal

Rotor stage

Rotor stage

Stator stage Sliding interface Sliding interface

Interface between primary

and secondary flow

at rim seal

Rotor-stator

disc cavity

Figure 1 Schematic of a Typical Interstage Cavity in a Turbine Section with Interfaces of Interest

NASA/CR—2005-212716 112
8

American Institute of Aeronautics and Astronautics

Figure 2.Flow Domain and Conditions for the Allison T56 Stage 1-2 Disc Cavity with Interstage Labyrinth Seal

NASA/CR—2005-212716 113
9

American Institute of Aeronautics and Astronautics

Figure 3. Computational Grids for the Cavity Problem at Various Levels of Refinement

(a) Root Grid, 1180 Cells (b) Adapted Grid, 2500 Cells

(c) Adapted Grid, 4000 Cells (d) Adapted Grid, 5000 Cells

NASA/CR—2005-212716 114
10

American Institute of Aeronautics and Astronautics

Figure 4. Cavity Solutions on the 5000 Cell Grid

(a) Streamline Plot (Lines in the Mainpath Have Been Supressed). Note Outgoing Flow in Both

Rim Seals

(b) Temperature Field in the Cavity

NASA/CR—2005-212716 115
11

American Institute of Aeronautics and Astronautics

Figure 5. Flowchart for the Coupled Execution of SCISEAL and MS-TVRBO Codes

NASA/CR—2005-212716 116
12

American Institute of Aeronautics and Astronautics

Figure 6. Cross Section of the Rim Seal Ingestion Rig

Figure 7. Details of the Stator and Rotor with Associated Cavity, Rim and Labyrinth Seals

NASA/CR—2005-212716 117

NASA/CR—2005-212716 119
NASA/CR—2005-212716 120
NASA/CR—2005-212716 121
NASA/CR—2005-212716 122
NASA/CR—2005-212716 123
NASA/CR—2005-212716 124
NASA/CR—2005-212716 125

Please see pages 23 to 26 for better representations of the above figures. 
NASA/CR—2005-212716 126

Please see pages 23 to 26 for better representations of the above figures. 
NASA/CR—2005-212716 127
NASA/CR—2005-212716 128
NASA/CR—2005-212716 129
NASA/CR—2005-212716 130
A Computational Study of Turbulent Flow and Heat Transfer 

in Rotating Disc Cavities

Mahesh M Athavale

N. Vaidya

CFD Research Corporation

3325 Triana Blvd.

Huntsville, AL 35805

Robert C. Hendricks

Bruce M. Steinetz

NASA Lewis Research Center

21000 Brookpark Rd.

Cleveland, OH. 44135

ABSTRACT

 The present paper describes the results of a computational study performed to examine turbulent flows in

rotating disc cavities with radial throughflow. The problems considered are: turbulent flow in a contrarotating cavity and turbulent flow and heat transfer in a co-rotating cavity. The standard k-ε model with wall

functions and the low Reynolds number model of Chien have been used to generate a comparative set of

results for specified values of the inlet mass flow rate, rotational Reynolds number, and imposed surface and

inlet temperature distributions. The comparisons provided include radial and angular velocity profiles in the

rotating cavity. The present predictions from the different turbulence models compare well with each other

and also with the available experimental data, thereby, indicating that any of these models may be applied to

simulate rotating cavity flows with reasonable confidence.

Keywords: Rotating cavity flow, Computational Fluid Dynamics, Turbine disc cavity, Turbulence models,

Flow and heat transfer

1. INTRODUCTION

 Disc cavities are present in turbine and compressor sections of a typical gas turbine engine. These may be

formed by a stator-rotor combination, e.g. cavities at the rotor disks and just under the blade platforms, as

well as rotor-rotor combination that exist between two rotor discs, underneath the rotor-stator cavities. In

general the rotating cavities have axial throughflow near the axis (e.g. compressor section) or a radial

throughflow that eventually enters the rotor-stator system for cooling and sealing purposes. Coolant flow

distributions become quite important in the turbine section where the air is used to cool the discs and blades

and thus affects the life of the components. The coolant air flow represents a loss in engine performance, and

represents a quantity for optimization in the drive for better engine performance and efficiency. With

reduced coolant flow rates, detailed and accurate information on flow/heat transfer occurring in the cavities

becomes critical to ensure adequate cooling of the hot components at varying engine operating conditions.

 A large number of studies on flows in stator-rotor systems as well as rotating cavity flows are available in

the literature. A number of early studies deal with experiments on simplified geometry cavity systems and

empirical correlations for flow and heat-transfer processes [1-3].

 Several studies involved development of simplified analytical models for the cavity flows, typically based

on the boundary layer equations at the walls which were linked with an inviscid core in the cavity center [3-

5]. Such techniques were useful and accurate for simplified cavity geometries and flows, however, accuracy

of such models can be expected to suffer when dealing with the complicated shapes of a typical disc cavity

Presented at the Seventh International Symposium on Transport Phenomena and Dynamics of Rotative Machinery( (ISROMAC-7)

February 22-26, 1998, Honolulu, Hawaii, USA 

131

case of the co-rotating cavity, and radial variation of the local Nusselt number in the case of the contraNASA/CR—2005-212716
and when interaction with the powerstream is present.

 Several recent studies have used the computational fluid dynamics (CFD) techniques to the cavity

problems. Treatment of single, simplified systems [7-9] as well as multiple cavities with multiple

intracavity as well as cavity-powerstream interactions [10-12]. These studies involved treatment of the flow

as well as heat transfer and coupled flow and conjugate heat transfer in the gas and the solid components.

These analyses have provided means of achieving detailed flow and heat transfer results and on complex

cavity shapes that were usually not amenable to simplified treatments. Additionally some efforts have also

been made towards working these problem in a time-dependent mode and with accounting for the

interaction with the non-axisymmetric flows generated by the powerstream blades. The list of references

cited here is by no means exhaustive, and represents only a small fraction of the work that has been done on

the cavity problems.

 The success of such computations depends on the employed numerical schemes as well as the physical

models. The flows that occur in the cavities are almost always turbulent, and the selection of the appropriate

turbulence model is one of the important issues when the physical modeling is concerned. A number of

turbulence models have been developed and employed including the simpler models such as BaldwinLomax and more detailed ones based on the turbulence energy and dissipation, for example, the standard kε model, multiple scale k-ε model, and various low Reynolds number models. The focus of the present

paper is to compare results obtained from two different, commonly used models on a prototypical cavity

problem and compare the results with experimental data. The choice of the models that are used and the

appropriateness of any one particular model to a particular problem is always a point of contention. In the

present work, rather than justifying the use of a given model, the focus is on the accuracy of the models that

are commonly and routinely used and are available in a number of general purpose CFD codes, and in

particular in SCISEAL [13]. Undoubtedly, there are other turbulence models available which may prove to

be more “accurate” for the class of problems considered herein.

2. DESCRIPTION OF THE CFD CODE

 The simulations presented here were performed using SCISEAL, an advanced 3-D CFD code developed

under a NASA contract for the fluid flow and force analyses of turbomachinery seals and secondary flow

systems [13]. The current version of the code uses a finite-volume, pressure-based scheme to integrate

Navier-Stokes equations. The code uses a SIMPLEC type of scheme for pressure-velocity coupling and can

treat compressible and incompressible flows. A full set of boundary conditions types and high order spatial

and temporal differencing schemes are available. The code has treatment for: conjugate heat transfer,

rotating and stationary frame, 2-D/3-D modeling, rotordynamics coefficient calculation procedures, and a

variety of turbulence models, including the ones used in the present study, namely standard k-ε model and

the low Reynolds number (low-Re) model of Chien [14].

 Patel et al. [15] evaluated the performance of several low-Re turbulence models for favorable and adverse

pressure gradients in boundary layers. The comparisons presented by them for the skin friction coefficient

Cf in the flat plate boundary layer case showed that the good agreement to data is obtained by the models of

Chien [14] and Wilcox and Rubesin [16], while those of Launder and Sharma [17] and Lam and Bremhorst

[18] under- and overpredicted the value, respectively. For the same case, the Lam and Bremhorst model was

able to capture the turbulent kinetic energy profile relatively very well. The Cf comparisons for favorable

pressure gradient flows involving relaminarization showed that the Launder and Sharma model provided

relatively better predictions. The overall conclusion of the study of Patel et al. [14] was that the above

models provide comparable results and that they all need further refinement to be used with confidence.

 With respect to the ease of implementation of the models for general complicated geometries, the Launder

and Sharma model has the distinct advantage in that the damping functions are not dependent explicitly on

the distance from the wall. However, the dissipation equation in this model has a complicated extra term

that is a function of the square of the second derivative of the velocity.

3. MODEL EQUATIONS

 The turbulence models used in the present study are the high Reynolds number standard k-ε model of

NASA/CR—2005-212716 132
Launder and Spalding and the low Reynolds number model of Chien. The k-ε system of equations in the

Chien model can be expressed as below:

where the dissipation ε is related to the quantity by

with εo being the value of ε at the wall.

 The production term P is defined as

where the turbulent stress tensor is modeled using Bousinessq’s eddy viscosity concept as

 The eddy viscosity is defined as

 The expressions used in the Chien model for the empirical damping functions fμ, f1 and f2, and the values

of the empirical constants are summarized in Table 1.

Table 1. Damping Functions and Empirical Constants Used in Chien’s

Low Reynolds Number Turbulence Model

 The nondimensional parameters ReT, Ry and y+ are defined as:

 In the above relations, ‘y’ is the distance to the wall and Uτ is the friction velocity. The boundary condition

for k at the no-slip wall is k = 0. The boundary condition for ε is built into the -equation by the inclusion

of the factor εo. The effective thermal conductivity in the case of heat transfer problems is calculated as

where CP is the specific heat, Pr and Prt are the laminar and turbulent Prandtl numbers with Prt taken as

equal to 0.9. 

fμ cε1 1.35

f1 1 cε2 1.80

f2 cμ 0.09

εo σk 1.0

E σε 1.3

∇⋅ ρVK = ∇⋅ μ + μt

σk ∇k +P– ρε

∇⋅ ρVε = ∇⋅ μ + μt

σε ∇ε + ε

k f1Cε1P–f2Cε2ρε + E

ε ̃

ε = εo + ε

P = τt : ∇V

τt = μt ∇V + ∇V T – 2

3μt ∇ ⋅ V I – 23ρkI

μt = fμCμρk2

ε

1–e– 0.0115y+

1 – 0.22 e– ReT / 6 2

2 μ k /y2

– 2 μ ε

ρ y2 e– 0.5 y+

ReT = ρk2

εμ , Ry = ρk1/2y

μ , y+ = ρUτyμ

ε ̃

λeff = CP

μ

Pr + μt

Prt

NASA/CR—2005-212716 133
4. DESCRIPTION OF THE FLOW PROBLEMS

 The two different types of rotating cavity configuration considered in the present study are: 

1. Flow in a cavity formed between two contra-rotating discs with a radial throughflow. This type of

flow has been studied in Refs. 16-18 and disc cavities of this type may be encountered in turbine

engines with proposed contra-rotating turbine sections [19-21].

2. Flow and heat transfer in a co-rotating cavity [22], which is a much more common type of disc

cavity and that which is usually found in the turbine section where the radial throughflow is used

as coolant and sealing air for the rotor-stator type of disc cavities. 

 Following are details of the geometry, flow conditions and results of the simulations.

1. CONTRA-ROTATING CAVITY FLOW

A. Geometry and flow conditions

 A schematic of this cavity is shown in Figure 1 and is based on the description provided in [19,20]. Using

the notation and details provided in [20], the geometry is described by the following aspect ratios: the gap

ratio G = s/b = 0.12, the shroud-clearance ratio Gc = sc/b = 0.016, and the inner to outer radius ratio a/b =

0.128, where the outer radius b of the cavity is 391 mm. The rotational speeds of the left and right disc are

equal and opposite (Γ = -1). The important flow parameters in this problem are the nondimensional inlet

mass flow rate Cw and the rotational Reynolds number Reφ. In the experiments in [19], the throughflow

entered through an axial hole in the left disc and then was introduced in the cavity radially through a pair of

rotating gauze tubes of 50 mm radius to provide a nearly uniform radial velocity distribution. Experimental

measurements include those of the radial and tangential velocity components along the axial direction at

several radial stations. 

Fig. 1. Schematic diagram of the contra-rotating cavity.

 The computational domain considered in the present study is enclosed by the two discs in the axial

direction, and by the shroud at the outer radius and the gauze tube at the inner radius (Figure 1). A 2-D grid

with 95 cells in the radial direction and 67 cells in the axial direction was generated with appropriate

clustering near the walls to yield proper near-wall distances needed in the low-Re model. For the standard

k-ε model with the wall functions the grid size was reduced to 47 cells in the axial and 88 cells in the radial

direction. The reduction is needed to keep the near wall distance large enough to be acceptable for the wall

Shroud

Egress

Rotating gauze tubes for

radial purge flow inlet

Ωr

Reφ = ρΩ b2/μ

Cw = m / bμ

Γ = Ωr/Ωl

b

a

Sc

S

x

Ωl r

NASA/CR—2005-212716 134
functions. A limited amount of grid-independence study was performed to ensure that the solutions were

nearly insensitive to further grid refinement. It should be noted here that the 95 x 67 grid resolution

employed here is comparable in the radial direction and nearly half as small in the axial direction as the 113

x 65 grid employed in [20] wherein the symmetry of the flow about the axial midplane was invoked. Thus,

the present results will serve as a good indicator of the minimum resolution required for reasonable accuracy

in the computed results. 

B. Computational Results and Discussion 

 Two-dimensional, axi-symmetric, swirling flow simulations were carried out at three different values of the

nondimensional flow rate Cw = 2310, 6320 and 9280, corresponding to Reφ = 6.66 x 105, 7.08 x 105

, and

6.84 x 105, respectively. In each case, the disc speed was fixed to achieve the appropriate value of Reφ.

 Air at 297 K was used as the working fluid, and at the low speeds involved, it was assumed to be

incompressible and to have constant properties. Central differencing scheme with 10% damping was used

for the convective fluxes. The simulations were carried out using the standard k-ε model with wall functions

and the low-Re model of Chien.

 An inlet boundary was specified at the gauze tube (i.e. at inner radius a) with a uniform radial velocity to

yield the correct volume flow rate (see Figure 1). The disc and shroud walls were specified as no-slip walls

with the appropriate angular velocities. At the clearance between the shrouds where the flow exits, a

constant pressure boundary was specified.

 The computed streamlines using the low-Re model of Chien are shown in Figure 2 for Cw = 2310 and

6320. As was described in [20], the following characteristic regions exist in this problem: a source region

extending radially outward from the inlet where the radial velocity is everywhere positive, an axial midplane

core region with radial inflow, boundary layers on the discs with radial outflow, and contra-rotating cells

between the boundary layers and the core. With reference to Figure 4, the present predictions for Cw = 2310

show the existence of two secondary contra-rotating cells close to the inlet apart from the two primary ones

near the core. Though the rotations of the secondary and primary cells on the same side of the axial

midplane were found to be in opposite direction, these cells are sufficiently separated radially by a region in

which rotational effects are nearly absent. At the higher value of Cw = 6320, the source region penetrates

comparatively farther into the core, and only a primary system of contra-rotating cells can be discerned.

Fig. 2. Computed streamlines for contra-rotating cavity.

 Experimental data [20] for this case are in terms of axial distribution of tangential and radial velocity

components at different radial locations. Although the simulations were carried out at three different coolant

flow rates Cw, results for one flow rate are shown here, specifically, for Cw = 6320. The radial and tangential

velocity distributions at r/b = 0.6, 0.7, 0.8 and 0.85 are plotted in Figures 3-6. The velocities have been 

a. Cw = 2310 b. Cw = 6320

NASA/CR—2005-212716 135
Fig. 3. Radial and tangential velocity distributions at r/b = 0.6.

Fig. 4. Radial and tangential velocity distribution at r/b = 0.7.

Fig. 5. Radial and tangential velocity distribution at r/b = 0.8.

Fig. 6. Radial and tangential velocity distribution at r/b = 0.85.

-1

-0.5

0

0.5

1

Expt. [20]

Chien

Std. k-e

Vt / Omega* r

-0.02

0

0.02

0.04

0.06

0.08

0.1

0.12

0.14

Expt. [20]

Chien

Std. k-e V

r / Omega* r

Vr / Ω rVφ / Ω r

-0.02

0

0.02

0.04

0.06

0.08

0.1

0.12

Expt. [20]

Chien

Std. k-e V

r / Omega* r

-1

-0.5

0

0.5

1

Expt. [20]

Chien

Std. k-e

V

t/ Omega*r

Vr / Ω rVφ / Ω r

-1

-0.5

0

0.5

1

0 02 04 06 08 1

Expt. [20]

Chien

Std. k-e Vt / Omega*r

-0.02

0

0.02

0.04

0.06

0.08

0.1

0.12

Expt. [20]

Chien

V

Std. k-e r / Omega*r

Vr / Ω r

Vφ / Ω r

-0.04

-0.02

0

0.02

0.04

0.06

0.08

0.1

0 0.2 0.4 0.6 0.8 1

Expt. [20]

Chien

Std. k-e V

r / Omega*r

Axial Distance x/L

-1

-0.5

0

0.5

1

1.5

0 0.2 0.4 0.6 0.8 1

Expt. [20]

Chien

Std. k-e

V

t / Omega*r

Axial Distance x/L

Vr / Ω r

Vφ / Ω r

x/S x/S

NASA/CR—2005-212716 136
scaled with the local wall tangential velocity which is equal to Ωr. Data points from measurements are

represented by symbols in these figures and the curves represent results from the simulations using the two

different turbulent models. In general the agreement between the two model predictions and with the data is

good to very good in the case of the tangential velocities at all radial locations. Radial velocity plots also

compare well with the experimental data near the shroud. At the lower radius, the experimental data shows

higher radial velocities near the downstream disc wall (x/S = 1). This is a result of the axial entry of the

coolant flow in the experimental setup. Although not shown here, this skewness in the radial velocity plots

gets more pronounced with increasing coolant flow rates.

2. CO-ROTATING CAVITY FLOW AND HEAT TRANSFER

A. Geometry and flow conditions

 The co-rotating cavity was formed with two discs joined at the outer radius with a single shroud [22]. The

configuration is similar to that of the contra-rotating cavity but with the discs now rotating in the same

direction, (Figure 1) i.e., Γ = 1. The values of the geometric ratios are the same as those used in [22]: gap

ratio G = 0.138, radius ratio a/b = 0.104, with the outer radius b = 428 mm. Coolant flow was introduced into

the cavity through an axial hole in the ‘upstream’ disk and the flow exited through the shroud holes. The

discs were instrumented for temperature and wall heat flux measurements and had embedded electric heaters

for heat addition. Radial distribution of wall heat fluxes were measured at different coolant flow rates,

rotational speeds and wall temperature distributions. Three different wall temperature distributions were

considered: constant, decreasing with radius, and increasing with radius.

 The flow domain considered is similar in shape to the one shown earlier for the contra-rotating cavity (see

Figure 1). The coolant was assumed to enter the cavity radially. The grid used for the low Reynolds number

model had 84 cells in the axial direction and 136 in the radial direction. The grid for the standard k-ε model

had 52 and 94 cells in the axial and radial directions, respectively. As before, this reduction was needed to

keep the near wall distances in the proper y+ range. This reduction is also one of the reasons why the

standard k-ε model becomes economical and hence attractive in complex simulations. 

B. Computational Results and Discussion

 The working fluid was taken as air. As before, central differencing scheme with 10% damping was used for

the convective fluxes. Boundary condition at the inlet (inner radius) was a specified inlet flow rate

corresponding to specified values of Cw and inlet temperature (see Figure 1). A constant pressure exit

boundary was specified at the slot in the shroud. In actuality this is a set of discrete holes; in the 2-d axisymmetric simulations a slot with equivalent flow area was used. No-slip walls with appropriate angular

velocities were assumed on disc and shroud surfaces. 

 Two choices were available for the specification of the energy equation boundary conditions at the disc

walls: 1) use the measured temperature profiles as imposed boundary values, and 2) model the disc as a solid

piece with embedded heaters and solve a conjugate heat transfer problem that would give both the flux and

temperatures as solutions. In the absence of sufficient details of heater construction and operation, the first

choice was used in the computations as was also done in [22]. Three different types of profiles were

generated in the experiments: radially constant, increasing and decreasing temperatures. A typical set of

these profiles is shown in Figure 7. These experimental temperature profiles were imposed on the upstream

and downstream disc walls for the energy equation.

 For a constant nondimensional coolant flow rate Cw of 7000, and a rotational Reynolds number Reφ of

2.x106, parametric simulations were performed by imposing the wall temperatures as described above. The

computed temperature distributions were post-processed to obtain the radial variation of the local Nusselt

number on the ‘upstream’ and ‘downstream’ discs.

 The predicted radial Nusselt number profiles from the two turbulence models are compared with the

experimental data [22] in Figures 8a-c. In these plots the computed values are represented by curves and the

data by symbols. Again, the comparison with the experimental data both in terms of the general trend as

well as local magnitudes is good. As was found in the experiments [22], the present predictions show that

the local Nusselt number becomes negative (Figure 8b) as the shroud is approached. Since the imposed

surface temperature is greater than the inlet temperature, i.e., TS - TI > 0, a negative value of Nu, by

NASA/CR—2005-212716 137
definition, implies that the local heat flux is negative, i.e., heat is transferred from the fluid to the wall. This

indicates that the heat gained by the fluid from the disc near the inlet region is returned to the disc at larger

radius. As in the previous case, predictions from the two turbulence models show little differences. These

comparisons provide confidence in the utilization of the standard k-ε model with a relatively much coarser

grid to simulate cavity heat transfer problems.

Fig. 7. Imposed disc surface temperature distributions. 

Fig. 8. Radial variation of local Nusselt number for various imposed disc wall temperatures.

a. Downstream wall b. Upstream wall

0

100

200

300

400

500

600

700

800

0 0.2 0.4 0.6 0.8 1

Expt. [22]

Low-Re, Chien

Std. k-e

Wall Nusselt No.

Radial Distance, r/R

-400

-200

0

200

400

600

0 0.2 0.4 0.6 0.8 1

Expt. [22]

Low-RE, Chien

Std. k-e

Wall Nusselt No.

Radial Distance, r/R

-200

0

200

400

600

800

0 0.2 0.4 0.6 0.8 1

Expt. [22]

Low-RE, Chien

Std. k-e

Local Nusselt No.

Radial Distance, r/R

case a. Radially Increasing Imposed Wall

Temperature 

case b. Radially Decreasing Imposed Wall

Temperature 

case c. Radially Uniform Imposed Wall

Temperature 

NASA/CR—2005-212716 138
SUMMARY

 An advanced 3-D CFD code, SCISEAL was applied to simulate flow and heat transfer in two different

rotating cavity configurations. The turbulence models employed were the standard k-ε model with wall

functions and the low Reynolds number model of Chien. This exercise was undertaken to validate the

numerics and physical models in SCISEAL by comparison with experiments, and to assess the performance

of the turbulence models on this class of problems. It is recognized that there are several other turbulence

models that are available and are being used. One can claim that these have better predictive capabilities;

however, the intent of this work was to test the accuracy of the more widely used models that were available

in the code. 

 The model predictions were compared with the available data for velocity profiles in the contra-rotating

cavity configuration, and for local Nusselt number in the co-rotating cavity configuration. The overall results

show that both models produce results that are very similar to each other, and show a good correlation with

the experimental data. The good agreement between the standard k-ε model and the low-Re model of Chien

is possibly due to the fairly high Reynolds numbers investigated in the present study. As expected, however,

the models show discrepancies near the walls where the viscous effects become predominant and where the

Chien model is expected to be more accurate. The correlation of the results with the experimental data

serves to validate the accuracy of the SCISEAL predictions. Based on this set of results, both models

employed in this study are seen to do an adequate job of dealing with the flows in disc cavities provided

proper care is taken in the mesh generation and boundary condition specifications to match the restrictions

and range of validity of each model.

REFERENCES

1. Owen, J.M., Air-Cooled Gas Turbine Discs: A Review of Recent Research, Int. J. Heat and Fluid Flow,

Vol. 9, No. 4 (1988) pp.354-365.

2. Bayley, F.J., Owen, J.M., The Fluid Dynamics of a Shrouded Disk System With a Radial Outflow of

Coolant, J. Engg.for Power (1970) pp.335-341.

3. Phadke, U.P., Owen, J.M., An Investigation of Ingress for an Air-Cooled Shrouded Rotating Disk

System With Radial-Clearance Seals, J. Engg. for Power, Vol. 105 (1983) pp. 178-183.

4. Chew, J.W., and Rogers, R.H., An Integral Method for the Calculation of Turbulent Forced Convection

in a Rotating Cavity with Radial Outflow, Int. J. Heat and Fluid Flow, Vol.9 (1988) pp.37.

5. Chew, J.W., A Theoretical Study of Ingress for Shrouded Disc Systems with Radial Outflow, ASME-89-

GT-178, ASME Gas Turbine and Aeroengine Expo, Toronto, Canada (1989).

6. Johnson, B.V, Daniels, W.A., Kaweki, E.J., and Martin, R.J., Compressor Drum Aerodynamic

Experiments and Analysis With Coolant Injected at Selected Locations, J. Turbomachinery, Vol.113

(1991) pp.272-280.

7. Chew, J.W., Predictions of Flow in Rotating Disk Systems Using the k-e Turbulence Model, ASME-88-

GT-229, ASME Gas Turbine and Aeroengine Expo, Amsterdam, The Netherlands (1988).

8. Ko, S.H., and Rhode, D.L., Thermal Details in a Rotor-Stator Cavity at Engine Conditions with a

Mainstream, ASME-91-GT-275, ASME Gas Turbine and Aeroengine Expo, Orlando, FL (1991).

9. Athavale, M.M., Przekwas, A.J., Hendricks, R.C., A Numerical Study of the Flow-FIeld in Enclosed

Turbine Disk-Cavities in Gas Turbine Engines, ISROMAC-4, Honolulu, HI (1992).

10. Virr, G.P., Chew, J.W., and Coupland, J., Application of Computational Fluid Dynamics to Turbine

Disk Cavities, J. Turbomachinery, Vol. 116 (1994) pp.701-708.

11. Athavale, M.M., Przekwas, A.J., Hendricks, R.C., and Steinetz, B.M., Numerical Analysis of IntraCavity and Power-Stream Flow Interaction in Multiple Gas-Turbine Disk-Cavities, ASME-95-325,

ASME Gas Turbine and Aeroengine Expo, Houston, TX (1995).

12. Ho, Y.H., Athavale, M.M., Przekwas, A.J., Forry, J.M., and Steinetz, B.M., Numerical Simulation of

Secondary Flow Gas Turbine Disc Cavities Including Conjugate Heat Transfer, ASME-96-67, ASME

Gas Turbine and Aeroengine Expo, Birmingham, U.K. (1996).

13. Athavale, M.M., Przekwas, A.J., Hendricks, R.C., and Liang, A., SCISEAL- A Three-Dimensional

CFD Code for Accurate Analyses of Fluid Flow and Forces in Seals, Proceedings of the Advanced

E.T.O. Technology, NASA MSFC, Huntsville, AL (1994).

NASA/CR—2005-212716 139
14. Chien, K.-Y., Predictions of Channel and Boundary Layer Flows with a Low-Reynolds-Number

Turbulence Model, AIAA Journal, Vol. 20 (1982) pp. 33-38.

15. Patel, V.C., Rodi, W., and Scheurer, G., Turbulence Models for Near-Wall and Low-Reynolds Number

Flows: A Review, AIAA Journal, Vol. 23 (1984) pp. 1308-1319.

16. Wilcox, D.C. and Rubesin, W.M., Progress in Turbulence Modeling for Complex Flow Fields Including

Effects of Compressibility, NASA Tech. Paper 1517 (1980).

17. Launder, B.E. and Sharma, B.I., “Application of the Energy-Dissipation Model of Turbulence to the

Calculation of Flow Near a Spinning Disc,” Letters in Heat and Mass Transfer, Vol. 1 (1974) pp. 131-

138.

18. Lam, C.K.G. and Bremhorst, K.A., Modified Form of the k-ε Model for Predicting Wall Turbulence,

Journal of Fluids Engineering, Vol. 103 (1981) pp. 456-460.

19. Gan, X. Kilic, M., and Owen, J.M., Superposed FLow Between Two Discs Contrarotating at

Differential Speeds, Int. J. Head and Fluid Flow, Vol. 15, No. 6 (1994) pp.438-446.

20. Gan, X., Kilic, M., and Owen, J.M., Flow Between Contrarotating Disks, J. Turbomachinery, Vol. 117

(1995) pp. 298,305. 

21. Kilic, M., Gan., X., and Owen, J.M., Turbulent Flow Between Two Disks Contrarotating at Different

Speeds, J. Turbomachinery, Vol. 118 (1996) pp. 408-413.

22. Northrop, A., and Owen, J.M., Heat Transfer Measurements in Rotating Disc Systems, Part 2: The

Rotating Cavity with a Radial Outflow of Cooling Air, Int. J. Heat and Fluid Flow, Vol.9, No.1 (1988)

pp. 27-36.

NOMENCLATURE

A = Area, m2

b = outer radius of cavity, m

Cw = Nondimensional coolant flow, q/νR

K = turbulence kinetic energy, m2/s2

k = thermal conductivity, w/m-K

L = Characteristic length, m

Nu = Nusselt Number, qr/TS-TI)

q = heat flux, w/m2

R = outer radius

Reφ = Rotational Reynolds number, ΩR2/ν

r = radial coordinate, m

T = Temperature, K

x,y,z = Cartesian coordinate directions, distances, m

y+ = Nondimensional friction distance

Greek

ρ = density, kg/m3

ν = kinematic viscosity, m2/s

μ = dynamic viscosity, Pa-S

ω = disc rotation speed, rad/s

τ = stress, Pa

ε = turbulence dissipation rate

Subscripts

S = wall

I = inlet

NASA/CR—2005-212716 140
Appendix B 

An Algorithm for Interpolation Between Computational 

Interfaces With Arbitrary Grid Matching 

NASA/CR—2005-212716 141

B.1 Introduction 

A robust interpolation algorithm was developed for the date exchange between SCISEAC and 

MS-TURBO across interfaces. The interpolation algorithm had to treat interfaces that had only partial 

overlaps, stressed grids on cylindrical surfaces, structured and unstructured grid topologies and different 

grid face counts in the two interfacing grids. The interpolation methodology that was developed and used 

here involves the following steps: 

(1) Interpolate values of the current variable from face centers to nodes on side 1 of the interface; 

(2) Use the nodal values of the current variable to calculate the gradient of the current variable at face 

centers on side 1 of the interface; and 

(3) Use values and gradients of the current variable at face centers on side 1 of the interface to 

calculate values of the current variable at face centers on side 2 of the interface. 

Details of each of these steps are given in the following subsections. 

B.2 Methods 

B.2.1 ‘Face center’ values vs. ‘cell center’ values.—The interface interpolation method described 

below is a discussion on how to interpolate from face center values on one side of the interface to face 

center values on the other side. This method therefore necessarily assumes that the face center values for a 

given variable are available along the interface. In the practical implementation of the algorithm, the CFD 

code which supplies the face center values can use as accurate a technique as desired for the extrapolation 

of this values from the cell center. 

B.2.2 Necessary input for the interpolation algorithm.—The complete list of information necessary 

for interpolation from a local interface boundary to a remote boundary is as follows: 

(1) Face-node list describing the nodes which surround a given face along the interface [local]. 

(2) Total number of faces, total number of nodes, and a list containing the number of nodes per face 

(the current algorithm is designed for the most general case of polynodal faces) [local]. 

(3) Nodal coordinates (x,y,z) along the interface [local] 

(4) “ordered_nodes” parameter which is true if the nodes are arranged sequentially (clockwise or 

counter-clockwise) around the face centroid in the face-node list or false if the nodes are not 

ordered [local] 

(5) Face centroids (sctr, yctr, zctr) for the remote interface [remote]. 

(6) Face center data (u,v,w,P,etc) [local] 

The code is capable of handling faces with any number of nodes and it is not necessary to order the 

face node list in any particular format. 

B.2.3 Face Normal Vectors.—The interpolation algorithm requires a normal vector for each face. 

This normal vector is uniquely defined for a three noded ‘tri’ face, but for the general case of polynodal 

faces, all of the nodes will not necessarily lie in the same plane. In this case, the face normal is calculated 

by averaging the ‘sub-face’ normals (figure B.1). The sub-face normals are calculated by taking a cross 

product of the vectors from the face centroid to two face nodes. The expression for the average face 

normal is therefore given by: 

sub face i

sub face i num nodes per face

i face normal n

n

_ ,

_ , _ _ _

1 _ v

v

∑

=

⎯⎯ → ⎯⎯⎯⎯ = (B.1) 

where 

_ , , , 1 x sub face i = ctr −node i ctr −node i+ n r r v v v (B.2) 

NASA/CR—2005-212716 143
This method for computing the face normals requires that the nodes be oriented in order (clock-wise 

or counter-clockwise) around the face centroid. If the nodes are not in order, the current doing will order 

the nodes before calculating the face normal. This ordering process is done as follows. A normalized 

baseline vector is established from the face centroid to the first node in the node list. 

The dot product between this baseline vector and the normalized vectors from the face center to all 

other nodes is evaluated. The node which yields the maximum dot product is established as the second 

node in the list. 

Next, the dot product and cross product between the second vector and all remaining center to node 

vectors are evaluated. In addition, the dot product of the first sub-face normal and the calculated cross 

products from the remaining nodes is evaluated. The node which produces the maximum dot product with 

the second node vector AND has a positive dot product between the old sub-face and the evaluated cross 

products is assigned to be the next node in the list. 

This process is repeated for the remaining nodes. 

The second dot product evaluation between the sub-face normal and the other subface normals is 

designed to be consistent for face geometries like that shown in figure B.2d. On this face, the dot product 

between the normalized vectors from the center to node 3 and the center to node 4 is larger than the dot 

product between the normalized vectors from the center to node 3 and the center to node 5. However, 

node 5 is the next node seen as this face is traversed clockwise. The constraint that the dot product 

between the previous sub-face normal and the current sub-face normal must be positive causes node 5 to 

be chosen as the next node rather than node 4. 

NASA/CR—2005-212716 144
B.2.4 Cell center to nodal interpolation.—The cell center to nodal interpolation is accomplished 

using Laplacian interpolation algorithms described in references 1 (three-dimensional) and 

2 (two-dimensional). The Laplacaian interpolation algorithm is designed to be 100 percent accurate in the 

interpolation of linear function form face centers to interior nodes. In summary, a nodal value, qo, can be 

obtained as a weighted average of cell center values (q1,q2,..qn) (figure B.3): 

∑

∑

=

= = n

i

i

n

i

i i

w

w q

q

1

1

0 (B.3) 

With the following definitions: 

( )( )( ) 0 0 0 w x x y y z z i = λ x i − + λ y i − + λ z i − (B.4) 

NASA/CR—2005-212716 145
[ ( ) ( )( )]

D

R I I I R I I I I R I I I I x yy zz yz y xy zz xz yz z xy yz yy xz

x

− − + − − − λ

2

 (B.5) 

[ ( ) ( ) ( )]

D

R I I I I R I I I R I I I I x xy zz xz yz y xx zz xz z xx yz xy xz

y

− + − − + − λ =

2

 (B.6) 

[ ( )( ) ( )]

D

R I I I I R I I I I R I I I x xy yz yy xz y xx yz xy xz z xx yy xy

z

2 − − + − − − λ = (B.7) 

( ) ( )( ) xx yy zz yz xy xy zz xz yz xz xy yz yy xz D = I I I − I − I I I − I I + I I I − I I 2 (B.8) 

∑( ) =

= −

n

i

x i R x x

1

0 (B.9) 

∑( ) =

= −

n

i

y i R y y

1

0 (B.10) 

∑( ) =

= −

n

i

z i R z z

1

0 (B.11) 

∑( ) =

= −

n

i

xx i I x x

1

2

0 (B.12) 

∑( ) =

= −

n

i

yy i I y y

1

2

0 (B.13) 

∑( ) =

= −

n

i

zz i I z z

1

2

0 (B.14) 

∑( )( ) =

= − −

n

i

xy i i I x x y y

1

0 0 (B.15) 

∑( )( ) =

= −

n

i

xz i i I x x z z

1

0 0 (B.16) 

∑( )( ) =

= − −

n

i

yz i i I y y z z

1

0 0 (B.17) 

NASA/CR—2005-212716 146
In practice this three-dimensional interpolation method fails under certain conditions such as when 

the contributing faces are coplanar. The current coding checks for these failure conditions and reverts to 

the two-dimensional Laplacian interpolation in the case of failure of the three-dimensional algorithm. 

Likewise the two-dimensional Laplacian fails under certain conditions (such as when the contributing 

faces are colinear). In this case the coding reverts to a distance based weighting: 

i node

i

r

w

−>

= 1 (B.18) 

where ri->nodeis the distance between face center I and the node 0. This means that for linear function, the 

interpolation (or extrapolation) of values to the boundary nodes will not necessarily be exact. 

The one difficulty with reverting form the 3–D Laplacian to the 2–D Laplacian interpolation is the 

choice of which two directions (i.e., x and y?; x and z?; y and z?) to use in the 2–D Laplacian. This 

problem is avoided in the current coding by projecting all face center cartesian coordinates (x, y, z) into 

the average normal plane (s1,s2,n) of the node (figure B.4): 

∑

= ⎯⎯ → ⎯⎯⎯⎯

⎯⎯ → ⎯⎯⎯⎯

⎯⎯ → ⎯⎯⎯⎯ =

num faces per node i

j

j face normal

j face normal

i node normal

_ _ _ ,

1

_

_

_ (B.19) 

Therefore the 3–D Laplacian uses the coordinates s1,s2, and n while the 2–D Laplacian uses only 

s1 and s2. It should be noted that the in-lane unit vectors s1 and s2 can be chosen arbitrarily using the node 

as the origin and the node_normal vector as the normal for the projection plane. 

NASA/CR—2005-212716 147
B.2.5 Calculation of Gradients.—Nodal values are used to calculate the face center gradient based 

upon a version of Green’s Theorem. Green’s theorem is given by 

V

q nd

q

∫ e

Γ

Γ

∇ =

r

 (B.20) 

where qe is the value of q on the boundary (Γ), n

r is the normal along the boundary, and V is the cell 

volume. On a 2–D face, eq. (B.20) becomes 

V

q n A

q

number of edges

∑ e i e i e i

= ∇ = i 1

, , ,

r

 (B.21) 

where e n

r is the normal vector at each edge, Ae is the edge ‘area’ (actually edge length), and V is the face 

‘volume’ (face area figure B.5). 

subface i

number of subfaces

V V ,

i 1

∑

=

= (B.22) 

,1 ,1 ,2 x 

2

1

subface ctr node ctr node V r r = − −

r r (B.23) 

( )( )2

2 1

2 ,1 2 1 A x x y y e = − + − (B.24) 

( ) 1 2 2

1 e,1 q q

q = + (B.25) 

The face volume is calculated by summing all of the sub-face volumes (eq. (B.22)), and each sub-face 

volume is calculated as one-half of the magnitude of the cross product between the vectors from the face 

center to the first node and the face center to the first node and the face center to the second node 

(eq. (B.23)). Note that the quantity qe is simply the average of the value of q at the two nodes of a given 

edge (eq. (B.25)). The variable “edge_normal” in the interpolation coding is the quantity: 

NASA/CR—2005-212716 148
V

n A

edge normal e,i e,i _

r

= (B.26) 

All of the above calculations are with the assumptions that the face lies in a 2–D plane. For the 

current algorithm, this is not necessarily the case. Therefore, before calculating the gradient, all nodes are 

projected in the average face normal plane (defined by the face center as the origin and the face_normal 

vector). 

B.2.6 Interpolation across the interface.—Interpolation across the interface is achieved by first 

finding the closest face centroid on the local interface to the remote face. Next, the remote face centroid is 

projected into the face-normal plane of the closest local centroid. Finally, a value of the variable of 

interest is assigned to the remote face based upon the value of the local face, the projected distance form 

the local face centroid to the opposing face centroid, and the gradient of the variable on the local face 

(figure B.6 and eq. (B.27)): 

{ } 1 2 q q a s , s remote = local + ∇ • ∆ ∆ (B.27) 

B.5 References 

1. Frink N.T. (1994). “Recent Progress Toward a Three-Dimensional Unstructured Navier-Stokes Flow 

Solver,” Presented at the 32nd Aerospace Sciences Meeting in Reno, Nevada. AIAA Paper No. 94-

0061. 

2. Rausch R.D., Vatina J.T., Yang H.T.Y. (1991). “Spatial Adaptation procedures on Unstructured 

meshes for Accurate Unsteady Aerodynamic Flow Computation,” Presented at the 

AIAA/ASME/ASCE/AHS/ASC 32nd Structures, Structural Dynamics, and materials Conference, 

Baltimore, Maryland. AIAA paper No. 91-1106. 

NASA/CR—2005-212716 149

Appendix C 

Users’ Manual for Coupled, Time-Accurate, Three-Dimensional 

Computations of Primary-Secondary Flow Interactions 

at Rim Seals With SCISEAL-MS–TURBO Codes 

Mahesh M. Athavale 

CFD Research Corporation 

Huntsville, Alabama 35805 

Summary 

 This document provides a methodology for coupling of two different flow solvers for flows across a 

moving interface, such as occurs in rotating machinery. Herein the coupling is between a flow code called 

MS-TURBO that will represent the behavior of the primary flow and SCISEAL that will be used to 

represent the secondary flow fields. For a typical turbomachine the primary flow is bounded between the 

casing or shrouds and the blade-vane platforms and drums. The secondary stream is sub-platform and 

represents the fluid that provides cooling and stability for seals, bearings, and cavities as well as the 

drums and several components of the primary flow, such as turbine blades. While coupling of the codes is 

described elsewhere in published documents, this report describes the basics for operating the codes 

singularly or as coupled codes and as such assumes that these codes are already part of the user’s 

computational system. 

Athavale, Mahesh M.: Users’ Manual for Coupled, Time-Accurate, Three-Dimensional Computations 

of Primary-Secondary Flow Interactions at Rim Seals With SCISEAL-MS⎯TURBO Codes. 

NASA/CR⎯2004-212983/VOL1, 2004. 

Available from the NASA Center for Aerospace Information. 

NASA/CR—2005-212716 151
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

Final Contractor Report

Unclassified

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

November 2005

NASA CR—2005-212716

CFDRC 4117/1

E–14240

Cost Center 2250000013

NAS3–27392

153

Analysis of Coupled Seals, Secondary and Powerstream Flow Fields in Aircraft

and Aerospace Turbomachines

M.M. Athavale, Y.H. Ho, and A.J. Przekwas

Turbomachine seals; Secondary flow; Design; Numerical analysis

Unclassified -Unlimited

Subject Categories: 01, 07, 20, and 37 Distribution: Nonstandard

CFD Research Corporation

215 Wynn Drive

Huntsville, Alabama 35805

Project Manager, Robert C. Hendricks, Research and Technology Directorate, NASA Glenn Research Center,

organization code R, 216–977–7507.

Higher power, high efficiency gas turbine engines require optimization of the seals and secondary flow systems as well as

their impact on the powerstream. This work focuses on two aspects: 1. To apply the present day CFD tools (SCISEAL) to

different real-life secondary flow applications from different original equipment manufacturers (OEM’s) to provide

feedback data and 2. Develop a computational methodology for coupled time-accurate simulation of the powerstream and

secondary flow with emphasis on the interaction between the disk-cavity and rim seals flows with the powerstream

(SCISEAL-MS-TURBO). One OEM simulation was of the Allision Engine Company T-56 turbine drum cavities including

conjugate heat transfer with good agreement with data and provided design feedback information. Another was the GE

aspirating seal where the 3-D CFD simulations played a major role in analysis and modification of that seal configuration.

The second major objective, development of a coupled flow simulation capability was achieved by using two codes

MS-TURBO for the powerstream and SCISEAL for the secondary flows with an interface coupling algorithm. The coupled

code was tested against data from three differed configurations: 1. bladeless-rotor-stator-cavity turbine test rig, 2. UTRC

high pressure turbine test rig, and, 3. the NASA Low-Speed-Air Compressor rig (LSAC) with results and limitations

discussed herein.