Analysis of a turbine rim seal cavity via 3D-CFD using conjugated heat transfer approach ZERELLI, N. - Heat Transfer Department MTU Aero Engines, 80995 Munich, Germany University: ISAE Institut Supérieur de l Aéronautique et de l Espace Toulouse, France The presented work makes a contribution to the European research effort MAGPI (main annulus gas path interactions). It deals with the computational fluid dynamics analysis of a turbine rim seal cavity. It is investigated through 3D-CFD (computational fluid dynamics) methods via the conjugated heat transfer approach. The flow and thermal behavior, is analyzed for different cavity configurations, i.e. with varying geometry and coolant mass flow rates. The different designs are evaluated on the basis of a thermal efficiency. Nomenclature Abbreviations 3D = three-dimensional CFD = computational fluid dynamics CHT = conjugated heat transfer, this corresponds to the baseline configuration SST = shear stress transport MAGPI = main annulus gas path interactions Subscripts _da = MAGPI model with modified cooling inlet position _seg = MAGPI model with leakage slot integration Variables C w = non-dimensional mass flow rate m& = mass flow rate, kg/s µ = dynamic viscosity, Pa. s P = power, W R = gas constant, with R=287 J/kg/K r = radius, m T hot = turbine inlet total temperature = 443 K T cool = mass-averaged cooling flow temperature = 287 K T wall = area-weighted static temperature on the cavity walls, K T total = total temperature, K v = fluid velocity υ = kinematic viscosity, m²/s Non-dimensional Numbers Re Φ = Rotational Reynolds Number y+ = n+ = non-dimensional wall distance 1
I I. Introduction N modern aero-engines approximately twenty percent of the of the main annulus gas is bled off to feed secondary air systems such as cooling and sealing flows. Their optimization is considered one of the most promising techniques to increase global engine efficiency. The accurate prediction of the stator, rotor and disc metal temperature is crucial for the reliable layout of such air systems. Above this, it allows the accurate calculation of thermal dilatation, gap clearance evolution, thermal stresses and hence component lifetime. The present study deals with a turbine stator well, providing the clearance between rotor discs and stator support ring. A cooling flow is bled off constantly into this inter-disc cavity in order to prevent hot gas ingress from the main gas path air and, hence, extensive disc heating. The flow behavior and thermal properties of rim seal cavities are characterized by complex flows due to interaction with the main annulus gas. In order to investigate this region a 3D CFD model of a 2-stage turbine, including its stator well, the metal rotor discs and the stator foot, is generated. It corresponds to a turbine test rig at the University of Sussex, in terms of geometry and operating conditions. The conjugated-heat-transfer (CHT) approach takes into account the thermal interaction between the fluid domain and the solid components. The method is a very promising way to achieve physically more coherent modeling of heat transfer in cavities, where interactions between heat convection in the fluid domain and heat conduction in the solid domain are expected to be noteworthy. At the interface between main annulus gas and secondary air systems, where strong temperature gradients occur, a conjugated approach is essential: it allows a fully modeled heat exchange along the solid-fluid interface, rather than fixed boundary conditions, and thus yields more reliable results. The project 1 is carried out in the framework of the European research effort MAGPI (main annulus gas path interactions), where the present study focuses on the first work-package Effects of Cooling System/Main Annulus Gas Interaction Rotor Heat Transfer. The MAGPI cavity is studied in different configurations: the first is the baseline configuration, which corresponds to the standard test rig and for which data validation will be performed in the near future. In a second setup, the cooling flow inlet is displaced further upstream, towards the upstream cavity wall. Finally, another configuration, which corresponds to a possible test rig setup, introduces a leakage slot in the upstream cavity that accounts for actual leakage flows in a typical turbine. Each setup is simulated at two coolant mass flow rates such that different cavity ingress/egress situations are analyzed: with a cooling mass flow of 30g/s the cavity is not fully sealed and annulus gas enters, ingress occurs; with a cooling mass flow of 60g/s, the cavity is sealed against hot gas ingress. The analysis focuses on the flow patterns as well as the heat transfer in the cavity. A non-dimensional parameter is defined in order to evaluate the cooling efficiency for the different cavity designs. The study is classified as a CFD - pre-study, the measurements from the corresponding test rig data are scheduled to be available in the near future. The numerical data will then undergo a validation process, which will include the matching of the boundary conditions to the test conditions. Previous analyses of other turbine and compressor rim seal cavities at MTU - Heat Transfer Department have shown that the employed solver allows the reliable simulation of rim seal cavities: this comprises the flow behavior and the heat transfer characteristics. The simulation of a turbine rather than a compressor rim seal usually yields physically more coherent results since typical for compressor operation phenomena such as stall and surge do not occur. It is hence concluded that a numerical investigation of the present turbine rim seal cavity is reasonable and expected to show coherent results during the validation process. 1 Cf. Ref [1] 2
II. Baseline MAGPI cavity A. Test Rig & Operating point The stator well test rig is located at the Thermo-Fluid Mechanics Research Centre at the University of Sussex 2. It comprises a two-stage axial flow turbine enclosed in an annular channel through which the mainstream gas flows. Each turbine stage includes 39 nozzle guide vanes and 78 rotor blades with a twisted profile and hence fully threedimensional flow. Figure 1 summarizes the geometry and inlet boundary conditions of the test section at the design point, with a rotational speed of 10630 rpm (1113,73 rad/s). In most aero-engines the stator foot is equipped with a honeycomb structure, since it presents an efficient means to further increase the sealing quality: UZKAN and LIPSTEIN (1986) 3 have shown that ingestion of external flow into the stator well can be lowered significantly by using honeycombs on the stator foot. The honeycombs are not included on the rig. However, in order to account for the beneficial effect on the sealing performance of the labyrinth seal, the distance between the stator foot and the labyrinth teeth is lowered (from 0.4mm originally to 0.3mm) for both, the test rig and the CFD model. B. Mesh and Physical Model The numerical model (cf. Figure 2) consists of a fluid and solid domain. The first includes two stator rows as well as both rotors and the cavity; the latter is composed of the rotor discs, stator foot and drive arm. The interface between rotating and stationary parts is the stage-interface frame-change/mixing model and performs circumferential averaging. The turbine model is axial-symmetric, strong circumferential variations are not expected since the combustion chamber is not part of the test rig. 2 Cf. Ref. [2] 3 Cf. Ref. [3] 3
The meshes of the fluid domain are based on multi-block structured grids with hexagonal-volumes and have an overall size of nearly 3 million cells. It is refined in the regions of strong adverse pressure gradients, such as the cavity walls and the labyrinth region. The solid mesh is considerably coarser since only the energy conservation equation is solved in that region. With respect to the materials used for the solid region, the exact material data of the test rig is included in the numerical model: the stationary parts (nozzle guide vanes and the stator shrouds) are made of stainless steel, Type 304; the rotating parts (rotor discs and the drive arm) are made of titanium alloy, TiAl6V4. The Ansys-CFX solver is used for the simulations, all run in steady state. The physical model of the fluid domain is the total energy heat transfer model including the viscous term: it corresponds to a coupled solver, modeling the transport of enthalpy including kinetic effects. The heat transfer modes taken into account in the fluid domain are conduction, convection, turbulent mixing and viscous work. The turbulence model chosen for all the simulations is SST (shear stress transport) with automatic near-wall treatment: it is well adapted for meshes with important grid spacing variations and a flow field characterized by adverse pressure gradient conditions 4. The solid domain is solved via the Thermal Energy model, which accounts for heat conduction. Radiation is negligible and hence not included. C. Overview of cavity physics The most important effects associated to the flow behavior inside a cavity are presented briefly. Figure 3 shows the main types of flow that are typically identified in rim seal cavities. In a turbine the pressure decreases across a stage, and hence there is an important pressure differential between the upstream trench of the cavity and its downstream trench. This constantly entrains a mass flow across the labyrinth which depends on the magnitude of the pressure difference between the upstream and downstream chamber and on the seal gap height (i.e. the distance between labyrinth teeth and stator foot). Hot gas from the main gas path therefore ingresses the upstream chamber predominantly and exits through the downstream trench. This can only be prevented by providing a sealing mass flow in the upstream chamber. The design criterion for engines is to inject a higher mass flow than would be required to reach exact sealing. Apart from the hot gas ingestion and the coolant injection, a third zone is distinguished in the cavity: the core zone forms due to the so-called pumping effect of the rotor disc. The fluid is entrained by the disc and centrifugally accelerated. The flow over the disc becomes turbulent for rotational Reynolds Numbers above 3x10 5, where Re Φ describes the ratio of kinetic to viscous forces in a rotating environment. In the laminar flow regime, the nondimensional entrained mass flow rate amounts 5 : (1) 4 Cf. Ref. [6] 5 Cf. Ref. [4] 4
Where the rotational Reynolds-Number is defined as follows: The contribution of each type of zone (ingress/cooling/core flow) to the flow field in the upstream cavity, depends on the operating point. The shaft rotating speed defines the pressure loss across a stage - hence the pressure difference between upstream and downstream cavity chamber. The cooling mass flow rate is the second parameter and acts directly on the amount of hot gas ingress. (2) D. Results a) Flow field and mass flow rates The flow patterns and total pressure profiles of the MAGPI cavity are shown in Figure 4. It is found that the main recirculation zones form as expected: - at 30g/s cooling flow injection nearly 20g/s of hot main gas path air enter the cavity. The central flow in the upstream cavity is the air that is pumped by the rotor-1, where the fluid is accelerated along the disc. The cooling flow injected at the cavity bottom can clearly be distinguished in the flow pattern which indicates low mixing between the core zone and the coolant. The downstream cavity is dominated entirely by the pumped flow which entrains a single recirculation zone. - at 60g/s cooling flow injection the cavity is definitely sealed, in fact 10g/s exit the upstream cavity. Hence, there are only two important zones to be identified in the upstream chamber: the pumped flow and the coolant recirculation. Similarly to the 30g/s case the mixing between those zones is rather poor and the flow situation in the downstream chamber remains unchanged. b) Temperature distribution The study of the thermal behavior reveals that the previous assessment of the flow patterns is confirmed: the mixing is poor and the injected cooling flow circulates in the lower chamber. This is due to the pressure differential across the labyrinth which forces the coolant to either pass through the labyrinth immediately or remain close to the cavity bottom, the exception being the coolant close to the rotor disc. The centrifugal acceleration forces a certain amount of coolant to the upper cavity part, which is observed for both cooling mass flow rates. 5
Another important finding is that a significant amount of thermal energy is transmitted from the main gas path into the cavity through the metal components. This is observed very clearly at 60g/s cooling flow, since no hot gas ingress occurs and thermal energy transport through the metal is the only heat source. The heat conducted through the metal components has an important impact on the temperature in both chambers, where the upstream side is affected predominantly. The thermal energy is transmitted from the upstream chamber through the stator foot to the cooler downstream chamber at both coolant mass flow rates. The cavity s thermal behavior is mainly triggered by the presence of the pump effect and the associated recirculation zones. Natural convection is negligible compared to the centrifugal effects. In conclusion, the MAGPI model reacts as expected, and the results are physically coherent. III. Cavity with displaced cooling-inlet A. Model Definition In the baseline MAGPI cavity configuration, the axis of the cooling flow inlet tube is at 18mm distance to the upstream cavity wall. The tube diameter is 3mm at the intersection of cavity floor and inlet tube. In the modified configuration, the inlet of the cooling flow is displaced by 8mm (axis-baseline to axis-modified) which results in a distance between the displaced cooling flow axis and the upstream cavity wall of nearly 4mm (cf. Figure 6). This design modification is studied since a stronger reaction of the coolant to the centrifugal pick-up is considered to be beneficial to the overall heat transfer characteristics. The flow injection angle remains the same as in the previous configuration (with the coolant entering the cavity normal to the cavity floor and with the momentum of the inlet nozzle, rotating at operating speed). B. Results a) Flow field and mass flow rates The velocity profiles at 30g/s and 60g/s change markedly (cf. Figure 7 and Figure 8). The coolant which enters the cavity at proximity to the cavity wall immediately enters the region of pumped flow. Through the centrifugal acceleration the flow is propelled further along the disc and reaches a maximum velocity of 40m/s at 30g/s (compared to 20m/s in the baseline MAGPI-model) and 75m/s at 60g/s (compared to 40m/s in the baseline MAGPImodel). 6
Another important aspect of the modified flow field is the fact that, independently of the cooling mass flow rate, there are no longer two separate zones distinguishing the core flow and the coolant flow. Both zones merge into each other, creating one main vortex in the upstream cavity. The downstream cavity chamber remains nearly unaffected. The overall increase in velocity has a significant effect on the ingress/egress situation of the cavity: the total pressure in the stationary frame is higher due to the acceleration of the coolant along the rotor1-disc. This in turn decreases the pressure differential between the main gas path and the upstream trench and hence the pressure differential between the chambers, as can be seen in Figure 9-LH. Therefore, less leakage flow passes through the labyrinth, thus less hot gas ingestion occurs at the upstream trench (cf. Figure 9 RH). b) Temperature distribution & Wall heat flux The modified flow paths in the upstream cavity strongly influence the total temperature distribution (cf. Figure 10). Immediate mixture between the cooling and core flow occurs throughout the entire upstream chamber, other than in the standard configuration where two separate zones remain. This causes the average fluid total temperature to drop significantly, particularly in the upstream cavity. This is due to two effects: first, with the displaced cooling inlet the majority of the coolant remains in the upstream chamber rather than directly passing through the labyrinth. Secondly, the total pressure increase in the upstream chamber results in a lower pressure difference across the labyrinth, which causes less hot gas to be ingested. 7
In the 60g/s simulation (cf. Figure 11), the fluid temperature drop is more equilibrated between upstream and downstream chamber. In this configuration the cavity is sealed, no hot gas ingestion occurs, and the coolant fills the upstream chamber entirely and also passes through the labyrinth causing the temperature to drop in both chambers significantly. The modification of the drive-arm cooling inlet position implies fundamental changes in the flow field which have a very beneficial effect on hot gas ingestion. Both, fluid and solid temperatures, decrease significantly: at lower mass flow rates the impact on the fluid temperature is concentrated in the upstream chamber, where at higher cooling mass flow injection the fluid temperature reduction is more equilibrated between both chambers. In the solid components the impact of the varying mass flow rate is less noticeable. A general design aim for such cavities can thus be extracted as follows: in order to benefit from the pump effect to the maximum extent it is most desirable to position the cooling flow inlet as close as possible to the rotor disc. IV. Cavity with integrated leakage slot A. Model Definition In the baseline MAGPI cavity configuration, no purge flow enters the cavity. This corresponds to one of several configurations in which the tests will be run on the actual turbine test rig. In the upstream cavity, however, so-called leakage slots can be opened which results in a small flow from the back-plate. Hence, with the integration of a leakage slot, additional test configurations are modeled. The geometry of the segmented slots, i.e. one vertical slot per sector, is illustrated in Figure 12. The slot length is 6mm, the slot height is 12mm and the width is 0.3mm. The boundary condition assigned to the new segmented slot part is an inlet with a specific mass flow rate at 300K. The mass flow rate entering the domain corresponds to a quarter of the cooling flow. B. Results The analysis of the flow patterns and fluid temperatures needs to be performed carefully, since two effects are overlapping: first, the cool second air inlet in the upstream cavity presents an additional heat sink. Secondly, integrating the leakage flow adds an airflow to the overall injected mass flow which automatically reduces the amount of hot gas ingestion when compared to the baseline model. 8
a) Flow field and mass flow rates The velocity profiles change slightly in the 30g/s simulation. Very locally, where the 7.5g/s purge flow enters, the velocity increases (cf. Figure 13Erreur! Source du renvoi introuvable.). This small zone does not present an important obstruction to the main flow paths in the cavity and is accorded an immediate centrifugal acceleration along the rotor1-disc. Generally, the flow paths are not affected compared to the baseline cavity; however, kinetic energy of the core zone is lost partially as the leakage flow enters normal direction the cavity wall. As expected, no effect is noticed in the downstream chamber. The velocity profiles at 60g/s cooling mass flow are shown in Figure 14. It is observed that the purge-flow bubble, forming in proximity to the segmented slot, eventually fully merges with the core zone. This influences the interaction between the core zone and the cooling flow recirculation, which is easily observed through the velocity vectors at the interface of the two zones. Their exchange increases the radial momentum of the core zone, entrained by the pump-effect. This momentum is conserved and, other than in the 30g/s case, results in an overall velocity increase of the core zone also near the stator foot. b) Temperature distribution The thermal analysis of the MAGPI_seg model shows that, even at small mass flow rate, the influence of the purge flow on the fluid total temperature is noteworthy in the upstream chamber. This occurs mainly near the cavity wall, the average fluid total temperature reduction amounts 3.7K. However, it needs to be taken into consideration that the leakage slot air enters the cavity at cooling flow temperature. 9
At 60g/s the higher mass flow rate of cool air dominates the overall cavity temperature. Better mixing between the zones core flow and coolant flow also has an important impact on the fluid total temperature. The injection of additional coolant presents a second zone of cooling flow and therefore lowers the fluid temperature. V. Thermal efficiency In order to compare the cavity configurations on an objective basis, a thermal efficiency is defined. The cooling performance is evaluated for five surfaces defining the cavity walls: two rotating walls, the labyrinth region and two stationary walls. The inlet and cooling flow temperatures serve as a reference and the efficiency is defined as described in equation (3). T hot = turbine inlet total temperature = 443 K T cool = mass-averaged cooling flow temperature = 287 K T wall = area-weighted static temperature on the cavity walls The results for both mass flow rates are shown in Figure 18. It is found that particularly for the sections of highest temperature, i.e. rotor 1 disc (Rot1) and the stator upstream side (Sta1), the modification of the cooling inlet position is noteworthy. When comparing the MAGPI_seg model with the other configurations it needs to be taken into account that the absolute amount of injected flow is higher than in the other configurations; the effect on the thermal efficiency is most noticeably in the 60g/s case. (3) In conclusion, the modification of the cooling flow inlet position shows the maximum rise in performance: not only does it yield the highest increase in thermal efficiency, but it also has an advantageous effect on the hot gas ingestion. 10
VI. Conclusion A general conclusion is derived from the sensitivity study concerning geometry modifications to the baseline cavity: any measure which increases the level of mixing of the two main zones, i.e. core and coolant flow, is to be encouraged. It allows the best-possible use of the very costly cooling flow and therefore increases the performance of the cooling system. The two design modifications studied in this project have proven to act as motors entraining the mixture, where the cooling flow inlet displacement has the maximum effect. As explained previously, this is due to the most efficient exploitation of the pump effect, a natural source of kinetic energy. In terms of future exploitability of the numerical results, the simulations have yielded physically coherent results which can be used for a validation study. The use of the conjugated heat transfer approach has shown to not only be possible, even for a rather large CFD model, but very promising when it comes to investigating the details of the fluid temperature in the cavity. Acknowledgments The author thanks the Heat Transfer Department of MTU AeroEngines in Munich, where this work was conducted, for the continuous support and gratefully acknowledges the permission for publication. Reports, Theses, and Individual Papers References 1 ZERELLI, N. Fluid Flow and Heat Transfer in Rim Seal Cavities a conjugated 3D-CFD study (2008) Master of Science Thesis: Germany, Munich ² STEFANIS, V. Annual Report: Turbine Stator Well Heat Transfer (2003) University of Sussex, Thermo-Fluid Mechanics Research Centre ³ UZKAN, T.; LIPSTEIN, N.J. Effects of honeycomb-shaped walls on the flow regime between a rotating disk and a stationary Wall (1986) ASME International Gas Turbine Conference & Exhibit: Germany, Düsseldorf 4 OWEN J.M.; ROGERS R.H. Flow and Heat Transfer in Rotating-Disc Systems Volume 1 Rotor-Stator Systems (1989) : Taunton, England: Research Studies Press Ltd. 5 MAGPI-Documentation: MAGPI, Part B, 12 July 2005 6 Validation Report: CFX-VAL10/0602: MENTER, F.R. (2002) 11