Numerical Investigation on the Heat Transfer and Flow Characteristics of a Leading Edge Impingement Cooling System for Low Pressure Turbine Vanes

Transcription

1 Numerical Investigation on the Heat Transfer and Flow Characteristics of a Leading Edge Impingement Cooling System for Low Pressure Turbine Vanes Pedro de la Calzada and Jose Javier Alvarez Abstract Deep insight on the flow physics driving the surface heat transfer phenomena in impingement cooling configurations is possible by the use of CFD simulations. Under the current work the main flow features affecting the heat transfer in a particular impingement cooling configuration used in a low pressure turbine vane were investigated by a numerical simulation. The particular impingement cooling system is representative of the one used for cooling the leading edge of a contra-rotating Power Turbine (PT) vane representative of a small turboshaft engine. Existing experimental results were used for code validation. Comparison of results is performed in terms of heat transfer surface distributions, impingement rows stagnation line local distributions and streamwise distributions along planes over the impingement stagnation points. The CFD results present local deviations in the heat transfer compared with experimental results although the surface averaged value is well matched. Additional flow features having a significant effect on the obtained surface heat transfer results were investigated. In particular the generation of impingement and ejection stagnation regions and their effect in the local maxima and minima observed on the surface heat transfer is analyzed. I. INTRODUCTION The increasing operating temperature of modern turbines usually requires internal cooling of the airfoils if acceptable metal temperature levels to fulfill integrity and life targets are to be achieved. In particular the Leading Edge (LE) area of the airfoils is critical since it is typically subject to the highest external heat transfer load hence requiring high cooling flow rates to reduce airfoil metal temperature. Although convective cooling through serpentine passages running all along the leading edge area (with or without ribs) is a proven technology for managing the heat load, more complex configurations are needed to further improve the system efficiency. Impingement cooling systems by arrays of jet holes offer some advantages as reduced cooling flow consumption and localized effect. Furthermore, the use of a tube plenum to feed the jet holes also Manuscript received February, P. de la Calzada is with Industria de Turbopropulsores SA, ITP, San Fernando de Henares, Madrid, Spain (phone: , fax: , mail: pedro.delacalzada@itp.es). Also Assistant Professor at Ocean Engineering and Naval Architecture School, UPM, Madrid, Spain. JJ. Alvarez is with Industria de Turbopropulsores SA, ITP, San Fernando de Henares, Madrid, Spain improves the uniformity of the surface heat transfer compared to serpentine passages of decreasing cooling potential. Therefore impingement cooling through rows of jets is usually the preferred design solution for cooling the LE of turbine vanes in modern engines. In order to develop the technology that allow the optimisation of impingement cooling systems in highly heat loaded turbines a deep insight in the physics associated to the flow phenomena involved in such processes is needed. Such technology has been based traditionally in analytical developments and experimental investigations which have allowed the development of correlations and tools to dimension those cooling systems. These designs have usually required experimental validations where real geometry and flow details are present. However it is the recent use of CFD simulations which has allowed a deeper insight in the main parameters playing key roles in the target surface heat transfer hence allowing the refinement of correlations and tools to further optimise these systems and decrease the level of risks associated to such solutions. Simple impingement cooling systems on flat plates are possible to be investigated by analytical models which allow to describe a limited number of main parameters affecting the surface heat transfer as revisited by Holley and Langston [1]. Additional deeper insight in the role played by the different parameters affecting the impingement cooling configuration is possible by experimental approaches. Extensive experimental investigations of cooling systems with impingement on flat surfaces have been conducted for many years. However, few have been performed on jets impinging on concave surface geometry representative of airfoil leading edges. The experimental investigations were initially focused on configurations to be used for correlating averaged heat transfer values in concave surfaces as done by Chupp [2] and Hrycak [3]. The interest was extended, with the help of more accurate experimental methods, to surface distribution of heat transfer around impingement regions. In particular, the work by De la Calzada and Alvarez [4] offers detailed surface heat transfer measurements on a representative engine geometry of a contrarotating PT vane hence allowing the validation of CFD simulations in real engine configurations. With regards to the numerical simulations some investigations have been performed recently although very few ISBN:

2 allow detail comparison with corresponding experimental data. The works of Jia et al [5], Ibrahim et al [6] and Rama and Prassad [7], among others, presented detail numerical results and comparison with experimental data with some insight on the special impingement flow features driving the main heat transfer characteristics on concave surfaces. Taslim and Khanicheh [8] offer more surface averaged heat transfer experimental and numerical results on airfoil leading edge geometry including more effects as gill film and showerhead holes. In the present work, the impingement cooling system for the LE of a contra-rotating PT vane was investigated numerically and the results were compared with the available experimental data. Comparison of results is performed in terms of heat transfer surface distributions, impingement rows stagnation line local distributions and streamwise distributions along planes over the impingement stagnation points. Additionally the numerical flow solution has been used to discuss in detail the main flow features affecting the surface heat transfer in this particular case. II. REAL ENGINE GEOMETRY The investigation presented in this paper was carried out with the aim at validating the CFD tools to be used in the real engine design, hence focusing on the particular geometry and conditions required in the real case. As presented by De La Calzada and Alvarez [4] the engine geometry model, corresponding to a contra-rotating PT vane of a small turboshaft, is shown in Fig.1. Coolant is fed into the insert tube through the open top end and then flows through two staggered rows of holes, impinging on the vane LE area as it can be seen on the zoomed area of the same figure. After jetting through the holes, the coolant flows along the PS and SS ribbed channels to mix at the TE cavity and eventually discharge through a spanwise row of ten holes on the airfoil PS. SS channels up to the TE cavity are a bit longer than PS ones due to the small curvature of the profile. Although a very sharp LE increases the heat load because of the higher external stagnation HTC, this constraint could not be relaxed because of the contra-rotating nature of the turbine which requires a very low turning profile with the lowest possible thickness in order to minimise the flow acceleration along the SS and the associated external aerodynamic losses. Fig. 1 Real Engine NGV Geometry (Detail of Insert Tube LE Impingement Orifices) The particular configuration of two staggered rows of impingement holes distributed all along the span of the LE was chosen mainly to minimize the coolant flow consumption and decrease the cooling system sensitivity to small deviations in the final real position of holes after manufacturing in the roduction phase. Longitudinal ribs at both airfoils sides were provided so as to ensure a good distribution of the cooling flow along the airfoil span. Five channels separated by four ribs with four holes each were defined. The chordal ribs in both airfoil sides start in the straight part of the airfoil (6.5d away from the airfoil LE). III. EXPERIMENTAL AND NUMERICAL GEOMETRY Fig. 2 is a scheme showing further details of the impingement geometry including a plane schematic projection of the full vane internal geometry. It is also shown the domain selected for the CFD analysis done which corresponds to the center channel of the real geometry. This central channel was also taken as the baseline in the test model which consists of three of theses channels to minimize any inlet or close end effects on the results. As shown in Fig. 2, SS will be presented at the left hand side and PS at the right hand side on all plots through the paper. Fig. 2 Impingement Layout Scheme and corresponding CFD domain ISBN:

3 A computational model is constructed by reproducing a domain corresponding to the geometry of the central channel of the real engine geometry. The computational model therefore also corresponds to the geometry of each of the three channels of the perspex model tested by De La Calzada and Alvarez [4]. Figure 3 shows the representative domain of the geometry and details of the mesh distribution on the internal surface of the domain. The impingement tube is extended well beyond the cooling side channels height in order to avoid any inlet effects on the impingement jets. It can be also identified that the computational domain also included the side channels developing along the airfoil sides, the rear cavity and the exit holes. This full configuration was run so that any upstream effect of the side channels and exit holes on the impingement jets was retained in the solution. This method ensures that any internal far field effect on the impingement cooling area was retained, although a much larger mesh size and computational time was needed. Fig. 3 CFD Geometry and Internal Surface Mesh Details IV. NUMERICAL SIMULATION The steady 3D CFD analysis was performed using the commercial CFD code, Fluent (Version 6.2), Inc, a pressurecorrection based, multi-block and multigrid solver. The mesh generation tool ICEMCFD was used to generate a structured mesh with about nodes. The mesh generated was fully structured by using hexahedra. The grid was generated with boundary layers on solid walls. Boundary layer was fully resolved with a criterion of y + = 1 at the wall and a ratio of cell size increase of about 20% when moving away form the walls. These mesh parameters ensure sufficient mesh independence results based on the experience of the authors when validating this CFD tool for heat transfer simulations. The turbulence was simulated with the k-ω Shear Stress Transport (SST) model, which blended the k-ω model in the near wall region with the free stream independence of the k-ω model in the far field. The model was defined as periodic spanwise and therefore the upper and lower boundaries, except for those of the impingement tube, were defined as periodic conditions. The impingement tube upper boundary was defined as flow inlet while the lower end was closed. Exit conditions with imposed static pressure were defined at the exit surface of the film cooling exit holes at the rear of the airfoil. The boundary condition values were defined in accordance to real engine conditions. Since similarity between real and tested conditions were obtained by the experimental set-up, the same Mach number and Reynolds number was ensured. In particular the condition simulated correspond to the nominal case (i.e. Reynolds number based on impingement holes diameter equal to 3334). In order to ensure that the heat transfer coefficient is captured with sufficient accuracy by the numerical simulation, while avoiding any affecting change in fluid density, the wall temperature was imposed as a constant value around 30 K greater than the inlet fluid total temperature. The conditions imposed were: P 0,in = Pa T 0,in = 670,4 K T wall = 700 K P ex = Pa Convergence of the numerical solution was achieved initially by a first order discretization and after by a second order discretization. A large amount of numerical and physical parameters were monitored throughout the process aiming at ensuring that an acceptable level of convergence was reached within the whole computational domain. Since the experimental technique used in this investigation was focused on the measurement of the HTC at the impingement region, only a detail comparison of this feature could be used as a means to assess the merit of the CFD simulation. Based on the conclusions of this comparison, some further analysis of the flow physics are performed. A. Heat Transfer Results Results from the CFD simulation are presented in Fig. 4 which can be compared with experimental results from Fig. 5. In general terms, the configuration of the HTC footprint is quite similar between experimental and CFD cases both featuring clear impingement regions for each jet and secondary areas of high HTC appearing in the mid way between jets both between spanwise located jets and between the staggered located jets. As expected from jets impinging on target surfaces the jet cores generate impingement stagnation regions characterized by high heat transfer rates due to the more perpendicular velocity to the wall and the corresponding reduction of the thermal boundary layer. These stagnation points are surrounded by regions where the incident fluid flows away along the wall hence increasing the dynamic and thermal boundary layers. As a result the HTC far around the impingement points decreases to low levels corresponding to ISBN:

4 the levels of a forced convection flow parallel to the wall. Where adjacent jets are present the confluence of the two streams generates a particular vortex configuration with large variations of HTC as will be explained further below. Although the system was designed symmetrically respect to the LE center line so that the same behavior was intended for SS and PS impingement jets, both numerical and experimental results show stronger HTC on the PS and weaker on the SS pronounced, with higher levels, HTC peaks with their contours more defined. This is thought to be due to the lower jet mixing expected to be predicted by the numerical simulation which would increase the jet core momentum compared with the real case and that would enhance the impingement capability of the jet. The lower jet mixing predicted by the CFD seems to be a general deficiency on these simulations in which the periphery jet shear layers plays an important role and where the numerical turbulence models usually do not provide the required level of mixing. Additionally, once the fluid flows along the wall around the stagnation region, the area of influence of the impingement is also larger in the numerical solution. Unlike the experimental results which present an elliptical shape of the impingement region a clear asymmetry appears in the CFD results where a more irregular shape is generated specially towards the side channels. These are also effects that can be expected by the difference in the mixing Fig. 4 CFD Nu Distribution MIN HTC MAX HTC MIN HTC Fig. 6 Sketch of the interaction mechanism between jets Fig. 5 Experimental Nu Distribution A remarkable difference between numerical and experimental results is the resulting shape definition of the impingement HTC contours. The CFD results present more With regards to the secondary areas of high HTC found at the interaction between jets, this phenomena has been identified already by other authors and was first described by Gardon and Akfirat [9] and more recently by some others as Son et al [10] for example. A sketch of this kind of interaction is presented in Fig. 6. Under this mechanism two small vortexes rotating in opposite directions would occur at the confluence of the two opposite side flows coming along the wall and would be located just underneath of the general ejection region created to evacuate the total flow. This model would explain the high HTC regions appearing just in the middle between jets by the generation of an injection stagnation region due to the confluence of the two counterrotating small vortexes. Here the fluid would flow perpendicular toward the wall hence generating an impingement stagnation region with a high velocity component perpendicular toward the wall, therefore generating a thin thermal boundary layer and therefore a point of high HTC. On the lateral side of the two vortexes, ejection stagnation regions would be generated. There, the flow arriving from the sides is ejected away from the wall hence generating an ejection stagnation region with a high perpendicular value of the velocity in direction away from the wall therefore generating a thick thermal boundary layer and therefore a low HTC. It is ISBN:

5 remarkable that these secondary areas are noticeable higher in the numerical prediction. Moreover the highest levels of these secondary HTC maxima appear in the CFD results due to the interaction of adjacent staggered jets while in the experiment the highest level is found due to the spanwise interaction of jets. The higher levels of the maximum peaks at the impingement point, the lower levels at the local minimum points, and the stepper variation of heat transfer coefficient predicted by the numerical simulation are clearly identifiable in Fig. 7 where the impingement effects of the SS jets are plotted. As was aforementioned, the higher levels of the second peak between jets due to its interaction in spanwise direction are higher in the experiments even though a sharper definition of this interaction is showed by the numerical results clearly showing the interaction mechanism explained in Fig. 6. However the surface averaged values are very similar in both cases and moreover match quite well Chupp correlation. Moreover clear and defined HTC peaks due to the jet core impingement are present in both results. It is acknowledged by the authors that the difference in peak values at impingement regions between simulation and experiment is up to a factor of 2 and that also there is important difference in the levels at regions around the jet influence. However the main details being discussed in this work are present in both results, i.e. the generation of a second peak at the confluence of two jets, hence demonstrating that a common mechanism must be present in both cases. different interactions: one between adjacent staggered jets from SS and PS, and the other from the spanwise adjacent jets at PS. Fig. 8 Nu Distribution Along a Streamwise Line Crossing the Upper SS Jet B. Main Flow Features No flow field visualization was made during the experiments and therefore the HTC prints on the target surface is the only information available for comparison. In order to be able to go further in the flow details and in the main flow characteristics, with effect on the surface HTC, analysis of the CFD results was carried out. Fig. 7 Nu Distribution Along SS Impingement Centrelines Comparison of CFD and experiments with regards to the HTC variation through the upper SS impingement jet is shown in Fig. 8. Again the much higher levels of HTC and more at the impingement region obtained by the CFD results are clear. It is also remarkable that the SS jets deflect towards the side channel as can be identified by noting that the HTC peak in the CFD results is moved to the left hand side hence indicating that the impingement point is moved further from the LE. Although the area of influence of the impingement region is similar in both results, extending to a relatively large region, the more defined and sharper jet impingement is clear on the numerical simulation. The two peaks appearing at the right side of the jet impingement dominated region correspond in this particular case to the local maxima values due to the two Fig. 9 Velocity Contours (m/s) at Jet Mid Planes In order to make a qualitative analysis a 3D view of the velocity contours in the mid plane of each of the four jets is shown in Fig. 9. Contrary to what could be expected out of the mass flow distribution through channels, being the double on the PS than on the SS, the SS jets are deviated towards the side channel impinging the wall with an angle while the PS jets follow a straighter path until it reaches the target wall at the LE area more perpendicularly. Additionally it is worth noting that at the PS the jet cores are not symmetrical and the high momentum flow is concentrated on the left side hence ISBN:

6 impinging closer to the LE and even more perpendicularly at the wall. This particular feature is thought to be responsible of the higher HTC peak values observed on the PS impingement regions as showed in Figs. 4 and 5 (especially on the numerical results) and therefore it is thought to be present in the real case although possible with a weaker effect since the experimental results did not show so large difference and the position of the impingement points are more symmetrically distributed. Additionally, the shapes of the HTC prints are more elliptical and with similar size in the experiments so that this effect is confirmed to be less important in the real case. REGION Fig. 11 Flow Details at the Left Side of Upper PS Jet Impingement Region. Background Coloured by Static Temperature (K) Fig. 10 Velocity Vectors at Mid Plane of Upper PS jet. Background Coloured by Static Temperature (K) A more detail view on the impinging flow from a PS hole is presented in Figs. 10 to 12, where the background of the plots has been colored by static temperature to help identifying the different phenomena affecting the heat transfer. The straight path followed by the jet and the general flow configuration and vortices can be easily observed in Fig. 10. Also the asymmetry in the jet core with reducing velocity at the side channel side can be identified. The true core is moved towards the jet side closer to the LE center where the impingement is more perpendicular to the target wall. Owing to the target surface angle the flow configuration is not symmetric. While towards the LE the typical boundary layer flow, with fluid flowing along the wall from the impinging jet, is followed by a vortex region at the point of confluence with the flow from the adjacent staggered jet, this feature is not present on the other side of the jet. This is clear shown in Fig. 11 where, due to the high angle formed by the wall and the jet on this side, the fluid is not able to flow backward along the wall. However a clear region of low heat transfer appears anyhow due to the low velocity stagnation region generated and the absence of a velocity boundary layer hence making it possible the development of a thick thermal boundary layer and low HTC. A more typical vortex configuration is generated on the left hand side of the impinging jet where the wall is almost perpendicular to the jet, as shown in Fig. 12. The flow from the jet interacts with the corresponding staggered opposite jet hence generating a large ejection flow moving away from the wall. In the standard configuration (i.e. Fig. 6) two smaller vortexes would be generated to eventually obtain one injection stagnation region with high HTC in the middle and two side ejection stagnation regions with low HTC. Although the configuration is not symmetric in Fig. 12, still a clear central region of high HTC and two sides of low HTC are generated as can be confirmed by Fig. 4. While a small closed vortex is clearly identifiable at the right hand side, generating an ejection region with low HTC and an impingement region with high HTC at the centre, the left vortex is not so clearly generated. This vortex is squeezed along the wall and, although a clear ejecting flow it is not generated, the wall flow coming from the impingement region suddenly decelerates, because of the opposite shear layer above it, hence making it possible the increase of both the velocity and thermal boundary layers and decreasing the HTC. REGION REGION REGION Fig. 12 Flow Details at the Right Side of Upper PS Jet Impingement Region. Background Coloured by Static Temperature (K) ISBN:

7 In particular, in our case the typical double vortex configuration, at the confluence of the two opposite boundary flows coming from the adjacent jets, is more clearly generated in the interaction between staggered jets from PS and SS as plotted in Fig. 13. In this particular plot the fluid flow along a horizontal cut at mid distance between upper PS and SS jets is represented. As already identified in the surface HTC plot in Fig. 4, a very clear region with high HTC is located between the staggered jets. Here the explanation of this behavior due to the double vortex configuration of Fig. 6 can be confirmed. As shown by the velocity vectors, a general ejection region is created by the opposite confluence streams flowing along the wall coming from each of the two staggered jets. This ejection region is needed to evacuate the total fluid coming along the side walls. However, underneath this general ejection region, a local impingement region at the center is generated surrounded by two opposite ejection regions hence generating the high HTC region at the center and the two low HTC regions at the two sides. This particular configuration is generated because the two side boundary flows approaching separate before reaching the center stagnation region due to the inability of the boundary layer flow to recover the inlet value of stagnation pressure hence generating the two separated flow vortexes at the sides and the center impingement region. This behavior must also be present on the experimental case since a local high HTC region is also present at the mid region between staggered jets specially on the down side although the extension of this area is much lower compared with the numerical simulation. The strength of this kind of vortex configuration and the magnitude of the HTC variation must then be driven by the low Reynolds number of this particular case. It is also though that the concave geometry of the LE region also can plays a role on this kind of configuration. Therefore it is expected that different levels of HTC variations at the confluence of side jets can appear depending of the Reynolds number and the wall curvature of the particular geometry. V. CONCLUSIONS A numerical simulation of an experimental test case representative of a real impingement cooling configuration for a counter-rotating low pressure vane has been performed. Available test results in terms of surface heat transfer at the LE region of the vane have allowed the comparison with the numerical predictions. The CFD simulation predicts higher peak values at the impingement point probably due to a higher jet core momentum due to poor mixing of the jet. Contrarily, CFD results show lower levels of HTC at region further from the impinging jet influence. However, the HTC relative variation between impinging jets is qualitatively well captured by the CFD simulation so that it has been possible to investigate this particular feature more in detail based on the CFD simulation results. In particular the high HTC region due to the impingement jets as well as the secondary region of local high HTC at the interaction between jets has been predicted by the CFD simulation. Higher and sharper peaks in the impingement regions are predicted by the numerical simulation (up to a factor of 2 compared with experiments) with more defined, though lower levels, secondary peaks at the confluence of two jets. This sharper definition is thought to be due to the lower mixing at the jet boundary shear layers expected to be predicted by the numerical simulation hence enabling a more defined, higher momentum jet to impinge on the wall and to interact with the other jets and the surrounding fluid. Clear impingement and ejection stagnation regions are found to be responsible of the maximum and minimum HTC local values at the wall. These HTC variations are generated by the impinging jets and the secondary vortexes generated at the confluence of the streams coming from adjacent jets. ACKNOWLEDGMENTS The authors wish to thank ITP for the permission to publish this paper. NOMENCLATURE Fig. 13 Standard Vortex Configuration of the Secondary Impingement Region Between staggered Jets. Background coloured by static temperature (K) 3D three-dimensional CFD Computational Fluid Dynamics d impingement hole diameter h, HTC heat transfer coefficient k thermal conductivity, W/mK LE leading edge NGV Nozzle Guide Vane Nu p P PS PT s SS SST h d k = Nusselt number streamwise row pitch, mm pressure pressure side power turbine streamwise distance suction side shear stress transport ISBN:

8 T temperature TE trailing edge y spanwise distance y+ non-dimensional wall distance Z impingement to target surface distance Subscripts 0 stagnation conditions in inlet conditions ex exit conditions wall wall conditions REFERENCES [1] Holley, B.M and Langston, L.S, 2007 Analytical Modeling of Turbine Cascade Leading Edge Heat Transfer using Skin Friction and Pressure Measurements, ASME paper GT [2] Chupp, R.E., Helms, H.E., McFadden, P.W., and Brown, T.R., 1969, Evaluation of Internal Heat Transfer Coefficients for Impingement Cooled Turbine Airfoils, J. Aircr., 6(3), pp [3] Hrycak, P., 1981, Heat Transfer from a Row of Impinging Jets to Concave Cylindrical surfaces, Int. J. of Heat Mass Transfer, 24, pp [4] De la Calzada, P., and Alvarez, J.J., 2010, Experimental Investigation on the Heat Transfer of a Leading Edge Impingement Cooling System for Low Pressure Turbine Vanes. ASME J. Heat Transfer, 132(12), [5] Jia, R., Rokni, M., and Sunden, B., Numerical Assessment of Different Turbulence Models for Slot Jet Impinging on Flat and Concave Surfaces. ASME paper GT [6] Ibrahim, M.B., Kochuparambil, B.J., Ekkad, S.V., and Simon, T.S., CFD Jet Impingement Heat Transfer with Single Jets and Arrays, ASME paper Nº GT [7] Rama, B.V.N., and Prassad, B.V.S.S.S., Computational Investigation of Flow and Heat Transfer for a Row of Circular Jets impinging on a Concave Surface, ASME paper GT [8] Taslim, M.E., and Khanicheh, A., Experimental and Numerical Study if Impingement on and Airfoil Leading Edge with and without Showerhead and Gill Film Holes, ASME paper Nº 2005-GT [9] Gardon, R., and Akfirat, J.C, 1966, Heat Transfer Characteristics of Impinging Two-Dimensional Air Jets, ASME J. Heat Transfer, 88, pp [10] Son, C., Gillespie, D, Ireland, P.I., and Dailey, G.M., 2000, Heat Transfer and Flow Characteristics of an Engine Representative Impingement Cooling System, ASME paper Nº 2000-GT-219. ISBN: