Essentials Of Turbo-machinery In Cfd

1

CFD Open Series +++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++

Essentials of TurboMachinery in CFD Ideen Sadrehaghighi, Ph.D.

Flow in Axial turboMacines (CDAdapco)

Unsteady Flow in Axial TurboMachines (ANSYS)

Unsteady Flow in Radial TurboMachines (ANSYS)

ANNAPOLIS, MD

2

Table of Content Introduction ............................................................................................................................................ 9 1

2

Preliminary Concepts in Rotating Machinery .................................................................... 11

1.1 Vortex........................................................................................................................................................................ 11 1.2 Properties of Vortex Flow ................................................................................................................................ 11 1.2.1 Vorticity ................................................................................................................................ 11 1.2.2 Vortex types ......................................................................................................................... 12 1.2.2.1 A rigid-body vortex ....................................................................................................... 12 1.2.2.2 An irrotational vortex ................................................................................................... 12 1.2.3 Vortex Geometry .................................................................................................................. 12 1.3.4 Pressure in Vortex ................................................................................................................ 13 1.4 Impeller .................................................................................................................................................................... 13 2.4.1 Types of Impeller .................................................................................................................. 14 1.4.2 Flow Characteristics for Impeller ......................................................................................... 14 1.4.3 Mixing Tanks......................................................................................................................... 15 1.4.4 Axial impellers ...................................................................................................................... 16 1.4.5 Radial impellers .................................................................................................................... 16 1.4.6 Power Number for Impeller ................................................................................................. 16 1.5 Pumps ....................................................................................................................................................................... 16 1.5.1 Types of Pumps .................................................................................................................... 17 1.5.2 Axial-Flow Pumps vs. Centrifugal Pumps ............................................................................. 18 1.6 Some Physics on Rotating Disks Flow ......................................................................................................... 18 1.6.1 Experimental Set-Up ............................................................................................................ 18 1.6.1.1 Recirculating flow ......................................................................................................... 19 1.6.1.2 Instability flow patterns ............................................................................................... 19

Conservation of Angular Momentum .................................................................................... 22

2.1 Flow in Rotating Reference Frame ................................................................................................................ 22 2.2.1 Relative Velocity Formulation ........................................................................................... 23 2.2.2 Absolute Velocity Formulation .......................................................................................... 23 2.3 Modeling Flows with Rotating Reference Frames (MRF) ................................................................... 23 2.3.1 Single Rotating Reference Frame (SRF) Modeling ............................................................... 24 2.3.2 Flow in Multiple Rotating Reference Frames (MRF) ............................................................ 25 2.3.2.1 Case Study – Mixing Tank............................................................................................. 26 2.3.3 The MRF Interface Formulation ........................................................................................... 26 2.3.2.1 Interface Treatment: Relative Velocity Formulation ................................................... 27 2.3.3.2 Interface Treatment: Absolute Velocity Formulation .................................................. 27 2.4 The Mixing Plane Model (MPM)..................................................................................................................... 27 2.4.1 Rotor and Stator Domains .................................................................................................... 28 2.4.2 The Mixing Plane Concept .................................................................................................... 29 2.4.3 Mixing Plane Algorithm ........................................................................................................ 29 2.4.3.1 Mass Conservation across the Mixing Plane ................................................................ 29 2.5 Sliding Mesh Modeling ....................................................................................................................................... 30 2.5.1 Sliding Mesh Theory ............................................................................................................. 30 2.5.2 The Sliding Mesh Technique ................................................................................................ 31

3

2.5.3

3

4

Sliding Mesh Concept ........................................................................................................... 32

Elements of Turbomachinery .................................................................................................. 34

3.1 Background ............................................................................................................................................................ 34 3.2 Historical Perspectives ...................................................................................................................................... 35 3.3 Modern Turbomachinery as related to Gas Turbine Engine.............................................................. 35 3.4 How does it work? ............................................................................................................................................... 37 1.5 Gas Turbine Performance................................................................................................................................. 38 3.6 Gas Compressors .................................................................................................................................................. 38 3.6.1 Axial-flow compressors ........................................................................................................ 39 3.6.2 Centrifugal Compressors ...................................................................................................... 40 3.6 Nomenclature of Terms .................................................................................................................................... 40 3.7 Component of Gas Turbine Engine .............................................................................................................. 43 3.7.1 Inlet ...................................................................................................................................... 43 3.7.2 Axial Compressor.................................................................................................................. 44 3.7.3 Diffuser ................................................................................................................................. 46 3.7.4 Nozzle ................................................................................................................................... 47 3.7.5 Combustor ............................................................................................................................ 47 3.7.6 Axial Gas Turbine.................................................................................................................. 48 3.8 Difference in Blading between Compressor and Turbine ................................................................... 49 3.8 Velocity Triangles in Turbomachines .......................................................................................................... 50 3.9 Energy Exchange with Moving Blades ........................................................................................................ 51 3.9.1 Euler’s equation for turbomachinery .................................................................................. 51 3.10 Compressors and their Reaction to Intake Distortion ....................................................................... 53 3.11 Effects of Turbine Temperature .................................................................................................................. 55 3.12 Compressor and Turbine Characteristics ............................................................................................... 57 3.12.1 Stall .................................................................................................................................... 57 3.12.1 Compressor Surge ............................................................................................................. 58 3.12.3 Choked Flow ....................................................................................................................... 59

Primary Research in Turbomachinery ................................................................................ 59 4.1 Research Spectrum ............................................................................................................................................. 60 4.2 Application of CFD in Turbomachinery ........................................................................................................ 61 4.3 Quasi 3D flow (Q3D) ........................................................................................................................................... 61 4.3.1 Stream Surface of Second Kind - Through flow (S2) ............................................................ 62 4.3.3 Stream Surface of First Kind (Blade 2 Blade – S1) ................................................................ 63 4.3.2 Theory of Radial Equilibrium in Through Flow (Cr = 0) ......................................................... 64 4.4 Governing Equation of Rotating Frame of Reference ........................................................................... 65 4.5 Efficiency effects in Turbomachinery .......................................................................................................... 67 4.5.1 Isentropic Efficiency ............................................................................................................. 67

5

Complex flow in Turbomachinery ......................................................................................... 69

5.1 Key Features of Transonic Fan (Turbine) Field ...................................................................................... 69 5.2 Sources of Unsteadiness in Turbomachinery........................................................................................... 70 5.3 Interaction of Potential flows in adjacent blade rows .......................................................................... 72 5.3.1 Interactions in Transonic Fan ............................................................................................... 72 5.4 Interaction between Wake Flow and Blade Rows.................................................................................. 73 5.5 Interaction between Secondary Flows and Blade Rows...................................................................... 74

4

5.6 Wake-Boundary Layer Interaction ............................................................................................................... 75 5.7 Unshrouded Tip Leakage Flow Interaction............................................................................................... 76 5.8 Film Cooling Effects ............................................................................................................................................ 77 5.9 General Review on Secondary Flows ........................................................................................................... 77 5.9.1 Classical View ....................................................................................................................... 78 5.9.2 Modern View ........................................................................................................................ 78 5.9.3 Latest View ........................................................................................................................... 80 5.9.4 Comparing and Contrasting Secondry Flow in Turbine and Compressors ........................... 82 5.9.5 3D Separation ....................................................................................................................... 84 5.10 Turbulence Consideration ............................................................................................................................. 85 5.11 Case Study - Heat Transfer in Separated Flows on the Pressure Side of Turbine Blades ... 86 5.11.1 Statement of Problem ........................................................................................................ 86 5.11.2 Literature Survey ................................................................................................................ 87 5.11.3 CFD Modeling ..................................................................................................................... 88 5.11.4 Description of the Blade and Computational Grids, and Results for Attached Flow ......... 89 5.11.5 Separated Flow with Large Separation Bubble ................................................................. 90 5.11.5.1 Inlet Flow Angle Effects .............................................................................................. 93 5.11.5.2 Reynolds Number Effect ............................................................................................ 94 5.11.6 Concluding Remarks ........................................................................................................... 96

6

Rotor-Stator Interaction Treatment (RST) ......................................................................... 98 6.1 Physical Perspectives ......................................................................................................................................... 98 6.2 Different Between Multi-Passage and Multi-Stages .............................................................................. 99 6.2 Steady Treatment of Interface ..................................................................................................................... 100 6.2.1 Mixing Plane ....................................................................................................................... 100 6.2.2 Frozen Rotor ....................................................................................................................... 101 6.3 Unsteady Treatment of Interface ............................................................................................................... 102 6.3.1 Sliding Mesh (MRF) ............................................................................................................ 102 6.3.2 Non-Linear Harmonic Balanced Method (NLHB) ............................................................... 103 6.3.3 Profile Transformation (Pitch Scaling)................................................................................ 105 6.3.4 Time Transformation Method (TT) using Phase-Shifted Periodic Boundary Conditions ... 105 6. 4 Revisiting Non-Linear Harmonic Balance (NLHB) Methodology ................................................ 107 6.4.1 Temporal and Spatial Periodicity Requirement ................................................................. 107 6.4.2 Boundary Conditions .......................................................................................................... 108 6.4.3 Solution Method ................................................................................................................ 108 6.4.4 Fourier 'Shape Correction' for Single Passage Time-Marching Solution ............................ 110 6.4.4 Case Study 1 – 2D Compressor Stage................................................................................. 111 6.4.5 Case Study 2 - 3D Flow in Turbine Cascade........................................................................ 112

7

Radial Flow.................................................................................................................................. 115

7.1 Centrifugal Compressor ................................................................................................................................. 115 7.1.1 Theory of operation ........................................................................................................... 115 7.1.2 Similarities to Axial Compressor......................................................................................... 115 7.1.3 Components of a simple Centrifugal Compressor ............................................................. 116 7.1.3.1 Inlet ............................................................................................................................ 116 7.1.3.2 Centrifugal Impeller ................................................................................................... 116 7.1.3.3 Diffuser ....................................................................................................................... 117

5

7.1.3.4 Collector ..................................................................................................................... 117 7.1.4 Applications ........................................................................................................................ 118 7.1.4.1 In gas turbines and auxiliary power units .................................................................. 118 7.1.4.2 Automotive engine and diesel engine turbochargers and superchargers ................. 118 7.1.4.3 Natural gas to move the gas from the production site to the consumer .................. 118 7.1.4.4 Oil refineries, natural gas processing, petrochemical and chemical plants............... 118 7.1.4.5 Air-conditioning and refrigeration and HVAC ............................................................ 118 7.1.4.6 In industry and manufacturing to supply compressed air ......................................... 119 7.1.4.7 In air separation plants to manufacture purified end product gases ........................ 119 7.1.4.8 Oil field re-injection of high pressure natural gas to improve oil recovery ............... 119 7.2 Radial turbine ..................................................................................................................................................... 119 7.2.1 Advantages and challenges ................................................................................................ 120 7.2.2 Types of Radial Turbines .................................................................................................... 120 7.2.2.1 Cantilever Radial Turbine ........................................................................................... 120 7.2.2.2 90 Degree IFR Turbine ................................................................................................ 120 7.2.2.3 Outward-flow radial stages ........................................................................................ 121

8

Best Practice Guidelines for Turbo Machinery CFD ..................................................... 122

8.1 Quasi-3D (Q3D) or 3D Simulation.............................................................................................................. 122 8.1.1 2-D Simulations .................................................................................................................. 122 8.1.2 Quasi-3D (Q3D) Simulation ................................................................................................ 122 8.1.3 Full 3D simulations ............................................................................................................. 122 8.2 Single vs Multi-Stage Analysis ..................................................................................................................... 123 8.2.1 Single Stage ........................................................................................................................ 123 8.2.2 Multi-Stage Analysis ........................................................................................................... 124 8.2.2.1 Steady Mixing-Plane simulations ............................................................................... 124 8.2.2.2 Steady frozen rotor simulations ................................................................................. 124 8.2.2.3 Unsteady Sliding Mesh stator-rotor simulations ....................................................... 124 8.2.2.4 Unsteady Harmonic Balance simulations................................................................... 124 8.2.2.5 Hybrid steady-unsteady stator-rotor simulations...................................................... 125 8.2.2.6 Other advanced multi-stage methods ....................................................................... 125 8.3 Inviscid or Viscid ............................................................................................................................................... 125 8.4 Transient or Steady-State .............................................................................................................................. 126 8.5 Meshing ................................................................................................................................................................. 126 8.5.1 Mesh size Guidelines .......................................................................................................... 127 8.5.2 Boundary Mesh Resolution ................................................................................................ 128 8.5.3 Periodic Meshing ................................................................................................................ 128 8.6 Boundary Conditions....................................................................................................................................... 129 8.7 Turbulence Modeling ...................................................................................................................................... 130 8.8 Aero-Mechanics ................................................................................................................................................. 131 8.8.1 Nodal Diameter .................................................................................................................. 132 8.9 Near Wall Treatment ....................................................................................................................................... 132 8.10 Transition Prediction.................................................................................................................................... 133 8.11 Numerical Consideration ............................................................................................................................ 133 8.12 Convergence Criteria .................................................................................................................................... 133 8.13 Single or Double Precision ......................................................................................................................... 134 8.14 Heat Transfer Prediction............................................................................................................................. 134

6

List of Tables Table 1 Table 2 Table 3

Prescribed Boundary zone for Mixing Plane ......................................................................................... 29 Glossary of Turbomachinery Terms ......................................................................................................... 40 Rotor/Stator Interaction Schemes............................................................................................................. 99

List of Figures Figure 1 Figure 2 Figure 3 Figure 4 Figure 5 Figure 6 Figure 7 Figure 8 Figure 9 Figure 10 Figure 11 Figure 12 Figure 13 Figure 14 Figure 15 Figure 16 Figure 17 Figure 18 Figure 19 Figure 20 Figure 21 Figure 22 Figure 23 Figure 24 Figure 25 Figure 26 Figure 27 Figure 28 Figure 29 Figure 30 Figure 31 Figure 32 Figure 33 Figure 34 Figure 35 Figure 36 Figure 37 Figure 38 Figure 39 Figure 40 Figure 41 Figure 42 Figure 43

Vortex created by the passage of an aircraft wing, revealed by colored smoke ................... 11 A rigid-body vortex ........................................................................................................................................ 12 A Plughole vortex ............................................................................................................................................ 13 Types of Impeller ............................................................................................................................................ 14 A centrifugal pump uses an impeller with backward-swept arms ............................................. 14 Flow direction of three different pumps/impellers. Image credit: Global spec ..................... 15 Axial flow impeller (left) and radial flow impeller (right) ............................................................. 15 Centrifugal Pumps .......................................................................................................................................... 17 Sketch of the experimental set-up............................................................................................................ 18 For s ≥ 0 co-rotation at different speed ............................................................................................... 20 For s < 0 counter-rotating at different speed................................................................................... 20 Rotating Frame of Reference ................................................................................................................... 22 Single Blade Model with Rotationally Periodic Boundaries ....................................................... 25 Mixing Tank geometry with one rotating impeller ........................................................................ 26 Mixing Tank with two rotating impellers ........................................................................................... 26 Interface Treatment for the MRF Model ............................................................................................. 27 Mixing Plane concepts as applied to axial rotation ........................................................................ 28 Mixing Plane concepts applied to radial rotation ........................................................................... 29 Illustration of Unsteady Interactions .................................................................................................... 30 Examples of transient interaction using sliding mesh .................................................................. 31 Initial position and some translation with Sliding Interface ...................................................... 32 Dynamic Interface Zones ........................................................................................................................... 33 Classification of Turbomachines ............................................................................................................ 34 Component of Turbomachines and their Thermodynamic (Brayton cycle) properties .. 36 Twin Pool Jet Engine ................................................................................................................................... 37 Gas Compressor Types ............................................................................................................................... 39 Schematics of Axial Compressor ............................................................................................................ 39 A single stage Centrifugal Compressor ................................................................................................ 40 Blade related terminology ........................................................................................................................ 44 Compressor Flow Characteristics .......................................................................................................... 44 Pressure and Velocity profile through a Multi-Stage Axial Compressor ............................... 45 Combustor primary operating components ...................................................................................... 48 Turbine Flow Characteristics .................................................................................................................. 48 Schematics of axial flow Turbine ........................................................................................................... 49 Examples of typical Blades for Compressor and Turbine............................................................ 50 Velocity triangles for an Axial Compressor ....................................................................................... 50 Velocity triangles in relation to incident angle ................................................................................ 52 Compressor operating map...................................................................................................................... 53 Sample engine Perssure, Velocity and Temperature variation ................................................. 55 Turbine Inlet Temperature27 ................................................................................................................... 56 Characteristics Graph of a Compressor ............................................................................................... 57 Illustration of the propagation of a stall cell in the relative frame .......................................... 58 Classical Compressor surge cycles ........................................................................................................ 58

7

Figure 44 Figure 45 Figure 46 Figure 47 Figure 48 Figure 49 Figure 50 Figure 51 Figure 52 Figure 53 Figure 54 Figure 55 Figure 56 Figure 57 Figure 58 Figure 59 Figure 60 Figure 61 Figure 62 Figure 63 Figure 64 Figure 65 Figure 66 Figure 67 Figure 68 Figure 69 Figure 70 Figure 71 Figure 72 Figure 73 Figure 74 Figure 75 Figure 76 Figure 77 Figure 78 Figure 79 Figure 80 Figure 81 Figure 82 Figure 83 Figure 84 Figure 85 Figure 86 Figure 87 Figure 88 Figure 89 Figure 90 Figure 91 Figure 92 Figure 93

Impact of CFD on SNECMA fan performance, over a period of 30 years ............................... 60 Illustration of S1 and S2 surfaces .......................................................................................................... 62 Streamline Curvature method................................................................................................................. 63 Radial Equilibrium ....................................................................................................................................... 65 Coriolis and Centripetal forces created by the Rotating Frame of Reference ..................... 66 Compression process .................................................................................................................................. 67 Expansion process ....................................................................................................................................... 67 Complex Flow phenomena compressors ............................................................................................ 69 Fan Tip section geometry.......................................................................................................................... 70 Flow structures with 5 to 6 orders of magnitudes variations in length and time scales 72 Shock Structure in Transonic Fan.......................................................................................................... 73 Pressure contour of wake flow .............................................................................................................. 74 Unsteady wakes convecting in blade passage .................................................................................. 74 Instantaneous absolute velocity contour pattern at nozzle exit ............................................... 75 Flow over an unshrouded tip gap......................................................................................................... 76 Typical high-pressure turbine stage showing rim seal and wheel-space ............................. 77 Classical Secondary Flow Model ............................................................................................................ 79 Modern Secondary Flow Model .............................................................................................................. 80 Vortex pattern of Latest secondary flows .......................................................................................... 81 Turbine Secondary Flow Model after Takeishi et al...................................................................... 82 Illustration of formation of hub corner stall together with ........................................................ 84 T106-300 Cascade geometry and aerodynamic design conditions ......................................... 89 2-D hybrid mesh around the T106 blade ........................................................................................... 90 Blade profile pressure coefficient .......................................................................................................... 91 Flow field at the front and middle parts of the separation bubble .......................................... 92 Heat transfer coefficient for different negative incidences......................................................... 93 Stanton number for different negative incidences ......................................................................... 94 Heat transfer coefficient for different Reynolds number ............................................................ 95 Stanton number for different Reynolds numbers ........................................................................... 96 Schematics of 3-D concept at IGV/Rotor/Stator interface .......................................................... 98 Interface between Rotor/Stator ............................................................................................................. 99 Difference between Passage and Stages ............................................................................................. 99 Axial rotor/stator interaction (Schematics illustrating the Mixing Plane concepts) .... 100 Block Computational domain for a Rotor with guiding vanes ................................................ 100 A compressor Pressure Distribution on a surface using a Mixing Plane ............................ 101 Predicted Total Pressure calculated by the frozen rotor .......................................................... 102 Half stencil and full stencil reconstruction with: A) Intersection, B) Halo-cell ............... 103 Relative velocities obtained using HB techniques ....................................................................... 104 Phase shifted Periodic Boundary ........................................................................................................ 105 Phase Shifted Periodic Boundary Conditions ................................................................................ 106 Stagnation Pressure Contours under inlet distortion for NASA Rotor 67 ......................... 111 Computational mesh for HB and TRS methods ............................................................................ 112 Instantaneous pressure distribution within the compressor stage using (NLHB) ........ 112 Instantaneous predictions of turbulent viscosity at mid-span turbine for the TRS ...... 113 Instantaneous predictions of turbulent viscosity at mid-span turbine for the HB ........ 113 velocity profile on interface line between two rows .................................................................. 113 Centrifugal impeller with a highly polished surface likely to improve performance ... 115 Cut-away view of a turbocharger showing the centrifugal compressor ............................ 116 Jet engine cutaway showing the centrifugal compressor and other parts. ....................... 117 Ninety degree inward-flow radial turbine stage .......................................................................... 119

8

Figure 94 Figure 95 Figure 96 Figure 97 Figure 98 Figure 99 Figure 100 Figure 101 Figure 102

Outward Flow Radial Turbine .............................................................................................................. 120 Different Flow (2D, Q3D, and full 3D) ............................................................................................... 123 Full Blade Simulation using Harmonic Balanced Method......................................................... 125 Transient Blade Row extensions enable efficient multi-stage CFD simulation ............... 126 Typical meshing of a Turbomachinery stage ................................................................................. 127 Multi-block grid for the space shuttle main engine fuel turbine ........................................... 127 Pressure contour plot, 2nd order spatial discretization scheme ........................................ 129 Analysis provided vibration required for flutter analysis ..................................................... 131 Examples of Nodal Diameter .............................................................................................................. 132

9

Introduction Fluid mechanics and thermodynamics are the fundamental sciences used for turbine aerodynamic design and analysis. Several types of fluid dynamic analysis are useful for this purpose. The concept through-flow analysis is widely used in axial-flow turbine performance analysis. This involves solving the governing equations for inviscid flow in the hub-to-shroud plane at stations located between blade rows. The flow is normally considered to be axisymmetric at these locations, but still three-dimensional because of the existence of a tangential velocity component. Empirical models are employed to account for the fluid turning and losses that occur when the flow passes through the blade rows. By contrast, hub-to-shroud through-flow analysis is not very useful for the performance analysis of radial-flow turbomachines such as radial-inflow turbines and centrifugal compressors. The inviscid flow governing equations do not adequately model the flow in the curved passages of radial turbomachines to be used as a basis for performance analysis. Instead, a simplified “pitch-line” or “mean-line” one-dimensional flow model is used, which ignores the hub-to-shroud variations. These also continue to be used for axial-flow turbine performance analysis. Computers are sufficiently powerful today that there is really no longer a need to simplify the problem that much for axial-flow turbomachinery. More fundamental internal flow analyses are often useful for the aerodynamic design of specific components, particularly blade rows. These include 2D flow analyses in either the blade-to-blade or hub to shroud (Through Flow) direction, and Quasi-3D flow analyses developed by combining those 2D analyses. Wall boundary layer analysis is often used to supplement these analyses with an evaluation of viscous effects1. Viscous CFD solutions are also in use for turbines. These are typically 3D flow analyses, which consider the effects of viscosity, thermal conductivity and turbulence. In most cases, commercial viscous CFD codes are used although some in-house codes are in use within the larger companies. Most design organizations cannot commit the dedicated effort required to develop these highly sophisticated codes, particularly since viscous CFD technology is changing so rapidly that any code developed will soon be obsolete unless its development continues as an ongoing activity. Consequently, viscous CFD is not covered here beyond recognizing it as an essential technology and pointing out some applications for which it can be effectively used to supplement conventional aerodynamic analysis techniques. Prediction of the flow through cascades of blades is fundamental to all aspects of turbomachinery aerodynamic design and analysis. The flow through the annular cascades of blades in any turbomachine is really a 3D flow problem. But the simpler two-dimensional blade-to-blade flow problem offers many advantages. It provides a natural view of cascade fluid dynamics to help designers develop an understanding of the basic flow processes involved. Indeed, very simple twodimensional cascade flow models were used in this educational role long before computational methods and computers had evolved enough to produce useful design results. Today, blade-to-blade (B2B) flow analysis is a practical design and analysis tool that provides useful approximations to many problems of interest. Inviscid blade-to-blade flow analysis addresses the general problem of two-dimensional flow on a stream surface in an annular. Two-dimensional boundary layer analysis can be included to provide an approximate evaluation of viscous effects. That approach ignores the effect of secondary flows that develop due to the migration of low momentum boundary layer fluid across the stream surfaces. Its accuracy becomes highly questionable when significant flow separation is present. These limitations require particular care when analyzing the diffusing flow in compressor cascades. They are less significant for analysis of the accelerating flow in turbine cascades, but designers still must recognize the approximations and limitations involved. Previously, it have been emphasized the influence of the blade surface velocity distributions on nozzle row and 1

Ronald H Aungier, e-Books, “The American Society of Mechanical Engineers”, (ASME.org).

10

rotor performance. A graph of the blade surface velocity distributions as a function of distance along the blade surface is often referred to as the blade-loading diagram. The fundamental role of blade loading diagrams for the evaluation of blade detailed aerodynamic designs was discussed. Blade-toblade flow analysis provides a practical method to calculate these blade-loading diagrams. Indeed, blade-to-blade flow analysis is an essential part of a modern aerodynamic design system. A Quasi-3D flow analysis employs 2D flow analyses in the hub-to-shroud and blade-to-blade surfaces to approximate the 3D flow in a blade passage. The fundamental concept is generally credited to Wu2. The present analysis achieves exceptional computational speed and reliability largely due to its use of the linearized blade-to-blade flow analysis. But that also imposes some limitations on the method that are particularly significant for turbines. Its limitation to subsonic or low transonic Mach number levels excludes a number of turbine applications. As noted, its accuracy is compromised when it is applied to the rather thick airfoils often used for turbines. It certainly could be extended for more general use on turbines by substituting a more general blade-to-blade flow analysis such as the timemarching method. But that would substantially increase the computation time required and significantly reduce its reliability. It is very doubtful that this Quasi-3D flow analysis would remain an attractive design tool if that were done. Indeed, it would lose most of its advantages over commercially available viscous CFD codes while offering a less general solution. We start with some explanation of Rotating flow, as well as, derivation of Conservation of Angular Momentum concept which is fundamental in rotating flow, as well as blade to blade passage.

2 Wu, C. H., "A General Theory of Three Dimensional Flow in Subsonic and Supersonic Turbomachines of Axial,

Radial, and Mixed Flow Types," National Advisory Committee on Aeronautics, NACA TN 2604, 1952.

11

1 1.1

Preliminary Concepts in Rotating Machinery Vortex

One of the major aspects of rotational flow, and in fact the flow in general, is the concept of Vorticity. In fluid dynamics, a vortex is a region in a fluid in which the flow rotates around an axis line, which may be straight or curved3. The plural of vortex is either vortices or vortexes. Vortices form in stirred fluids, and may be observed in phenomena such as smoke rings, whirlpools in the wake of boat, or the winds surrounding a tornado, etc. (see Figure 1). Vortices are a major component of turbulent flow. The distribution of velocity, vorticity (the curl of the flow velocity), as well as the concept of circulation are used to characterize vortices. In most vortices, the fluid flow velocity is greatest next to its axis and decreases in inverse proportion to the distance from the axis. In the absence of external forces, viscous friction within the fluid tends to organize the flow into a collection of irrotational vortices, Figure 1 Vortex created by the passage of an aircraft wing, revealed by colored smoke possibly superimposed to larger-scale flows, including larger-scale vortices. Once formed, vortices can move, stretch, twist, and interact in complex ways. A moving vortex carries with it some angular and linear momentum, energy, and mass4.

1.2

Properties of Vortex Flow

1.2.1 Vorticity A key concept in the dynamics of vortices is the vorticity, a vector that describes the local rotary motion at a point in the fluid, as would be perceived by an observer that moves along with it. Conceptually, the vorticity could be observed by placing a tiny rough ball at the point in question, free to move with the fluid, and observing how it rotates about its center. The direction of the vorticity vector is defined to be the direction of the axis of rotation of this imaginary ball (according to the right-hand rule) while its length is twice the ball's angular velocity. Mathematically, the vorticity is defined as the curl (or rotational) of the velocity field of the fluid, usually denoted by ω and expressed by the vector analysis formula ∇ × u , where u is the local flow velocity. The local rotation measured by the vorticity ω must not be confused with the angular velocity vector Ω of that portion of the fluid with respect to the external environment or to any fixed axis. In a vortex, in particular, ω may be opposite to the mean angular velocity vector of the fluid relative to the vortex's axis.

3 4

Ting, L.,. “Viscous Vortical Flows. Lecture notes in physics”, Springer-Verlag, 1991, ISBN 3-540-53713-9. From Wikipedia, the free encyclopedia.

12

1.2.2 Vortex types In theory, the speed u of the particles (and, therefore, the vorticity) in a vortex may vary with the distance r from the axis in many ways. There are two important special cases, however: 1.2.2.1 A rigid-body vortex If the fluid rotates like a rigid body, that is, if the angular rotational velocity Ω is uniform, so that u increases proportionally to the distance r from the axis. A tiny ball carried by the flow would also rotate about its center as if it were part of that rigid body (see Figure 2). In such a flow, the vorticity is the same everywhere, its direction is parallel to the rotation axis, and its magnitude is equal to twice the uniform angular velocity Ω of the fluid around the center of rotation.

Ω  (0, 0, Ω)

Figure 2

A rigid-body vortex

r  (x, y, 0)

,

(.)

u  Ω  r  (-Ω y , Ω x , 0)  ω    u  (0, 0, 2Ω)  2Ω 1.2.2.2 An irrotational vortex If the particle speed u is inversely proportional to the distance r from the axis, then the imaginary test ball would not rotate over itself; it would maintain the same orientation while moving in a circle around the vortex axis. In this case the vorticity is zero at any point not on that axis, and the flow is said to be irrotational.

Ω  (0, 0, r -2 )

,

r  (x, y, 0)

(.)

u  Ω  r  (- yr -2 ,  xr -2 , 0)  ω    u  0 1.2.3 Vortex Geometry In a stationary vortex, the typical streamline (a line that is everywhere tangent to the flow velocity vector) is a closed loop surrounding the axis; and each vortex line (a line that is everywhere tangent to the vorticity vector) is roughly parallel to the axis. A surface that is everywhere tangent to both flow velocity and vorticity is called a vortex tube. In general, vortex tubes are nested around the axis of rotation. The axis itself is one of the vortex lines, a limiting case of a vortex tube with zero diameter. According to Helmholtz's theorems, a vortex line cannot start or end in the fluid – except momentarily, in non-steady flow, while the vortex is forming or dissipating. In general, vortex lines (in particular, the axis line) are either closed loops or end at the boundary of the fluid. A whirlpool is an example of the latter, namely a vortex in a body of water whose axis ends at the free surface. A vortex tube whose vortex lines are all closed will be a closed torus-like surface. A newly created vortex will promptly extend and bend so as to eliminate any open-ended vortex lines. For example, when an airplane engine is started, a vortex usually forms ahead of each propeller, or the turbofan of each jet engine. One end of the vortex line is attached to the engine, while the other end usually stretches out and bends until it reaches the ground. When vortices are made visible by smoke or ink trails, they may seem to have spiral path lines or streamlines. However, this appearance is often an illusion and the fluid particles are moving in closed paths. The spiral streaks that are taken

13

to be streamlines are in fact clouds of the marker fluid that originally spanned several vortex tubes and were stretched into spiral shapes by the non-uniform flow velocity distribution. 1.3.4 Pressure in Vortex The fluid motion in a vortex creates a dynamic pressure (in addition to any hydrostatic pressure) that is lowest in the core region, closest to the axis, and increases as one moves away from it, in accordance with Bernoulli's Principle. One can say that it is the gradient of this pressure that forces the fluid to follow a curved path around the axis. In a rigid-body vortex flow of a fluid with constant density, the dynamic pressure is proportional to the square of the distance r from the axis. In a constant gravity field, the free surface of the liquid, if present, is a concave paraboloid. In an irrotational vortex flow with constant fluid density and cylindrical symmetry, the dynamic pressure varies as P∞ − K/r2, where P∞ is the limiting pressure infinitely far from the axis. This formula provides another constraint for the extent of the core, since the pressure cannot be negative. The free surface (if present) dips sharply near the axis line, with depth inversely proportional to r2. The shape formed by the free surface is called a hyperboloid. The core of a vortex in air is sometimes visible because of a plume of water vapor caused by condensation in the low pressure and low temperature of the core; the spout of a tornado is an example. When a vortex line ends at a boundary surface, the reduced pressure may also draw matter from that surface into the core. For example, a dust devil is a column of dust picked up by the core of an air Figure 3 A Plughole vortex vortex attached to the ground. A vortex that ends at the free surface of a body of water (like the whirlpool that often forms over a bathtub drain) may draw a column of air down the core (see Figure 3). The forward vortex extending from a jet engine of a parked airplane can suck water and small stones into the core and then into the engine.

1.4

Impeller

An impeller (also written as impellor ) is a rotor used to increase (or decrease in case of turbines) the pressure and flow of a fluid. It has been used in variety of everyday equipment such as pumps, compressors, medical devices, mixing tanks, water jets and washing machines. More specifically, an impeller is a rotating component equipped with vanes or blades used in turbomachinery (e. g. centrifugal pumps). Flow deflection at the impeller vanes allows mechanical power (energy at the vanes) to be converted into pump power output. Depending on the fluid flow pattern in multistage pumps and the impellers' arrangement on the pump shaft, impeller design and arrangements are categorised as: single-stage, multistage, single-entry, double-entry, multiple-entry, in-line (tandem) or back-to-back arrangement. Axial and radial flow impellers are rotating industrial mixer components designed for various types of mixing. Both types of impellers are primarily constructed from stainless steel. Impellers impart flow. They serve the purpose of transferring the energy from the motor to the substance of a tank as efficiently as possible. Impellers are organized by their flow patterns.

14

2.4.1 Types of Impeller The impeller of a Centrifugal Pump can be of three types as shown in Figure 4   

Open Impeller where the vanes are cast free on both sides. Semi-Open Impeller when the vanes are free on one side and enclosed on the other. Enclosed Impeller The vanes are located between the two discs, all in a single casting5.

Figure 4

Types of Impeller

1.4.2 Flow Characteristics for Impeller Impellers can be designed to impart various flow characteristics to pump or tank media. Impeller flow designs can take on three distinct types: Axial, Radial, or Mixed (see Error! Reference source not found.). Because centrifugal pumps are also classified in this manner, the impeller selection depends upon matching the pump's flow characteristic to that of the impeller6.   

Axial flow impellers move media parallel to the impeller. Radial flow impellers move media at right angles to the impeller itself. Mixed flow impellers have characteristics of both axial and radial flow. They may move media at an angle which is different from right angle radial flow.

An impeller is a rotating component of a centrifugal pump, usually made of iron, steel, bronze, brass, aluminum or plastic, which transfers energy from the motor that drives the pump to the fluid being pumped by accelerating the fluid outwards from the center of rotation. The velocity achieved by the impeller transfers into pressure when the outward movement of the fluid is confined by the pump casing. Impellers are

5 6

Figure 5 A centrifugal pump uses an impeller with backward-swept arms

Presented by: Matt Prosoli, “Centrifugal Pump Overview”, Pumps Plus Inc. See Previous.

15

usually short cylinders with an open inlet (called an eye) to accept incoming fluid, vanes to push the fluid radially, and a splined, keyed, or threaded bore to accept a drive-shaft. The impeller made out of cast material in many cases may be called rotor, also. It is cheaper to cast the radial impeller right in the support it is fitted on, which is put in motion by the gearbox from an electric motor, combustion engine or by steam driven turbine. The rotor usually names both the spindle and the impeller when they are mounted by bolts.

Figure 6

Flow direction of three different pumps/impellers. Image credit: Global spec

1.4.3 Mixing Tanks Impellers in mixing tanks are used to mix fluids or slurry in the tank. This can be used to combine materials in the form of solids, liquids and gas. Mixing the fluids in a tank is very important if there are gradients in conditions such as temperature or concentration. Figure 7 shows two types of impeller used in mixing tanks, namely:  

Axial flow impeller Radial flow impeller

Radial flow impellers impose essentially shear stress to the fluid, and are used, for example, to mix immiscible liquids or in general when there is a deformable interface to break. Another application of radial flow impellers are the mixing of very viscous fluids. Axial flow impellers impose essentially bulk motion, and are used on homogenization processes, in which increased fluid volumetric flow rate is important. Impellers can be further classified principally into three sub-types7  7

Propellers

From Wikipedia, the free encyclopedia.

Figure 7

Axial flow impeller (left) and radial flow impeller (right)

16

 

Paddles Turbines

1.4.4 Axial impellers Are best for mixing applications that require stratification or solid suspension. Axial impellers are set up to create effective top to bottom motion in the tank. This motion is highly effective when placed over the center of a baffled tank. Some common types of axial flow impellers include: marine impellers, pitched blade impellers, and hydrofoils. Hydrofoil impellers are also known as high efficiency impellers. They are a popular choice for applications that require a range from general blending to storage tanks. This is largely due to the greatest pumping per horsepower, cost effectiveness, and are ideal for shear sensitive applications. 1.4.5 Radial impellers are designed in 4-6 blades. In radial flow impellers, the fluid moves perpendicularly to the impeller. They produce a radial flow pattern which moves the contents of the mixing tank to the sides of the vessel. The radial flow impacts the side which causes in either an up or down direction which fills the top and the bottom of the impeller to be ejected once more. It is also important to note that setting up baffles helps to minimize vortex and swirling motions in the tank, therefore, enhancing agitation efficiency. Radial impellers are a great fit for low-level applications inside longer tanks based upon the production of higher shear due to the angle of attack. 1.4.6 Power Number for Impeller Power number is a value specific to mixing impellers which describes the impeller's power consumption. The formula for calculating an impeller's power number is

Np 

p n D 5ρ 3

(.)

where Np = power number, P = impeller power in watts, ρ = density of tank liquid in kg/m3, n = shaft speed in revolutions/second and D=impeller diameter in meters. Because of the difficulty in obtaining many of these values, power numbers can be considered the summary of various correlated test results (when dealing with standard-sized mixing tank) rather than a precise specification. Therefore, manufacturers often specify an impeller's power number as a function of its power and size8.

1.5

Pumps

A pump is a device that moves fluids (liquids or gases), or sometimes slurries, by mechanical action. Pumps can be classified into three major groups according to the method they use to move the fluid: direct lift, displacement, and gravity pumps. Pumps operate by some mechanism (typically reciprocating or rotary), and consume energy to perform mechanical work by moving the fluid. Pumps operate via many energy sources, including manual operation, electricity, engines, or wind power, come in many sizes, from microscopic for use in medical applications to large industrial pumps. Mechanical pumps serve in a wide range of applications such as pumping water from wells, aquarium filtering, pond filtering and aeration, in the car industry for water-cooling and fuel injection, in the energy industry for pumping oil and natural gas or for operating cooling towers. In the medical industry, pumps are used for biochemical processes in developing and manufacturing

8

Engineering 360 powered by IEEE global spec.

17

medicine, and as artificial replacements for body parts, in particular the artificial heart and penile prosthesis. 

Single stage pump: When in a casing only one impeller is revolving then it is called single stage pump.



Multi stage pump: When in a casing two or more than two impellers are revolving then it is called double/multi stage pump.

Pumps are used throughout society for a variety of purposes. Early applications includes the use of the windmill or watermill to pump water. Today, the pump is used for irrigation, water supply, gasoline supply, air conditioning systems, refrigeration (usually called a compressor), chemical movement, sewage movement, flood control, marine services, etc. Because of the wide variety of applications, pumps have a plethora of shapes and sizes: from very large to very small, from handling gas to handling liquid, from high pressure to low pressure, and from high volume to low volume. Single Stage

Multi Stage

Figure 8

Centrifugal Pumps

1.5.1 Types of Pumps Pump types can be characterized as : 

Positive displacement pumps  Rotary positive displacement pumps  Reciprocating positive displacement pumps  Various positive displacement pumps  Gear pump  Screw pump  Progressing cavity pump  Roots-type pumps  Peristaltic pump  Plunger pumps  Triplex-style plunger pumps  Compressed-air-powered double-diaphragm pumps

18

 

  

 Rope pumps Impulse pumps  Hydraulic ram pumps Velocity pumps  Radial-flow pumps  Axial-flow pumps  Mixed-flow pumps  Jet pump Gravity pumps Steam pumps Valve less pumps

1.5.2 Axial-Flow Pumps vs. Centrifugal Pumps Axial flow pumps differ from radial flow in that the fluid enters and exits along the same direction parallel to the rotating shaft. The fluid is not accelerated but instead "lifted" by the action of the impeller. They may be likened to a propeller spinning in a length of tube. Axial flow pumps operate at much lower pressures and higher flow rates than radial flow pumps. A centrifugal pump is a roto-dynamic pump that uses a rotating impeller to increase the pressure and flow rate of a fluid. Centrifugal pumps are the most common type of pump used to move liquids through a piping system. The fluid enters the pump impeller along or near to the rotating axis and is accelerated by the impeller, flowing radially outward or axially into a diffuser or volute chamber, from where it exits into the downstream piping system. Centrifugal pumps are typically used for large discharge through smaller heads.

1.6

Some Physics on Rotating Disks Flow

In order to investigate the fluid flow in rotating frames, researchers performed various experiments. The basic idea is that the (viscous) fluid is confined between two rotating disks9. In general two boundary layers may be present. The problem is that the equations of motion are so complex, that no exact solutions are known for this problem even in the stationary regime (one disk fixed the other rotating). Therefore scientist have to make use of numerical simulations and various experiments to shed light on the physical mechanisms going on in the rotating fluid10. 1.6.1 Experimental Set-Up In order to study the flow between two rotating disks the experimental set-up shown in Figure 9 was built. The cell consists of a cylinder of small height h closed by a top disk and a bottom disk, both of radius R = 140 mm. The upper disk is made of glass and rotates together with the cylindrical sidewall which is made of PVC. The reason why the cylinder and top disk are made of PVC and glass is to allow visualization from above and from 9

Figure 9

Sketch of the experimental set-up

Miha Meznar, “Fluid Flows In Rotating Frames”, University of Ljubljana, March 2005. Here the focus is not on the recirculation flow but rather on the instability patterns in rotating fluids.

10

19

side. The bottom disk is made of rectified brass, with a black coating to improve visualization contrast. To allow the differential rotation the radius of the bottom disk is slightly smaller (a tenth of millimeter) than the radius of the shrouding cylinder. The thickness h of the cell can be varied between few mm up to several The cell is filled with a mixture of water, glycerol and small anisotropic flakes. The latter enable us to visualize the fluid flow. The flakes' orientation with the fluid leads to variations of the reflected light. For example, if the flakes are mainly horizontal, they reflect light, if they are vertical they do not reflect it so well. The kinematic viscosity ν = μ/ρ lies between 1x10−6 < ν < 8 x10−6 m2/s due to different concentration of glycerol11. Each of two disks rotate with its own angular velocity Ωi, where index i = b, where t stands for bottom and top disk respectively. Angular velocities of the disks range from 0 to 10 rad/s but the upper disk rotates anticlockwise only, whereas the bottom one can rotate clock- or anticlockwise. Anticlockwise rotation is taken positive. We call co-rotation the situation where both disks rotate in the same direction (b and t are of the same sign) and counter-rotation when the disks rotate in the opposite directions (they have opposite signs). If one of the disks is left fixed, the other rotating, the regime is called rotor-stator regime. We will define some dimensionless numbers that describe our cell. The first is radius-to-height ratio defined as Γ = R/h , where R is radius and h height of the cell. The second number is Reynolds number Rei = Ωih2/ν , where index i = b, t denotes the bottom and top disk respectively, i is the angular velocity of the disks and ν the kinematic viscosity. The last number is rotation ratio defined as s = Ωb/Ωt = Reb/Ret . Rotation ratio is positive (s > 0) in the co-rotation regime and negative (s < 0) in the counterrotation regime. 1.6.1.1 Recirculating flow Each rotation is associated with a meridian recirculating flow, which can be inward or outward depending on the rotation ratio. For arbitrary positive and small negative rotation ratio s, the radial recirculating flow is roughly the same as in the rotor-stator case (s = 0): it consists of an outward boundary layer close to the faster disk and an inward boundary layer close to the slower disk. At small negative rotation ratio the centrifugal effect of the slower disk is not strong enough to counteract the inward flow from the faster disk. But as the rotation ratio s is decreased below −0.2, the slower disk induces a centrifugal flow too, and the radial recirculating flow appears to come organized into two-cell recirculating structure as shown in Figure 7, 8. 11 At the interface of these two cells a strong shear layer takes place. The centrifugal flow induced by the faster disk recirculates towards the center of the slower disk due to the lateral end wall. This inward recirculation flow meets the outward radial flow induced by the slower disk, leading to a stagnation circle where the radial component of the velocity vanishes. 1.6.1.2 Instability flow patterns We now turn to the instability patterns of the flow between two rotating disks close to each other (Γ = 20.9), in both co- and counter-rotating flows. For s ≥ 0 (rotor-stator or co-rotation) and Reb fixed, on increasing Ret, propagating circular structures are first observed. These axisymmetric vortices appear close to the landrail wall, propagate towards the center and disappear before reaching the center of the cell. Above a secondary threshold of Ret, spiral structures appear at the periphery of the disks, and circles remain confined between two critical radii (Figure 10 (a)). These spirals are called positive spirals (denoted S+) since they roll up to the center in the direction of the faster disk (here the top one). Increasing Ret further, positive spirals progressively invade the whole cell. Still increasing Ret, the flow becomes more and more disordered (denoted D, Figure 10 (c)). G. Gauthier, P. Gondret, F. Moisy and M. Rabaud, “Instabilities in the flow between co- and counter-rotating disks”, J. Fluid Mech, volume 473, pp. 1-21, 2002. 11

20

It can be shown that co-rotation shifts upwards the instability thresholds for circles and positive spirals12. However, threshold line for circles is parallel to the solid body rotation (b = t) indicating that the angular velocity difference Ω = Ωt − Ωb is the only control parameter of this instability and no influence of the global rotation occurs. By contrast, the borderline for the positive spirals has a larger

Figure 10

For s ≥ 0 co-rotation at different speed

slope than the solid body rotation line; in this case the relative angular velocity Ω is not the only control parameter and an extra velocity of the upper disk is needed for the spirals to arise. The global rotation in this case has a stabilizing effect. For s < 0 (counter-rotating case) the onset of the instability patterns depends on the Reynolds numbers of both disks. For low bottom Reynolds number, −11 < Reb < 0, on increasing the Reynolds number of the upper disk, the appearance of the instability patterns is the same as in the rotor-stator or co-rotation case: axisymmetric propagating vortices, positive spirals and disorder. But, for −18 < Reb < −11, spirals of a new kind appear on increasing Ret. These spirals are said to be negative (and denoted S−) since they now roll up to the center in the direction of the slower counter-rotating disk (Figure 11 (a)). Unlike circles and positive spirals, negative spirals extend from the periphery to the center, they invade the whole cell. Also, the onset time for negative spirals is much longer than for

Figure 11 12

For s < 0 counter-rotating at different speed

Miha Meznar, “Fluid Flows In Rotating Frames”, University of Ljubljana, March 2005.

21

positive ones or circles; when the onset is carefully approached from below, the growth time of negative spirals can exceed 15 minutes which strongly contrasts circles and positive spirals which appear almost instantaneously. Increasing Ret further, positive spirals appear as well at the periphery of the disk, as can be seen in Figure 11 (b). Here negative and positive spirals seem to coexist without strong interaction, which indicates the difference in their origin. The circles and positive spirals have their origin in the boundary layer instability whereas negative ones, on the other hand, originate from shear layer instability. Still increasing Ret, negative spirals disappear and positive spirals alone remain (Figure 11(c)). Increasing Ret yet further, circles appear as in the co-rotation case. Still increasing Ret, the structures become disorganized and the flow becomes turbulent. For Reb < −18 the negative spirals described above become wavy, the flow is more and more disorganized and continuously becomes turbulent without a well-defined threshold. Depending on the Reynolds number, the disorder can be generated first at the periphery or in the center and then invades the entire cell. Up to now our instability patterns were limited to radius-to-height ratio Γ = 20.9. Does anything changes if one changes it? Researchers enlarged the gap h between the disks (Γ diminishes) and observed a new pattern that consisted of a sharp-cornered polygon of m sides, surrounded by a set of 2m outer spiral arms. These polygons arise only for small Γs (less than approx. Γ = 10). For higher values the vertical confinement leads to a saturated pattern where inner arms, connecting the corners of the polygon to the center of polygons, turn into negative spirals. Another interesting property of the patterns is that they are not fixed but rather rotate as a whole. Therefore we define the azimuthal phase velocity ωφ in the laboratory frame. It corresponds to the angular velocity of the global rotation of the spiral pattern. For the S+ spirals ωφ is always positive (anticlockwise), i.e. the positive spirals rotate in the direction of the faster (top) disk, regardless of motion of the bottom one. S− spirals, on the other hand change sign of ωφ. It means that for small Ret the pattern rotates in the direction of the slower (bottom) disk while at higher Ret it moves with the top (faster) disk. Here only compare the directions of the disks and phase velocity. The size of phase velocity is only a fraction of the disk velocities. We see that the co-rotation flow (Reb > 0, right-hand part of the diagram) is qualitatively the same as the rotor-stator flow (vertical line Reb = 0); the thresholds of instabilities (circles C and positive spirals S+) are found to increase just with the bottom Reynolds number. By contrast, the counter-rotating case (Reb < 0, left-hand part) is much more rich.

22

2

Conservation of Angular Momentum

2.1 Flow in Rotating Reference Frame Consider a coordinate system which is rotating steadily with angular velocity ω (bold face represents the vector quantity in picture) relative to a stationary (inertial) reference frame, as illustrated in Figure 12. The origin of the rotating system is located by a position vector r013.

Figure 12

Rotating Frame of Reference

The fluid velocities can be transformed from the stationary frame to the rotating frame using the following relation:

ur  u  ω r 

where

 ω  ωa

(.)

whirl velocity

In the above, ur is the relative velocity (the velocity viewed from the rotating frame), v is the absolute velocity (the velocity viewed from the stationary frame), ω x r is the whirl (or moving) velocity (the velocity due to the moving frame), and â is unit directional vector depending or rotation direction. When the equations of motion are solved in the rotating reference frame, the acceleration of the fluid is augmented by additional terms that appear in the momentum equations14. Moreover, the equations can be formulated in two different ways:  

Expressing the momentum equations using the relative velocities as dependent variables (known as the relative velocity formulation). Expressing the momentum equations using the absolute velocities as dependent variables in the momentum equations (known as the absolute velocity formulation).

The exact forms of the governing equations for these two formulations will be provided in the sections below. It can be noted here that pressure-based solvers provide the option to use either of 13 14

FLUENT 6.3 User's Guide. G. K. Batchelor. An Introduction to Fluid Dynamics. Cambridge Univ. Press, Cambridge, England, 1967.

23

these two formulations, whereas the density-based solvers always use the absolute velocity formulation. 2.2.1 Relative Velocity Formulation For the relative velocity formulation, the governing equations of uid ow for a steadily rotating frame can be written as follows:

ρ  .( ρu r )  0 t  M omentum ( ρu r )  .( ρu r u r )  ρ(2ω  u r  ω  ω  r )  p  τ ijr  F    t Centripetal M ass

Coriolis

Energy

 ( ρEr )  .( ρu r H r )  .(kT  τ ijr .u r )  Sh t p 1 p E r  h   u 2r  (ω  r ) 2 , H r  E r  ρ 2 ρ





Here the momentum equation contains two additional acceleration terms, the Coriolis acceleration (2ωxur), and the Centrifugal acceleration (ωxωxr). In addition, the viscous stress τijr is defined as before except that relative velocity derivatives are used. The energy equation is written in terms of the relative internal energy (Er) and the relative total enthalpy (Hr), also known as the rothalpy15. 2.2.2 Absolute Velocity Formulation For the absolute velocity formulation, the governing equations of uid ow for a steadily rotating frame can be written as follows:

ρ  .( ρu r )  0 t  M omentum ( ρu)  .( ρu r u)  ρ(ω  u)  p  τ ij  F  t I  Energy ( ρE )  .( ρu r H  p(ω  r )  .(kT  τ ij .u)  Sh t M ass

In this formulation, the Coriolis and Centripetal accelerations can be collapsed into a single term (I). Be advised that from now on we will be dealing with linear momentum if noted otherwise16.

2.3

Modeling Flows with Rotating Reference Frames (MRF)

By default, the equations of fluid flow and heat transfer are solves in a stationary (or inertial) reference frame. However, there are many problems where it is advantageous to solve the equations in a moving (or non-inertial) reference frame. Such problems typically involve moving parts (such as 15 16

FLUENT 6.3 User's Guide. Same as prvious.

24

rotating blades, impellers, and similar types of moving surfaces), and it is the flow around these moving parts that is of interest. In most cases, the moving parts render the problem unsteady when viewed from the stationary frame. With a moving reference frame, however, the flow around the moving part can (with certain restrictions) be modeled as a steady-state problem with respect to the moving frame. The moving reference frame modeling capability allows you to model problems involving moving parts by allowing you to activate moving reference frames in selected cell zones. When a moving reference frame is activated, the equations of motion are modified to incorporate the additional acceleration terms which occur due to the transformation from the stationary to the moving reference frame. By solving these equations in a steady-state manner, the flow around the moving parts can be modeled. For simple problems, it may be possible to refer the entire computational domain to a single moving reference frame. This is known as the single reference frame (or SRF) approach. The use of the SRF approach is possible, provided the geometry meets certain requirements17. For more complex geometries, it may not be possible to use a single reference frame. In such cases, you must break up the problem into multiple cells zones, with well-defined interfaces between the zones. The manner in which the interfaces are treated leads to two approximate, steady-state modeling methods for this class of problem:   

Single Reference Frame (SRF) Multiple Reference Frame (MRF) Mixing Plane Method (MPM)

If unsteady interaction between the stationary and moving parts is important, you can employ the Sliding Mesh approach to capture the transient behavior of the flow. 2.3.1 Single Rotating Reference Frame (SRF) Modeling Many problems permit the entire computational domain to be referred to as a single rotating reference frame (SRF modeling). In such cases, the equations for a Rotating Reference Frame are solved in all fluid cell zones. Steady-state solutions are possible in SRF models provided suitable boundary conditions are prescribed. In particular, wall boundaries must adhere to the following requirements: 

Any walls which are moving with the reference frame can assume any shape. An example would be the blade surfaces associated with a pump impeller. The no slip condition is defined in the relative frame such that the relative velocity is zero on the moving walls.



Walls can be defined which are non-moving with respect to the stationary coordinate system, but these walls must be surfaces of revolution about the axis of rotation. Here the so slip condition is defined such that the absolute velocity is zero on the walls. An example of this type of boundary would be a cylindrical wind tunnel wall which surrounds a rotating propeller.

Rotationally periodic boundaries may also be used, but the surface must be periodic about the axis of rotation. As an example, it is very common to model through a blade row on a turbomachine by assuming the flow to be rotationally periodic and using a periodic domain about a single blade. This permits good resolution of the flow around the blade without the expense of model all blades in the blade row (see Figure 13). Flow boundary conditions (inlets and outlets) can be in most cases prescribed in either the stationary or rotating frames. For example, for a velocity inlet, one can specify 17

FLUENT 6.3 User's Guide.

25

either the relative velocity or absolute velocity, depending on which is more convenient. In some cases (e.g. pressure inlets) there are restrictions based upon the velocity formulation which has been chosen. For additional information, reader should refer to FLUENT 6.3 user manual. 2.3.2 Flow in Multiple Rotating Reference Frames (MRF) Many problems involve multiple moving parts or contain stationary surfaces which are not surfaces of Figure 13 Single Blade Model with Rotationally Periodic revolution (and therefore cannot Boundaries be used with the Single Reference Frame modeling approach). For these problems, you must break up the model into multiple fluid/solid cell zones, with interface boundaries separating the zones. Zones which contain the moving components can then be solved using the moving reference frame equations, whereas stationary zones can be solved with the stationary frame equations. The manner in which the equations are treated at the interface lead to two approaches: 

Multiple Reference Frame model (MRF) & Mixing Plane Model (MPM)



Sliding Mesh Model (SMM)

Both the MRF and Mixing plane approaches are steady-state approximations, and differ primarily in the manner in which conditions at the interfaces are treated. These approaches will be discussed in following sections. The sliding mesh model approach is, on the other hand, inherently unsteady due to the motion of the mesh with time. The MRF model is, perhaps, the simplest of the two approaches for multiple zones. It is a steady-state approximation in which individual cell zones move at different rotational and/or translational speeds. The flow in each moving cell zone is solved using the moving reference frame equations. If the zone is stationary (ω = 0), the stationary equations are used. At the interfaces between cell zones, a local reference frame transformation is performed to enable flow variables in one zone to be used to calculate fluxes at the boundary of the adjacent zone. The MRF Interface Formulation. It should be noted that the MRF approach does not account for the relative motion of a moving zone with respect to adjacent zones (which may be moving or stationary); the grid remains fixed for the computation. This is analogous to freezing the motion of the moving part in a specific position and observing the instantaneous flow field with the rotor in that position. Hence, the MRF is often referred to as the frozen rotor approach. While the MRF approach is clearly an approximation, it can provide a reasonable model of the flow for many applications. For example, the MRF model can be used for turbomachinery applications in which rotor-stator interaction is

26

relatively weak, and the flow is relatively uncomplicated at the interface between the moving and stationary zones. In mixing tanks, for example, since the impeller-baffle interactions are relatively weak, large-scale transient effects are not present and the MRF model can be used. Another potential use of the MRF model is to compute a flow field that can be used as an initial condition for a transient sliding mesh calculation. This eliminates the need for a startup calculation. The multiple reference frame model should not be used, however, if it is necessary to actually simulate the transients that may occur in strong rotor-stator interactions, the sliding mesh model alone should be used.

Figure 14

Mixing Tank geometry with one

rotating impeller 2.3.2.1 Case Study – Mixing Tank In a mixing tank with a single impeller, you can define a rotating reference frame that encompasses the impeller and the flow surrounding it, and use a stationary frame for the flow outside the impeller region. An example of this configuration is illustrated in Figure 14. (The dashes denote the interface between the two reference frames). Steady-state flow conditions are assumed at the interface between the two reference frames. That is, the velocity at the interface must be the same (in absolute terms) for each reference frame. The grid does not move. You can also model a Figure 15 Mixing Tank with two rotating impellers problem that includes more than one rotating reference frame. Figure 15 shows a geometry that contains two rotating impellers side by side. This problem would be modeled using three reference frames: the stationary frame outside both impeller regions and two separate rotating reference frames for the two impellers. (As noted above, the dashes denote the interfaces between reference frames.)

2.3.3 The MRF Interface Formulation The MRF formulation that is applied to the interfaces will depend on the velocity formulation being used. The specific approaches will be discussed below for each case. It should be noted that the interface treatment applies to the velocity and velocity gradients, since these vector quantities change with a change in reference frame. Scalar quantities, such as temperature, pressure, density,

27

turbulent kinetic energy, etc., do not require any special treatment, and thus are passed locally without any change. 2.3.2.1 Interface Treatment: Relative Velocity Formulation In implementation of the MRF model, the calculation domain is divided into subdomains, each of which may be rotating and/or translating with respect to the laboratory (inertial) frame. The governing equations in each subdomain are written with respect to that subdomain's reference frame. Thus, the flow in stationary and translating subdomains is governed by Continuity and Momentum Equations, while the flow in rotating subdomains is governed Figure 16 Interface Treatment for the MRF Model by the equations presented in Equations for a Rotating Reference Frame. At the boundary between two subdomains, the diffusion and other terms in the governing equations in one subdomain require values for the velocities in the adjacent subdomain (see Figure 16). To enforce the continuity of the absolute velocity, u, is to provide the correct neighbor values of velocity for the subdomain under consideration. (This approach differs from the mixing plane approach described previously; The Mixing Plane Model, where a circumferential averaging technique is used). When the relative velocity formulation is used, velocities in each subdomain are computed relative to the motion of the subdomain. Velocities and their gradients are converted from a moving reference frame to the absolute inertial frame using following equation. For a translational velocity ut, we have

u  u r  (ω  r)  u t 

,

u  u r  (ω  r)

(.)

Swirl Velocity

Note that scalar quantities such as density, static pressure, static temperature, species mass fractions, etc., are simply obtained locally from adjacent cells. 2.3.3.2 Interface Treatment: Absolute Velocity Formulation When the absolute velocity formulation is used, the governing equations in each subdomain are written with respect to that subdomain's reference frame, but the velocities are stored in the absolute frame. Therefore, no special transformation is required at the interface between two subdomains. Again, scalar quantities are determined locally from adjacent cells.

2.4

The Mixing Plane Model (MPM)

The mixing plane model provides an alternative to the multiple reference frame and sliding mesh models for simulating flow through domains with one or more regions in relative motion. The Multiple Reference Frame Model, the MRF model is applicable when the flow at the boundary between adjacent zones that move at different speeds is nearly uniform (mixed out). If the flow at this boundary is not uniform, the MRF model may not provide a physically meaningful solution. The sliding mesh model (Sliding Mesh Theory) may be appropriate for such cases, but in many situations it is not practical to employ a sliding mesh. For example, in a multistage turbomachine, if the number

28

of blades is different for each blade row, a large number of blade passages is required in order to maintain circumferential periodicity. Moreover, sliding mesh calculations are necessarily unsteady, and thus require significantly more computation to achieve a final, time-periodic solution. For situations where using the sliding mesh model is not feasible, the mixing plane model can be a costeffective alternative. In the mixing plane approach, each fluid zone is treated as a steady-state problem. Flow-field data from adjacent zones are passed as boundary conditions that are spatially averaged or mixed at the mixing plane interface. This mixing removes any unsteadiness that would arise due to circumferential variations in the passage-to-passage flow field (e.g., wakes, shock waves, separated flow), thus yielding a steady-state result. Despite the simplifications inherent in the mixing plane model, the resulting solutions can provide reasonable approximations of the time-averaged flow field. 2.4.1 Rotor and Stator Domains Consider the turbomachine stages shown schematically in Figure 17 and Figure 18. In each case, the stage consists of two flow domains: the rotor domain, which is rotating at a prescribed angular velocity, followed by the stator domain, which is stationary. The order of the rotor and stator is arbitrary (that is, a situation where the rotor is downstream of the stator is equally valid). In a numerical simulation, each domain will be represented by a separate mesh. The flow information between these domains will be coupled at the mixing plane interface (as shown in Figure 18 and Figure 17) using the mixing plane model. Note that you may couple any number of fluid zones in this manner; for example, four blade passages can be coupled using three mixing planes. Note that the stator and rotor meshes do not have to be conformal; that is, the nodes on the stator exit boundary do not have to match the nodes on the rotor inlet boundary. In addition, the meshes can be of different types (e.g., the stator can have a hexahedral mesh while the rotor has a tetrahedral mesh).

Figure 17

Mixing Plane concepts as applied to axial rotation

29

2.4.2 The Mixing Plane Concept The essential idea behind the mixing plane concept is that each fluid zone is solved as a steady-state problem. At some prescribed iteration interval, the flow data at the mixing plane interface are averaged in the circumferential direction on both the stator outlet and the rotor inlet boundaries. By performing circumferential averages at specified radial or axial stations, profile of flow properties can be defined. These profiles which will be functions of either the axial or the radial coordinate, depending on the orientation of the mixing plane are then used to update boundary conditions along the two zones of the mixing plane interface. In Figure 18 Mixing Plane concepts applied to radial rotation the examples shown in Figure 18 and Figure 17, profiles of averaged total pressure (p0), direction cosines of the local flow angles in the Radial, Tangential, and Axial directions (αr; αt; Up Stream Down Stream αz), total temperature (T0), turbulence kinetic energy Pressure Outlet Pressure Inlet (k), and turbulence dissipation rate (ε) are computed at Pressure Outlet Velocity Inlet the rotor exit and used to update boundary conditions Pressure Outlet Mass flow Inlet at the stator inlet. Likewise, a profile of static pressure (ps), direction cosines of the local flow angles in the Table 1 Prescribed Boundary zone for radial, tangential, and axial directions (αr ; αt ; αz), are Mixing Plane computed at the stator inlet and used as a boundary condition on the rotor exit. Passing profiles in the manner described above assumes specific boundary condition types have been defined at the mixing plane interface. The coupling of an upstream outlet boundary zone with a downstream inlet boundary zone is called a mixing plane pair. In order to create mixing plane pairs, the boundary zones must be as prescribed as Table 1. 2.4.3

Mixing Plane Algorithm

The basic mixing plane algorithm can be described as follows:    

Update the flow field solutions in the stator and rotor domains. Average the flow properties at the stator exit and rotor inlet boundaries, obtaining profiles for use in updating boundary conditions. Pass the profiles to the boundary condition inputs required for the stator exit and rotor inlet. Repeat steps 1-3 until convergence.

Note that it may be desirable to under-relax the changes in boundary condition values in order to prevent divergence of the solution (especially early in the computation).

30

2.4.3.1 Mass Conservation across the Mixing Plane Note that the algorithm described above will not rigorously conserve mass flow across the mixing plane if it is represented by a pressure inlet and pressure outlet mixing plane pair. If you use a mass flow inlet and pressure outlet pair instead, we will force mass conservation across the mixing plane. The basic technique consists of computing the mass ow rate across the upstream zone (pressure outlet) and adjusting the mass flux profile applied at the mass flow inlet such that the downstream mass flow matches the upstream mass ow. This adjustment occurs at every iteration, thus ensuring rigorous conservation of mass ow throughout the course of the calculation. Also note that, since mass flow is being fixed in this case, there will be a jump in total pressure across the mixing plane. The magnitude of this jump is usually small compared with total pressure variations elsewhere in the flow field. Other quantities which will be conserved across Mixing Plane are Swirl and Total Enthalpy.

2.5

Sliding Mesh Modeling

In sliding meshes, the relative motion of stationary and rotating components in a rotating machine will give rise to unsteady interactions. These interactions are illustrated in Figure 19, and generally classified as follows:    

Potential interactions: flow unsteadiness due to pressure waves which propagate both upstream and downstream. Wake interactions: flow unsteadiness due to wakes from upstream blade rows, convecting downstream. Shock interactions: for transonic/supersonic ow unsteadiness due to shock waves striking the downstream blade row.

Where the multiple reference frame (MRF) and mixing plane (MP) models, are models that are applied to steady-state cases, thus neglecting unsteady interactions, the sliding mesh model cannot neglect unsteady interactions. The sliding mesh model accounts for the relative motion of stationary and rotating components. 2.5.1 Sliding Mesh Theory When a time-accurate solution for rotor-stator interaction Figure 19 Illustration of Unsteady Interactions (rather than a time-averaged solution) is desired, you must use the sliding mesh model to compute the unsteady flow field. As mentioned in Section 10.1: Introduction, the sliding mesh model is the most accurate method for simulating flow in multiple moving reference frames, but also the most computationally demanding. Most often, the unsteady solution that is sought in a sliding mesh simulation is time periodic. That is, the unsteady solution repeats with a period related to the speeds of the moving domains. However, you can model other types of transients, including translating, sliding mesh zones (e.g., two cars or trains passing in a tunnel). Reminder that for flow situations where there is no interaction between stationary and

31

moving parts (i.e., when there is only a rotor), the computational domain can be made stationary by using a rotating reference frame. (ω = 0). When transient rotor-stator interaction is desired (as in the examples in Figure 20 (a) and Figure 20 (b), you must use sliding meshes. If you are interested in a steady approximation of the interaction, you may use the multiple reference frame model or the mixing plane model, as described before.

(a) Rotor-Stator Interaction

Figure 20

(b) Blower

Examples of transient interaction using sliding mesh

2.5.2 The Sliding Mesh Technique In the sliding mesh technique two or more cell zones are used. (If you generate the mesh in each zone independently, you will need to merge the mesh profiles prior to starting the calculation. Each cell zone is bounded by at least one interface zone where it meets the opposing cell zone. The interface zones of adjacent cell zones are associated with one another to form a grid interface. The two cell zones will move relative to each other along the grid interface. Be advised that the grid interface must be positioned so that it has fluid cells on both sides. For example, the grid interface for the geometry shown in Figure 21(c) must lie in the fluid region between the rotor and stator; it cannot be on the edge of any part of the rotor or stator. During the calculation, the cell zones slide (i.e., rotate or translate) relative to one another along the grid interface in discrete steps. To recap, topological Mesh Changes in Sliding Interface are: 

Defined by a master and slave surfaces.



As surfaces move relative to each other, perform mesh cutting operations and replace original faces with facets.



Re-assemble mesh connectivity on all cells and faces touching the sliding surface: fully connected 3-D mesh.



Once the mesh is complete, there is no further impact!



Connectivity across interface changes with relative motion (see Figure 21 9(a-d)).

32

Figure 21 (a) and Figure 21 (b) show the initial position of two grids and their positions after some translation has occurred. For an axial rotor/stator configuration, in which the rotating and stationary parts are aligned axially instead of being concentric (see Figure 21 (d)), the interface will be a planar sector. This planar sector is a cross-section of the domain perpendicular to the axis of rotation at a position along the axis between the rotor and the stator.

(b) Sliding mesh

(a) Initial position

(c) Rotor /Starter interactions Figure 21

(d) Linear grid interface

Initial position and some translation with Sliding Interface

Figure 21

2.5.3 Sliding Mesh Concept As discussed before, the sliding mesh model allows adjacent grids to slide relative to one another. In doing so, the grid faces do not need to be aligned on the grid interface. This situation requires a means of computing the flux across the two non-conformal interface zones of each grid interface. To compute the interface flux, the intersection between the interface zones is determined at each new time step. The resulting intersection produces one interior zone (a zone with fluid cells on both sides) and one or more periodic zones. If the problem is not periodic, the intersection produces one interior zone and a pair of wall zones (which will be empty if the two interface zones intersect entirely), as shown in Figure 22(a). (You will need to change these wall zones to some other appropriate boundary type.) The resultant interior zone corresponds to where the two interface zones overlap; the resultant periodic zone corresponds to where they do not. The number of faces in these intersection zones will vary as the interface zones move relative to one another. Principally, fluxes across the grid interface

33

are computed using the faces resulting from the intersection of the two interface zones, rather than from the interface zone faces themselves. In the example shown in Figure 22 (b), the interface zones are composed of faces A-B and B-C, and faces D-E and E-F. The intersection of these zones produces the faces a-d, d-b, b-e, etc. Faces produced in the region where the two cell zones overlap (d-b, b-e, and e-c) are grouped to form an interior zone, while the (a) Zones Created by NonPeriodic Interface Intersection

(b) Two-Dimensional Grid Interface

Figure 22

Dynamic Interface Zones

remaining faces (a-d and c-f) are paired up to form a periodic zone. To compute the flux across the interface into cell IV, for example, face D-E is ignored and faces d-b and b-e are used instead, bringing information into cell IV from cells I and III, respectively.

34

3

Elements of Turbomachinery

3.1

Background

Turbomachinery is widely used equipment in industry such as compressors and turbines in a jet engine; steam turbine in power plants, propeller for ships, hydraulic turbines for irrigation, wind turbines for green energy, small fans for cooling, and so on18. A common feature of these devices is that they all work with fluid and have rotating component. Gorla19 gives a general definition of turbomachinery which says “Turbomachinery is a device in which the energy transfer occurs between a flowing fluid and a rotating element due to dynamic action, and results in a change in pressure and momentum of the fluid”. The usage of turbomachinery has a long history. It is

Axial Flow Devices Flow Direction

Centrifugal Flow Devices Mixed Flow Devices

Wind Turbine

Comprssible

Gas Turbine

Turbomachines

Steam Turbine

Fluid Physics

Pumps Incompressible Hydroulic Turbine Figure 23

Classification of Turbomachines

Xiaodong Wang, “CFD Simulation of Complex Flows in Turbomachinery and Robust Optimization of Blade Design”, Submitted to the Department of Mechanical Engineering Doctor of Philosophy, July 2010. 19 R. S. R. Gorla. Turbomachinery: Design and Theory. CRC Press, 2003. 18

35

recorded that the waterwheel, a kind of primitive turbomachinery, was invented and used for power generation more than hundred years ago. Although the configuration is simple, it does follow the same basic principle with other complicated modern turbomachinery’s, for instance the compressor and the gas turbine in a jet engine. Figure 23 represents classification of turbomachines. Here we concern with axial devices mainly. As the air is compressed in compressor before entering the combustion chamber where it is mixed with fuel and combustion occurs (a.k.a., aggravated stage). Then the gas with high pressure and high temperature flows through gas turbines and leaves the engine through a nozzle. While expanding through the turbine blades, power is released from the gas and drives the turbine rotating. This constitutes the modern gas turbine engine phenomena to be discussed next.

3.2

Historical Perspectives

The gas turbine is an internal combustion (IC) engine that uses air as the working fluid. It is the production of hot gas during fuel combustion, not the fuel itself that the gives gas turbines the name. Gas turbines can utilize a variety of fuels, including natural gas, fuel oils, and synthetic fuels. Combustion occurs continuously in gas turbines, as opposed to reciprocating IC engines, in which combustion occurs intermittently. The engine extracts chemical energy from fuel and converts it to mechanical energy using the gaseous energy of the working fluid (air) to drive the engine and propeller, which, in turn, propel the airplane. The gas turbine engine was first invented in the 1930s∼1940s, which gave the opportunity of rapid development to turbomachinery. From the initial turbojet engine to the modern turbofan engine with large bypass ratio, the evolution of jet engine requires more advanced compressors and turbines with higher stage pressure ratio and higher efficiency. Since 1988, the military of USA launched a series of research projects to develop advanced turbines, such as “IHPTET” (Integrated High Performance Turbine Engine Technology), “VAATE” (Versatile Affordable Advanced Turbine Engines) etc. The primary goal is to double the thrust-toweight ratio (TWR) of engine which will reach to 15∼20, decrease the fuel consumption ratio by 15%∼30%. Compressor and turbine are two core components of jet engine. The performance of a jet engine strongly depends on the design level of compressor and turbine. Therefore, significant researching efforts have been spent on improving the performance of turbomachinery. Today, the modern compressor stage has an efficiency of about 90% and the modern turbine stage has an efficiency of up to 95%. Further improvements become more and more difficult and require much deeper understanding of the flow field inside of the turbomachinery. Meanwhile, in industrial field, steam turbine and gas turbine are the main instruments of power generation. Due to the energy crisis, design of advanced turbine with higher efficiency is much more crucial than ever before. Therefore, similar strong demands of improving the performance of turbomachinery are also brought forward. While a turbine transfers energy from a fluid to a rotor, a compressor transfers energy from a rotor to a fluid. These two types of machines are governed by the same basic relationships including Newton's second Law of Motion and Euler's energy equation for compressible fluids 20.

3.3

Modern Turbomachinery as related to Gas Turbine Engine

In general, the rotating element is named rotor which is usually composed of one or several rows of rotating blades. There also exits a stator which is also composed of rows of blades, but not rotating. A pair of stator and rotor constitutes a stage. According to the way of energy transfer, turbomachines are generally divided into two main categories. The first category is used primarily to generate power which is called Turbine, including steam turbines, gas turbines and hydraulic turbines. The main function of the second category is to increase the total pressure of the working fluid by consuming power which includes compressors, pumps and fans as detailed in Figure 24. According to inlet and outlet flow directions, turbomachines can be classified into two types: axial turbomachinery and 20

See previous.

36

radial turbomachinery. However, here we concern only focuses on the axial turbomachinery. More detail classification and description about the configurations can be found in21. Considerable progress in development and application of CFD for aero-engines internal flow systems has been made in recent years. CFD is regularly used in industry for assessment of air systems, and performance of CFD for basic axisymmetric rotor/rotor and stator/rotor disc cavities with radial through flow is largely understood and documented. In cooperation with 3D geometrical features and calculation of unsteady flow are becoming common place. Automation of CFD, coupling with thermal models of solid components, is current area of development. A wide variety of flow phenomena, which are coupled in nature, occur in Turbomachinery CFD ranging from shock surfaces,

Figure 24

Component of Turbomachines and their Thermodynamic (Brayton cycle) properties

boundary layer, secondary flow, and vortex generating from blade tip and hob. These, makes the flow analysis of turbo-machinery extremely complex and CFD limited. The number of turbine stages varies in different types of engines, with high bypass ratio engines tending to have the most turbine stages. The number of turbine stages can have a great effect on how the turbine blades are designed for each stage. Many gas turbine engines are twin spool designs, meaning that there is a high pressure spool and a low pressure spool. The high pressure turbine is exposed to the hottest, highest pressure air, and the low pressure turbine is subjected to cooler, lower pressure air. The difference in conditions leads to the design of high pressure and low pressure turbine blades that are significantly different in material and cooling choices even though the aerodynamic and thermodynamic principles are the same. Under these severe operating conditions inside the gas and steam turbines, the blades face high temperature, high stresses, and potentially high vibrations. Steam turbine blades are critical components in power plants which convert the linear motion of high temperature and high pressure 21

M. T. Schobeiri. Turbomachinery: Flow Physics and Dynamic Performance. Springer, Berlin, 2005. 2, 37, 38

37

steam flowing down a pressure gradient into a rotary motion of the turbine shaft. Figure 25 illustrates of a twin spool jet engine. The high pressure turbine is connected by a single spool to the high pressure compressor (purple) and the low pressure turbine is connected to the low pressure compressor by a second spool (green)22.

Figure 25

Twin Pool Jet Engine

3.4 How does it work? Gas turbines are comprised of three primary sections mounted on the same shaft: the compressor, the combustion chamber (or combustor) and the turbine, as described above. The compressor can be either axial flow or centrifugal flow. Axial flow compressors are more common in power generation because they have higher flow rates and efficiencies. Axial flow compressors are comprised of multiple stages of rotating and stationary blades (or stators) through which air is drawn in parallel to the axis of rotation and incrementally compressed as it passes through each stage. The acceleration of the air through the rotating blades and diffusion by the stators increases the pressure and reduces the volume of the air. Although no heat is added, the compression of the air also causes the temperature to increase23. The compressed air then mixed with fuel injected through nozzles. The fuel and compressed air can be pre-mixed or the compressed air can be introduced directly into the combustor. The fuel-air mixture ignites under constant pressure conditions and the hot combustion products (what we like to call: aggravated gases) are directed through the turbine where it expands rapidly and imparts rotation to the shaft. The turbine is also comprised of stages, each with a row of stationary blades (or nozzles) to direct the expanding gases followed by a row of moving blades. The rotation of the shaft drives the compressor to draw in and compress more air to sustain continuous combustion. The remaining shaft power is used to drive a generator which produces electricity. Approximately 55-65 % of the power produced by the turbine is used to drive the compressor. To optimize the transfer of kinetic energy from the combustion gases to shaft 22 23

From Wikipedia, the free encyclopedia. J., López, Digital & Content Marketing Specialist, Wärtsilä Finland Oy.

38

rotation, gas turbines can have multiple compressor and turbine stages. Because the compressor must reach a certain speed before the combustion process is continuous – or self-sustaining – initial momentum is imparted to the turbine rotor from an external motor, static frequency converter, or the generator itself. The compressor must be smoothly accelerated and reach firing speed before fuel can be introduced and ignition can occur. Turbine speeds vary widely by manufacturer and design, ranging from 2,000 revolutions per minute (rpm) to 10,000 rpm. Initial ignition occurs from one or more spark plugs (depending on combustor design). Once the turbine reaches self-sustaining speed above 50% of full speed; the power output is enough to drive the compressor, combustion is continuous, and the starter system can be disengaged. Simply put, in a compressor, to raise the pressure, the fluid must be slowed down as it passes through a blade row. In a turbine, to drop the pressure, the fluid must be accelerated as it passes through a blade row. By having alternate stationary and moving blade rows and making use of the change of frame of reference, it is possible to always slow down (relative to the blade row) or always speed up the fluid. For example: In a turbine the flow is accelerated in the stator (stationary blade row). However, because the rotor row is moving, the flow appears to be moving more slowly in the relative frame and so can be reaccelerated in the relative frame. This appears to be a deceleration in the absolute frame24.

1.5

Gas Turbine Performance

The thermodynamic process used in gas turbines is the Brayton cycle. Two significant performance parameters are the pressure ratio and the firing temperature. The fuel-to-power efficiency of the engine is optimized by increasing the difference (or ratio) between the compressor discharge pressure and inlet air pressure. This compression ratio is dependent on the design. Gas turbines for power generation can be either industrial (heavy frame) or aero derivative designs. Industrial gas turbines are designed for stationary applications and have lower pressure ratios – typically up to 18:1. Aero derivative gas turbines are lighter weight compact engines adapted from aircraft jet engine design which operate at higher compression ratios up to 30:1. They offer higher fuel efficiency and lower emissions, but are smaller and have higher initial (capital) costs. Aero derivative gas turbines are more sensitive to the compressor inlet temperature. The temperature at which the turbine operates (firing temperature) also impacts efficiency, with higher temperatures leading to higher efficiency. However, turbine inlet temperature is limited by the thermal conditions that can be tolerated by the turbine blade metal alloy. Gas temperatures at the turbine inlet can be 1200°C to 1400°C, but some manufacturers have boosted inlet temperatures as high as 1600°C by engineering blade coatings and cooling systems to protect metallurgical components from thermal damage. Because of the power required to drive the compressor, energy conversion efficiency for a simple cycle gas turbine power plant is typically about 30 percent, with even the most efficient designs limited to 40 %. A large amount of heat remains in the exhaust gas, which is around 600˚C as it leaves the turbine. By recovering that waste heat to produce more useful work in a combined cycle configuration, gas turbine power plant efficiency can reach 55 to 60 percent. However, there are operational limitations associated with operating gas turbines in combined cycle mode, including longer startup time, purge requirements to prevent fires or explosions, and ramp rate to full load.

3.6

Gas Compressors

A gas compressor is a mechanical device that increases the pressure of a gas by reducing its volume. An air compressor is a specific type of gas compressor. Compressors are similar to pumps: both increase the pressure on a fluid and both can transport the fluid through a pipe. As gases are compressible, the compressor also reduces the volume of a gas. Liquids are relatively incompressible; 24

University of Cambridge, Compressor and Turbine stages.

39

Axial Dynamic Centrifugal

Single Acting

Reciprocating

Compressor Types

Double Acting Diaphram

Positive Displacement

Vane Scroll Rotery

Liquid Ring Screw Lobe

Figure 26

Gas Compressor Types

while some can be compressed, the main action of a pump is to pressurize and transport liquids. The main types of gas compressors are illustrated in Figure 26. where here we deal with two commonly used Axial and Centrifugal compressors. 3.6.1 Axial-flow compressors The dynamic rotating compressors that use arrays of fan-like airfoils to progressively compress a fluid. They are used where high flow rates or a compact design are required. The arrays of airfoils are set in rows, usually as pairs: one rotating and one stationary. The rotating airfoils, also known as blades or rotors, accelerate the fluid. The stationary airfoils, also known as stators or vanes, decelerate and redirect the flow direction of the fluid, preparing it for the rotor blades of the next stage (see Figure 27). Axial compressors are almost always multi-staged, with the crosssectional area of the gas passage diminishing along the compressor to maintain an optimum axial Mach number. Beyond about 5 stages or a 4:1 design pressure ratio a compressor will not function unless fitted with features such as stationary vanes with variable angles (known as variable inlet guide vanes and variable stators), the ability to allow some air to escape part-way along the compressor (known as inter-stage bleed) and Figure 27 Schematics of Axial Compressor being split into more than one rotating assembly (known as twin spools, for example). Axial compressors can have high efficiencies; around 90% at their design conditions. However, they are relatively expensive, requiring a large number of

40

components, tight tolerances and high quality materials. Axial-flow compressors are used in medium to large gas turbine engines, natural gas pumping stations, and some chemical plants. 3.6.2 Centrifugal Compressors Centrifugal compressors use a rotating disk or impeller in a shaped housing to force the gas to the rim of the impeller, increasing the velocity of the gas. A diffuser (divergent duct) section converts the velocity energy to pressure energy. They are primarily used for continuous, stationary service in industries such as oil refineries, chemical and petrochemical plants and natural gas processing plants.[1][14][15] Their application can be from 100 horsepower (75 kW) to thousands of horsepower. With multiple staging, they can achieve high output pressures greater than 10,000 psi (69 MPa). Many large snowmaking operations (like ski resorts) use this type of compressor. They Figure 28 A single stage Centrifugal are also used in internal combustion engines as Compressor superchargers and turbochargers. Centrifugal compressors are used in small gas turbine engines or as the final compression stage of medium-sized gas turbines. (see Figure 28).

3.6

Nomenclature of Terms

Before going further, it is prudent to get familiarize our self with terminology used in industry regarding components of turbomachines25. From personal experience, it is an important issue. Some of these are shown in Error! Reference source not found. and shown alphabetically in Table 2 below. Table 2

Glossary of Turbomachinery Terms

aspect ratio

ratio of the blade height to the chord

axial chord axial solidity

Length of the projection of the blade, as set in the turbine, onto a line parallel to the turbine axis. It is the axial length of the blade. Ratio of the axial chord to the spacing.

adiabatic

insulated; occurring with no external heat transfer

blade exit angle

Angle between the tangent to the camber line at the trailing edge and the turbine axial direction. radius at the tip minus the radius at the hub

blade height blade inlet angle blower bucket

angle between the tangent to the camber line at the leading edge and the turbine axial direction Rotary machine that produces a low-to-moderate pressure rise in a compressible fluid (usually air), usually incorporated in a duct. See "fan" and "compressor." same as rotor blade

David Gordon Wilson; "The Design of High-Efficiency Turbomachinery and Gas Turbines", pp 487-492, published by the MIT Press, Cambridge, Massachusetts, 1984, 5th printing 1991. 25

41

camber angle camber line CBE CBEX chord chord line compressor deflection deviation angle diffuser EGV effectiveness efficiency

External angle formed by the intersection of the tangents to the camber line at the leading and trailing edges. It is equal to the sum of the angles formed by the chord line and the camber-line tangents Mean line of the blade profile. It extends from the leading edge to the trailing edge, halfway between the pressure surface and the suction surface Compressor-burner-expander, or the "simple" gas-turbine "cycle." Compressor (heat exchanger)-burner-expander-heat exchanger, or the "regenerated," "recuperated," or "heat-exchanger" gas-turbine "cycle." Length of the perpendicular projection of the blade profile onto the chord line. It is approximately equal to the linear distance between the leading edge and the trailing edge. Two-dimensional blade section were laid convex side up on a flat surface, the chord line is the line between the points where the front and the rear of the blade section would touch the surface. rotary machine that produces a relatively high pressure rise (pressure ratios greater than 1.1) in a compressible fluid Total turning angle of the fluid. It is equal to the difference between the flow inlet angle and the flow exit angle the flow exit angle minus the blade exit angle A duct or passage shaped so that a fluid flowing through it will undergo an efficient reduction in relative velocity and will therefore increase in (static) pressure. at the exit of the compressor consisting of another set of vanes further diffuses the fluid and controls its velocity entering the combustors and is often known as the Exit Guide Vanes (EGV) term applied here to define the heat-transfer efficiency of heat exchangers

flow exit angle

Performance relative to ideal performance. There are many types of efficiency requiring very precise definitions A property of a substance defined in terms of other properties. Its change during a process is of more interest than its absolute value. In an adiabatic process, the increase of entropy indicates the magnitude of losses occurring A rotary machine that produces shaft power from a flow of compressible fluid at high pressure discharged at low pressure. Here the only types of expander treated are turbines angle between the fluid flow direction at the blade exit and the machine axial direction

flow inlet angle

angle between the fluid flow direction at the blade inlet and the machine axial direction

head hub

the height to which a fluid would rise under the action of an incremental pressure in a gravitational field the portion of a turbomachine bounded by the inner surface of the flow annulus

hub-tip ratio

same as hub-to-tip-radius ratio

IGV

An additional row of stationary blades that frequently used at the compressor inlet and are known as Inlet Guide Vanes (IGV) to ensure that air enters the first-stage rotors at the desired flow angle, these vanes are also pitch variable thus can be adjusted to the varying flow requirements of the engine ratio of the hub radius to the tip radius

entropy expander

hub-to-tip radio incident angle intensive property

the flow inlet angle minus the blade inlet angle Property that does not increase with mass; for instance, the pressure and temperature of a body of material do not double if an equal mass at the same temperature and pressure is joined to it. (The energy, on the other hand, would double.)

42

intercoolers isentropic

heat exchangers that cool a gas after initial compression and before subsequent compression occurring at constant entropy

isothermal

occurring at constant temperature

leading edge

the front, or nose, of the blade

mean section

the blade section halfway between the hub and the tip

meridional plane nozzle blade

a plane cutting a turbomachine through a diametric line and the (longitudinal) axis

pitch

the distance in the direction of rotation between corresponding points on adjacent blades The concave surface of the blade. Along this surface, pressures are highest

pressure surface pump radius ratio recuperator regenerated cycle regenerator reheat reheat combustor root

same as stator blade, for turbines only

A machine that increases the pressure or head of a fluid. In connection with turbomachinery it usually refers to a rotary machine operating on a liquid. same as hub-to-tip-radius ratio a heat exchanger, defined in this book as one with nonmoving surfaces, transferring heat from a hot fluid to a cold fluid See "CBEX." a heat exchanger, defined in this book as one having moving surfaces or valves switching the hot and cold flows The effect of losses in increasing the outlet enthalpy, or in decreasing the steam wetness, in a steam-turbine expansion. Also see "reheat combustor." a combustor fitted between two turbines to bring the gas temperature at inlet to the second turbine to approach the temperature at inlet to the first

rotor

The compressor or turbine-blade section attaching it to its mounting platform. Rotor blade root sections are normally at the hub, and stator- blade roots at the shroud the rotating part of a machine, usually the disk or drum plus the rotor blades

rotor blade

a rotating blade

separation shroud

when a fluid flowing along a surface ceases to go parallel to the surface but flows over a near-stagnant bubble, or an eddy, or over another stream of fluid the surface defining the outer diameter of a turbomachine flow annulus

solidity

the ratio of the chord to the spacing

spacing

same as pitch

stagger angle

the angle between the chord line and the turbine axial direction (also known as the setting angle) the condition of operation (usually defined by the incidence) of an airfoil, or row of airfoils, at which the fluid deflection begins to fall rapidly and/or the fluid losses increase rapidly conditions or properties of fluids as they would be measured by instruments moving with the flow

stall static (conditions) stator stator blade

the stationary part of a machine, normally that part defining the flow path A stationary blade.

43

suction surface

The convex surface of the blade. Along this surface, pressures are lowest

surge

the unstable operation of a high-pressure-ratio compressor whose stalls propagate upstream from the high-pressure stages or components allowing reverse flow and the discharge of the reservoir of high-pressure fluid, followed by re-establishment of forward flow and a repetition of the sequence. The outermost section of the blade or "vane."

tip total (conditions) trailing edge

conditions or properties of fluids as they would be measured by stationary instruments that bring the fluid isentropically to rest

transverse plane turbine

the plane normal to the axis of a turbomachine

turbomachines working fluid

3.7

the rear, or tail, of the blade

A rotary machine that produces shaft power by extracting energy from a stream of fluid passing through it, using only fluid-dynamic forces (as distinct from "positive displacement" or piston-and-cylinder-like machines). As for "turbine," except that the shaft power may be produced or absorbed, and the energy may be extracted from or added to a stream of fluid. Fluid that undergoes compression, expansion, heating, cooling, and other processes in a heat-engine cycle. In an open-cycle gas turbine the working fluid is air

Component of Gas Turbine Engine

3.7.1 Inlet The air inlet duct must provide clean and unrestricted airflow to the engine26. Clean and undisturbed inlet airflow extends engine life by preventing erosion, corrosion, and Foreign Object Damage (FOD). Consideration of atmospheric conditions such as dust, salt, industrial pollution, foreign objects (birds, nuts and bolts), and temperature (icing conditions) must be made when designing the inlet system. Fairings should be installed between the engine air inlet housing and the inlet duct to ensure minimum airflow losses to the engine at all airflow conditions. The inlet duct assembly is usually designed and produced as a separate system rather than as part of the design and production of the engine.

26

“Fundamentals of Gas Turbine Engines”, Cast-Safty.org.

44

Figure 29

Blade related terminology

3.7.2 Axial Compressor The compressor is responsible for providing the turbine with all the air it needs in an efficient manner. In addition, it must supply this air at high static pressures. The example of a large turboprop axial flow compressor will be used. The compressor is assumed to contain fourteen stages of rotor blades and stator vanes. The overall pressure ratio (pressure at the back of the compressor compared to pressure at the front of the compressor) is approximately 9.5:1. At 100% (>13,000) RPM, the engine compresses approximately 433 cubic feet of air per second. At standard day Figure 30 Compressor Flow Characteristics air conditions, this equals approximately 33 pounds of air per

45

Figure 31

Pressure and Velocity profile through a Multi-Stage Axial Compressor

second. The compressor also raises the temperature of the air by about 550F as the air is compressed and moved rearward. The power required to drive a compressor of this size at maximum rated power is approximately 7000 horsepower. In an axial flow compressor, each stage incrementally boosts the pressure from the previous stage. A single stage of compression consists of a set of rotor blades attached to a rotating disk, followed by stator vanes attached to a stationary ring. The flow area between the compressor blades is slightly divergent. Flow area between compressor vanes is also divergent, but more so than for the blades. In general terms, the compressor rotor blades convert mechanical energy into gaseous energy. This energy conversion greatly increases total pressure (PT). Most of the increase is in the form of velocity (V), with a small increase in static pressure (PS) due to the divergence of the blade flow paths. The stator vanes slow the air by means of their divergent duct shape, converting 'the accelerated velocity (V) to higher static pressure (PS). The vanes are positioned at an angle such that the exiting air is directed into the rotor blades of the next stage at the most efficient angle. This process is repeated fourteen times as the air flows from the first stage through the fourteenth stage. Figure 30 shows one stage of the compressor and a graph of the pressure characteristics as the air flows through the stage. The stator removes swirl from the flow, but it is not a moving blade row and thus cannot add any net energy to the flow. Rather, the stator rather converts the kinetic energy associated with swirl to internal energy (raising the static pressure of the flow). Thus typical velocity and pressure profiles through a multistage axial compressor look like those shown in Figure 30. Alternatively, assuming incompressible, constant density, and with no body force, we can use Bernoulli’s equations (Eq. 3.15; PT = PS + 1/2ρV2) where PT is the stagnation pressure, a measure of the total energy carried in the flow, p is the static pressure a measure of the internal energy, and the velocity terms are a measure of the kinetic energy associated with each component of velocity27. The rotor adds swirl to the flow, thus increasing the total energy carried in 27

MIT OpenCourseWare

46

the flow by increasing the angular momentum (adding to the kinetic energy associated with the tangential or swirl velocity, 1/2rv2). The stator removes swirl from the flow, but it is not a moving blade row and thus cannot add any net energy to the flow. Rather, the stator rather converts the kinetic energy associated with swirl to internal energy (raising the static pressure of the flow). Thus typical velocity and pressure profiles through a multistage axial compressor look like those shown in Figure 31. In addition to the fourteen stages of blades and vanes, the compressor also incorporates the inlet guide vanes and the outlet guide vanes. These vanes, located at the inlet and the outlet of the compressor, are neither divergent nor convergent. The inlet guide vanes direct air to the first stage compressor blades at the "best" angle. The outlet guide vanes "straighten" the air to provide the combustor with the proper airflow direction. The efficiency of a compressor is primarily determined by the smoothness of the airflow. During design, every effort is made to keep the air flowing smoothly through the compressor to minimize airflow losses due to friction and turbulence. This task is a difficult one, since the air is forced to flow into ever-higher pressure zones. Air has the natural tendency to flow toward low-pressure zones. If air were allowed to flow "backward" into the lower pressure zones, the efficiency of the compressor would decrease tremendously as the energy used to increase the pressure of the air was wasted. To prevent this from occurring, seals are incorporated at the base of each row of vanes to prevent air leakage. In addition, the tip clearances of the rotating blades are also kept at a minimum by the use of coating on the inner surface of the compressor case. All components used in the flow path of the compressor are shaped in the form of airfoils to maintain the smoothest airflow possible. Just as is the case for the wings of an airplane, the angle at which the air flows across the airfoils is critical to performance. The blades and vanes of the compressor are positioned at the optimum angles to achieve the most efficient airflow at the compressor’s maximum rated speed. Any deviation from the maximum rated speed changes the characteristics of the airflow within the compressor. The blades and vanes are no longer positioned at their optimum angles. Many engines use bleed valves to unload the force of excess air in the compressor when it operates at less than optimum speed. 28 The example engine incorporates four bleed valves at each of the fifth and tenth compressor stages. They are open until 13,000 RPM (~94% maximum) is reached, and allow some of the compressed air to flow out to the atmosphere. This results in higher air velocities over the blade and vane airfoils, improving the airfoil angles. The potential for airfoil stalling is reduced, and compressor acceleration can be accomplished without surge. 3.7.3 Diffuser All turbomachines and many other flow systems incorporate a diffuser (e.g. closed circuit wind tunnels, the duct between the compressor and burner of a gas turbine engine, the duct at exit from a gas turbine connected to the jet pipe, the duct following the impeller of a centrifugal compressor, etc.)29. Air leaves the compressor through exit guide vanes, which convert the radial component of the air flow out of the compressor to straight-line flow. The air then enters the diffuser section of the engine, which is a very divergent duct. The primary function of the diffuser structure is aerodynamic. The divergent duct shape converts most of the air’s velocity (Pi) into static pressure (PS) with the aid of Bernoulli equation. As a result, the highest static pressure and lowest velocity in the entire engine is at the point of diffuser discharge and combustor inlet. Other aerodynamic design considerations that are important in the diffuser section arise from the need for a short flow path, uniform flow distribution, and low drag loss. In addition to critical aerodynamic functions, the diffuser also provides: 

Engine structural support, including engine mounting to the nacelle

MIT, OpenCourseWare. Dixon, “Fluid Mechanics and Thermodynamics of Turbomachinery”, 5th edition, Senior Fellow at University of Liverpool, 1978-1998. 28

29 S. L.

47

 

 

Support for the rear compressor bearings and seals Bleed air ports, which provide pressurized air for:  Airframe "customer" requirements (air conditioning, etc.)  engine inlet anti-icing  control of acceleration bleed air valves Pressure and scavenge oil passages for the rear compressor and front turbine bearings. Mounting for the fuel nozzles.

The primary fluid mechanical problem of the diffusion process is caused by the tendency of the boundary layers to separate from the diffuser walls if the rate of diffusion is too rapid30. The result of too rapid diffusion is always large losses in stagnation pressure. On the other hand, if the rate of diffusion is too low, the fluid is exposed to an excessive length of wall and fluid friction losses become Pre-dominant. Clearly, there must be an optimum rate of diffusion between these two extremes for which the losses are minimized. 3.7.4 Nozzle In a large number of turbomachinery components the flow process can be regarded as a purely nozzle flow in which the fluid receives an acceleration as a result of a drop in pressure (see Figure 25). Such a nozzle flow occurs at entry to all turbomachines and in the stationary blade rows in turbines. In axial machines the expansion at entry is assisted by a row of stationary blades (called guide vanes in compressors and nozzles in turbines) which direct the fluid on to the rotor with a large swirl angle. Centrifugal compressors and pumps, on the other hand, often have no such provision for flow guidance but there is still a velocity increase obtained from a contraction in entry flow area. In reality, Nozzle and Diffuser work against each other. A nozzle increases the velocity of a fluid, while a diffuser decreases the velocity of a fluid. Nozzles can be used by jets and rockets to provide extra thrust. Conversely, many jet engines use diffusers to slow air coming into the engine for a more uniform flow. 3.7.5 Combustor Once the air flows through the diffuser, it enters the combustion section, also called the combustor. The combustion section has the difficult task of controlling the burning of large amounts of fuel and air. It must release the heat in a manner that the air is expanded and accelerated to give a smooth and stable stream of uniformly heated gas at all starting and operating conditions. This task combustion liners must position and control the fire to prevent flame contact with any metal parts. The engine under consideration here uses a can-annular combustion section with six combustion liners (cans). They are positioned within an annulus created by inner and outer combustion cases. Combustion takes place in the forward end or primary zone of the cans. Primary air (amounting to about one fourth of the total engine’s total airflow) is used to support the combustion process. The remaining air, referred to as secondary or dilution air, is admitted into the liners in a controlled manner (Figure 32). The secondary air controls the flame pattern, cools the liner walls, dilutes the temperature of the core gasses, and provides mass. This cooling air is critical, as the flame temperature is above 1930C (3500F), which is higher than the metals in the engine can endure. It is important that the fuel nozzles and combustion liners control the burning and mixing of fuel and air under all conditions to avoid excess temperatures reaching the turbine or combustion cases. Maximum combustion section outlet temperature (turbine inlet temperature) in this engine is about 1070C (>1950F). The rear third of the combustion liners is the transition section. The transition section has a very convergent duct shape, which begins accelerating the gas stream and reducing the static pressure in preparation for entrance to the turbine section.

30

See 13.

48

Figure 32

Combustor primary operating components

3.7.6 Axial Gas Turbine This example engine has a four-stage turbine. The turbine converts the gaseous energy of the air/burned fuel mixture out of the combustor into mechanical energy to drive the compressor, driven accessories, and, through a reduction gear, the propeller. The turbine converts gaseous energy into mechanical energy by expanding the hot, high-pressure gases to a lower temperature and pressure. Each stage of the turbine consists of a row of Figure 33 Turbine Flow Characteristics stationary vanes followed by a row of rotating blades. This is the reverse of the order in the compressor. In the compressor, energy is added to the gas by the rotor blades, then converted to static pressure by the stator vanes. In the turbine, the stator vanes increase gas velocity, and then the rotor blades extract energy. The vanes and blades are airfoils that provide for a smooth flow of the gases. As the airstream enters the turbine section from the combustion section, it is accelerated through the first stage stator vanes. The stator vanes (also called nozzles) form convergent ducts that convert the gaseous heat and pressure energy into higher velocity gas flow (V). In addition to accelerating the gas, the vanes "turn" the flow to direct it into the rotor blades at the optimum angle. As the mass of the high velocity gas flows across the turbine blades, the gaseous energy is converted to mechanical energy. Velocity, temperature, and pressure of the gas are sacrificed in order to rotate the turbine to generate shaft power. Figure 33 represents one stage of the turbine and the characteristics of the gases as it flows through the stage. A multi-stage turbine is illustrates in Figure 32. The efficiency of the turbine is determined by how well it extracts mechanical energy from the hot, high-velocity gasses. Since air flows from a high-pressure zone to a low pressure zone, this task is accomplished fairly easily. The use of properly positioned airfoils allows a smooth flow and expansion of gases through the blades and vanes of the turbine. All the air

49

must flow across the airfoils to achieve maximum efficiency in the turbine. In order to ensure this, seals are used at the base of the vanes to minimize gas flow around the vanes instead of through the intended gas path. In addition, the first three stages of the turbine blades have tip shrouds to minimize gas flow around the blade tips. We can apply the same analysis techniques to a turbine. Again, the stator does no work. It adds swirl to the flow, converting internal energy into kinetic energy. The turbine rotor then extracts work from the flow by removing the kinetic associated with the swirl velocity.

Figure 34

3.8

Schematics of axial flow Turbine

Difference in Blading between Compressor and Turbine

There is quite a difference between Compressor and Turbine blading. Aside from shape of it, they are number of stages and arrangement of it. While Compressor blades are generally thin and straight, and resemble a tiny rectangular wing with low Compressor camber thickness. Turbine • Area increase: pressure rise blades are more curved. In particularly large and • Flow deceleration: thick boundary layers recent engines, where • Little flow turning: many stages efficiency is critical, turbine blades will often be full of tiny holes for Turbine cooling effects. The difference best described • Area decrease: pressure drop below and examples of • Flow acceleration: thin boundary layers blade shown in Figure 35. To distinguish • Large flow turning: few stages between high pressure

50

and low pressure stages (compressor or turbine does not matter), the length of the blade and its torsion (i.e. how much the aerodynamic profile turns around the axis of the blade going from the root to the tip) are key: shorter and more twisted blades will be high pressure ones, longer and straighter blades will be low pressure. Note that two blades of the same length could come one from a high pressure stage and the other from a low pressure one of a different engine: "short" and "long" are relative to the engine size.

Typical Compressor Blade ( Air Defence Museum) Figure 35

3.8

Typical Turbine Blade

Examples of typical Blades for Compressor and Turbine

Velocity Triangles in Turbomachines

An important aspect of Turbomachinery is the velocity triangle and their goal to change the flow apparatus. It is basic vector relationship between relative and absolute frame. Velocity triangles are typically used to relate the flow properties and blade design parameters in the relative frame (rotating with the moving blades), to the properties in the stationary or absolute frame. It uses the study of first year Static, and by “unwrapping” the compressor. That is, we take a cutting plane at a particular radius (see Figure 36). Here we have assumed that the area of the annulus through which the flow passes is nearly constant and the

Figure 36

Velocity triangles for an Axial Compressor

51

density changes are small so that the axial velocity is approximately constant. Let’s examine the velocities of the gas, as it passes through a rotor and a stator. At the point we’re examining, the rotor is moving with a velocity U. The velocity of the gas relative to the rotor is denoted by C and V is absolute velocity or V = C + U. The angle between the flow velocity C and the shaft axis is denoted by α. The angle between the rotor blade angle and the shaft axis is denoted by β. The component of the velocity C in axial direction is denoted by Ca. It is assumed to be constant along the compressor. Notice the tangential velocity increase across the rotor for compressor. In some circles, they used W instead of C or W = V – U. In drawing these velocity diagrams it is important to note that the flow typically leaves the trailing edges of the blades at approximately the trailing edge angle in the coordinate frame attached to the blade (i.e. relative frame for the rotor, absolute frame for the stator). We will mainly look at axial compressors as they are the most used type of compressors. Also, axial compressors work very similar to axial turbines where stator gives tangential velocity, and rotor moves in the direction of tangential velocity, having work done on them by flow. Notice tangential velocity decrease across turbine rotors. (Figure 36).

3.9

Energy Exchange with Moving Blades

The Euler turbine equation relates the power added to or removed from the flow, to characteristics of a rotating blade row. The equation is based on the concepts of conservation of angular momentum and conservation of energy. They are both turbomachinery: machines that transfer energy from a rotor to a fluid, or the other way around. The working principle of the compressor and the turbine is therefore quite similar. 3.9.1 Euler’s equation for turbomachinery 31 Let’s examine a rotor, rotating at a constant angular velocity ω. The initial radius of the rotor is r 1, while the final radius is r2. A gas passes through the rotor with a constant velocity c. The rotor causes a moment M on the gas. The power needed by the rotor is thus P = Mω. It would be nice if we can find an expression for this moment M. For that, we first look at the force F acting on the gas. It is given by

dFu 

dmc   m c dt

(15.1)

Where we have used the assumption that c stays constant. Only the tangential component Fu contributes to the moment. Every bit of gas contributes to this tangential force. It does this according to

 dcu dFu  m

(15.2)

Where cu is the tangential velocity of the air. Let’s integrate over the entire rotor. We then find that 2

2

2

1

1

1

  r dc u  m  (cu,2 r2  c u,1 r1 ) M   dM   r dFu  m The power is now given by

31

“Compressor and turbines”, Aerostudents.

(15.3)

52

 (cu,2 r2  cu,1 r1 ) ω  m  (cu,2 u 2  cu,1 u1 ) P MωTωm

(15.4)

In this equation, T denotes Torque, u denotes the speed of the rotor at a certain radius r. We have also used the fact that ω = u1/r1 = u2/r2. The above equation is known as Euler’s equation for turbomachinery. From (Eq. 1.4) it is obvious that: 

If the tangential velocity increases across a blade row (where positive tangential velocity is defined in the same direction as the rotor motion) then work is added to the flow (a compressor).



If the tangential velocity decreases across a blade row (where positive tangential velocity is defined in the same direction as the rotor motion) then work is removed from the flow (a turbine).

Furthermore, another form of Euler’s Turbomachinery equation, with aid of the steady flow energy equation:

H2  H1  ω (cu,2 r2  cu,1 r1 )  Cp (T2  T1 ) where Cp  constant

(15.5)

It relates the temperature ratio (and hence the pressure ratio) across a turbine or compressor to the rotational speed and the change in momentum per unit mass. Note that the velocities used in this equation are what we call absolute frame velocities (as opposed to relative frame velocities).32 It is given fact that:

Figure 37 

32

Velocity triangles in relation to incident angle

If angular momentum increases across a blade row, then T2 > T1 and work was done on the fluid (a compressor).

MIT, OpenCourseWare.

53



3.10

If angular momentum decreases across a blade row, then T2 < T1 and work was done by the fluid (a turbine)

Compressors and their Reaction to Intake Distortion

During the design phase of an aircraft and its engine it is important that the compatibility aspects at the aerodynamic interface between the aircraft intake and the engine are given sufficient consideration because of the implications failures in this area may have33. On a macroscopic level and in isolation from other effects, the isentropic relation can be applied. Compressors, as the name implies, compress air by a repeated sequence of first adding kinetic energy to the flow and then converting the kinetic energy to pressure by a process of flow deceleration. The elements within a compressor achieving this process are a number of airfoils, either rotating or stationary. Work input to the flow by a rotor row is achieved via change of the angular momentum of the flow, and these properties are related to each other via the following equation,

H 2  H1  u 2 cu,2  u1 cu,1 where

   cwU

(15.6)

Especially for axial compressors where rotor angular velocities at rotor inlet and exit are very similar to each other, it is evident that an increase in total enthalpy requires changing the angular velocity of flow. Velocity triangles at rotor inlet and exit exemplified in Figure 37 show how angular flow velocities, rotor inlet flow angles and rotor exit flow angles are related to each other. The symbol “c” denotes velocity in the absolute frame of reference. Due to the rotational speed Figure 38 Compressor operating map “u” of the rotor, rotor blades experience flow velocities within their rotating (or relative) frame of reference, denoted by the symbol “w”. For the sake of simplicity, it is assumed that the flow at rotor inlet has no angular component (c u, 1 = 0), and the exit flow angle of the rotor blade remains unchanged (in the rotor frame of reference). With these assumptions, an increase in work input according to equation 1 can only be achieved by an increase of cu,2. According to the dependencies shown in Figure 37, this requires reducing the axial velocity component of the flow behind the rotor. Because of conservation of mass flow through the rotor, also the axial velocity at rotor inlet will be reduced, leading to an increased incidence of the flow to the Breuer, B., Bissinger, N., C., “Encyclopedia of Aerospace Engineering – Volume 8 - Chapter EAE 573-Basic Principles – Gas Turbine Compatibility – Gas Turbine Aspects”. 33

54

rotor blade. Translating the state of flow behind the rotor from the rotating frame of reference into the stationary one, Figure 37 also shows that an increase of work delivered to the flow by the rotor increases the incidence to the subsequent stator row as well. Therefore, an increase of work input to the flow means increasing incidences to both rotor and stator airfoils. Therefore, an increase of work input to the flow means increasing incidences to both rotor and stator airfoils. Very much like aircraft wings, these airfoils have certain operating limits in terms of airfoil angle of attack or incidence. With increasing incidence, rotor airfoils provide for a larger work input and hence pressure rise, but at the same time the aerodynamic loading increases, up to a point where the flow separates. On a larger scale, the pressure rise capability of a compressor is typically depicted using a compressor map where pressure rise is depicted as a function of compressor mass flow for different rotational speeds. An example map is provided with Figure 38, and for the sake of illustration, it also relates different regimes of compressor operating range to an aircraft operating at different angles of attack. At low pressure ratios, the airfoils operate with negative to small incidence, and usually elevated losses. When the pressure ratio is increased, airfoil incidences now approach a condition with minimum losses. Further increasing the pressure ratio is equivalent to further rise of airfoil aerodynamic loading and losses increase due to formation of regions of separated flow. At the upper end of a speed line, there is a point where regions of separated flow have enlarged to an extent where no further pressure rise is achievable, in analogy to aircraft wings reaching the stall limit where no further increase of lift can be provided34. The upper operational limit of a compressor map is called the surge line, representing a condition where large flow separation prevents further pressure rise. The surge line represents an operational limit for engine operation, since the occurrence of compressor surge (sometimes also referred to as compressor stall) leads to a highly unsteady flow field within the engine, quite often also entailing periods of reversed flow, that is air flowing in the “wrong” direction through the compressor. Surge is associated with large fluctuations of power output. Furthermore, it is accompanied by increased structural loads caused by the rapid changes of flow field state. Compressor maps are usually established (either numerically or by means of testing) for a standard set of inlet conditions. These inlet conditions are typically derived from simplified installation assumptions and assume a simplified inlet profile with radial variations only, but uniform in circumferential direction. Intake distortion considerations deal with conditions that deviate from these design assumptions and aim to identify the consequences of these deviations with regard to engine operation.

34

See 71.

55

3.11

Effects of Turbine Temperature

The materials used in the turbine section of the engine limit the maximum temperature at which a gas turbine engine can operate35. The first metal the hot gases from the combustion section strike is the turbine inlet. The temperature of the gas stream is carefully monitored to ensure that over temperature does not occur. Compromises are made in turbine design to achieve the optimum balance of power, efficiency, cost, engine life, and other factors. As an example, our sample engine can operate at a higher turbine inlet temperature than previous models due to improved materials and design. The higher temperature allows for increased power and improved efficiency while adding higher cost for the direct cooling of the first turbine stage airfoils and other components. Figure 39 shows the temperature, velocity and pressure variation across a gas turbine engine36.

Pressure

Temperature

Figure 39

Velocity

Sample engine Perssure, Velocity and Temperature variation

To increase the overall performance of the engine and reduce the specific fuel consumption, modern gas turbines operate at very high temperatures. However, the high temperature level of the cycle is limited by the melting point of the materials. Therefore, turbine blade cooling is necessary to reduce the blade metal temperature to increasing the thermal capability of the engine. Due to the contribution and development of turbine cooling systems, the turbine inlet temperature has doubled over the last 60 years. The cooling flow has a significant effect on the efficiency of the gas turbine. It has been found that the thermal efficiency of the cooled gas turbine is less than the uncooled gas turbine for the same input conditions (Figure 40). The reason for this is that the temperature at the inlet of turbine is decreased due to cooling and therefore, work produced by the turbine is slightly decreased. It is also known that the power consumption of the cool inlet air is of considerable concern

“Fundamentals of Gas Turbine Engines”, Cast-Safety.org. Shahrokh Sorkhkhah, “Gas Turbine Fundamentals”, Faculty of Karaj , Azad University Design Director of Iran Gas Turbine Company. 35 36

56

since it decreases the net power output of the gas turbine37-38. With this in mind, during the design phase of gas turbine it is very important to optimize the cooling flow if you are considering both the performance and reliability. Cooled Gas turbine design is quite complicated and requires not only the right methodology, but also the most appropriate design tools, powerful enough to predict the results accurately from thermodynamics cycle to aerothermal design, ultimately generating the 3D blade. Different cooling methods that are employed depend on the extent of the cooling required. The

Figure 40

Turbine Inlet Temperature27

cooling flow passes through several loops internally and is then ejected over the blade surface to mix with the main flow. The mixing of the cooling flow with the main flow alters the aerodynamics of the flow within the turbine cascade. The cooling flow that is injected into the main flow needs to be optimized, not only in terms of thermodynamic parameters, but also in terms of the locations to ensure the turbine vanes and blade surfaces are maintained well below the melting surface. The spacing between the holes, both in horizontal and vertical direction, affects not only the surface temperature of the blade, but also the strength of the blade and its overall life. Performing a 3D analysis for optimizing the flow, spacing, and location of cooling flow is computationally expensive. One has to resort to reduced order 1D flow and heat network simplifies the task of not only arriving at the optimal configuration of cooling holes and location, but also in aerothermal design of the gas turbine flow path and generation of the optimized 3D blades with reduced overall design cycle time. Designers are faced with the challenge of simplifying the complex 3D cooled blade and accurately modelling it.

37 Amjed Ahmed

Jasim AL-Luhaibi, Mohammad Tariq, “Thermal Analysis of Cooling Effect on Gas Turbine Blade”, eISSN: 2319-1163 | pISSN: 2321-7308. 38 Posted by: Abdul Nassar, “Optimizing the Cooling Holes in Gas Turbine Blades”, SoftInWay® Incorporated, 2016.

57

3.12

Compressor and Turbine Characteristics

The compressor has several important parameters. There are the mass flow m͘ , the initial and final temperatures T02 and T03, the initial and final pressures p02 and p03, the shaft speed ω (also denoted as N), the rotor diameter D, and so on39. Let’s suppose we’ll be working with different kinds of compressors. In this case, it would be nice if we could compare these parameters in some way. To do that, dimensionless parameters are used. By using dimensional analysis, we can find that there are four dimensionless parameter groups. They are

 RT02 m p 02D 2

,

p 03 , p 02

ωD RT02

and η

(15.7)

These parameter groups are known as the mass flow parameter group, the pressure ratio, the shaft speed parameter group and the efficiency. The efficiency can be either polytrophic or isentropic. (These two efficiencies depend on each other anyway). The relation between the four dimensionless parameters can be captured in a graph, known as a Figure 41 Characteristics Graph of a Compressor characteristic. An example of a characteristic is shown in Figure 41. When applying dimensional analysis to a turbine, the same results will be found. However, this time the initial and final pressures are p04 and p05. The initial and final temperatures are T04 and T05. 3.12.1 Stall 40 Let’s examine the air entering the rotor. Previously, we have assumed that this air has exactly the right angle of incidence “i” to follow the curvature of the rotor blade. In reality, this is of course not the case. In fact, if the angle of incidence is too far off, then the flow can’t follow the curvature of the rotor blades. The other phenomena associated with Stall is if there are pockets of low axial velocity covering one or two blade passages (see Figure 42). This is called stall and usually starts at one rotor blade. However, this stall alters the flow properties of the air around it. Because of this, stall spreads around the rotor. And it does this opposite to the direction of rotation of the rotor. This phenomenon is called rotating stall. Often, only the tips of the rotor blades are subject to stall. This is because the 39 40

MIT OpenCourseWare. See previous

58

velocity is highest there. This is called part span stall. If, however, the stall spreads to the root of the blade, then we have full span stall. For high compressor speeds ω, stall usually occurs at the last stages. On the other hand, for low compressor speeds, stall occurs at the first stages. Generally, the possibility of stalling increases if we get further to the left of the characteristic. (See also Figure 41). 3.12.1 Compressor Surge 41 Let’s suppose we control the Figure 42 Illustration of the propagation of a stall cell in the mass flow m˙ in a compressor, relative frame running at a constant speed ω. The mass flow m˙ effects the pressure ratio p03/p02. There can either be a positive or a negative relation between these two. Let’s examine the case where there is a negative relation between these two parameters. Now let’s suppose we increase the mass flow m˙. The pressure at the start of the compressor will thus decrease. However, the pressure upstream in the compressor hasn’t noticed the change yet. There is thus a higher pressure upstream than downstream. This can cause flow reversal in the compressor. Flow reversal itself is already bad. However, it doesn’t stop here. The flow reversal causes the pressure upstream in the compressor to drop. This causes the compressor to start running again. The pressure upstream again increases. Also, the mass flow increases. But this again causes the pressure downstream to increase. Flow reversal thus again occurs. A rather unwanted cycle has thus been initiated. This cyclic phenomenon is called surge. It causes the whole compressor to start vibrating at a high frequency (see Figure 43). Surge is different from stall, in that it effects the entire compressor. However, the occurrence of stall can often lead to surge. There are several ways to prevent surge. We can blow-off bleed air. Figure 43 Classical Compressor surge cycles This happens halfway through the compressor. This provides an escape for the air. Another option is to use variable stator vanes (VSVs). By adjusting the stator vanes, we try to make sure that we always have the correct angle of incidence i. Finally, the compressor can also be split up into parts. Every part will then have a different speed ω. Contrary to compressors, turbines aren’t subject to surge. Flow simply never tends to move upstream in a turbine.

41

MIT OpenCourseWare.

59

3.12.3 Choked Flow Let’s examine the pressure ratio p04/p05 in a turbine. Increasing this pressure ratio usually leads to an increase in mass flow m˙. However, after a certain point, the mass flow will not increase further. This is called choked flow42. It occurs, when the flow reaches supersonic velocities. Choked flow can also occur at the compressor. If we look at the right side of Figure 41, we see vertical lines. So, when we change the pressure ratio p03/p02 at constant compressor speed ω, then the mass flow remains constant.

42

See previous.

60

4 4.1

Primary Research in Turbomachinery Research Spectrum

The design of turbomachinery is a complex task due to the complicated flow phenomena and interaction of multi-disciplines which involves aerodynamics, heat transfer43, structural dynamic, control theory, materials and manufacture engineering etc. Among these design processes, aerodynamic analysis is the keystone of the design, which decides the performance of turbomachinery directly. While, without numerical technologies (CFD simulation and numerical optimization), it is impossible to meet the increasing rigorous requirements of design. Hence, the research on numerical aerodynamic analysis and numerical design of turbomachinery are outstandingly important. The aerodynamic performance of turbomachinery mainly depends on the complex internal flows which usually are strongly three dimensional, viscous and unsteady. Figure 44 shows the impact of CFD on SNECMA fan performance over a 30 year period (Escuret, 1998). The flows in blade passages may be laminar, Figure 44 Impact of CFD on SNECMA fan performance, over a turbulent and transitional, and period of 30 years may include wake flow, and secondary flows etc. In addition, there also may exist other complicated flow phenomena, such as transition, boundary layer separation, shock and shock-boundary layer interaction, the unsteady interaction between the blade rows, the interactions between the blade row and end-wall, etc. In 1999, a NASA report of “Numerical Simulation of Complex Turbomachinery Flows”44 stated four typical complex flows in turbomachinery which have been investigated extensively and may remain being the key research problems of turbomachinery in next few decades. These flows are:    

Unsteady flow Turbulence Film cooling Three dimensional flow in turbine including tip leakage effect

Xiaodong Wang, “CFD Simulation of Complex Flows in Turbomachinery and Robust Optimization of Blade Design”, Submitted to the Department of Mechanical Engineering Doctor of Philosophy at the Vrije Universiteit Brussel July 2010 44 X. D. Wang, Sh. Kang, “Solving stochastic burgers equation using polynomial chaos decomposition”, J. Eng. Therm., 31(3):393-398, 2010. (In Chinese) 43

61

4.2

Application of CFD in Turbomachinery

4.3

Quasi 3D flow (Q3D)

Accurate and robust turbomachinery off-design performance prediction remains elusive. Representation of transonic compression systems, most notably fans, is especially difficult, due in large part to highly three-dimensional blade design and the resulting flow field45. Complex shock structure and subsequent interactions (with blade boundary layers, end-walls, etc.) provide additional complications. Surely, turbomachinery design has benefited greatly from advancements in computational power and efficiency. However, practical limitations in terms of computational requirements, as well as limitations of turbulence and transition modeling, make it difficult to use CFD to analyze complex off-design issues. Accurate and robust turbomachinery off-design performance prediction remains elusive. Representation of transonic compression systems, most notably fans, is especially difficult, due in large part to highly three-dimensional blade design and the resulting flow field. Complex shock structure and subsequent interactions (with blade boundary layers, end-walls, etc.) provide additional complications. Surely, turbomachinery design has benefited greatly from advancements in computational power and efficiency. However, practical limitations in terms of computational requirements, as well as limitations of turbulence and transition modeling, make it difficult to use CFD to analyze complex off-design issues. For example, CFD analyses have only recently been used to explore the complex flow fields resulting from inlet distortion through modern multistage fans. The time-accurate investigation by Hah, et al, 1998, which included unsteady circumferential and radial variations of inlet total pressure, is one of the most complete in the open literature. Even so, Hah’s calculation was limited to two blade passages with boundary conditions just upstream and downstream of the first rotor of a two-stage fan. As discussed below, improvements to traditional numerical approaches are needed. With the development of computer technology, the Reynolds Averaged Navier-Stokes (RANS) simulations are developed rapidly since 1980s. In the same time, a couple of turbulence models are proposed successively to complete RANS model. In most design processes, the steady RANS simulations give satisfied prediction of overall performance. While in elaborate design processes, unsteady RANS (URANS) simulations are needed since the flows in turbomachinery are highly unsteady. Respecting to the approximation level of geometry, CFD simulation of turbomachinery developed from 2-D to 3D, from planar cascade to annular cascade, from single blade passage to whole ring, from single stage to multi stages. The increase of model accuracy to the real geometry has significant effects on turbomachinery design. Figure 44 Exhibits the impact of CFD on the performance improvement of aircraft engine in SNECMA (France) over a period of almost 30 years46. The evolution, from the initial use of simple 2-D potential flow models in the early 1970s to the current applications of full 3D Navier-Stokes code, has led to overall gain in efficiency close to 10 points47.

The definition Fully 3D methods replace the stream surface calculation of blade-to-blade (S1) and hub-to-tip (S2) stream surface was introduced by Wu48 , and this viewpoint dominated the subject until the early 1980s when fully three dimensional (3D) methods first became available. Wu’s static Boyer, K., M., “An Improved Streamline Curvature Approach for Off-Design Analysis of Transonic Compression Systems “, PhD. Dissertation, Virginia Polytechnic Institute and State University, 2001. 46 J. F. Escuret, D. Nicoud, and Ph. Veysseyre,”Recent advances in compressors aerodynamic design and analysis”, AVT TP/1, RTO/NATO, 1998. 47 Xiaodong Wang, “CFD Simulation of Complex Flows in Turbomachinery and Robust Optimization of Blade Design”, Submitted to the Department of Mechanical Engineering Doctor of Philosophy at the Vrije universiteit Brussel July 2010. 48 Wu, C. H. “A general through flow theory of fluid flow”, NACA paper TN2302, 1951. 45

62

pressure S1/S2 approach was far ahead of his time in that he saw flow velocity it as a method of solution for fully 3D flow. Wu’s ideas were considerably simplified by circumferential distance assuming that the S1 stream surfaces were surfaces of revolution (i.e. untwisted) while the S2 stream surfaces were reduced to a single mean stream surface that could be treated as an axisymmetric flow (Figure 45). The axisymmetric hub-to-tip (S2) calculation is often called the ‘Through flow calculation’ and has become the backbone of turbomachinery design, while the ‘blade-to-blade’ (S1) calculation remains the basis for defining the detailed blade shape. Fully 3D methods Figure 45 Illustration of S1 and S2 surfaces replace the stream surface calculation of blade-to-blade (S1) and hub-to-tip (S2) stream surface calations by a single calculation for the whole blade row. This removes the modelling assumptions of the quasi 3-D (Q3D) approach but requires far greater computer power and so was not usable as a design tool until the late 1980s. For similar reasons, early methods had to use coarser grids that introduced larger numerical errors than in the Q3D approach. Radial equilibrium and through-flow methods determine the meridional variations in the velocity field, but they assume that the turbomachinery flow field is axisymmetric. Cascade analysis and blade-to-blade computational methods consider the flow variations across the blade passages, but they neglect span wise variations and radial flows. These two views of a turbomachine are very useful and both are essential in the design process, but in reality the flow field in all axial turbomachinery, to some degree, varies in the axial, radial, and tangential directions. 4.3.1 Stream Surface of Second Kind - Through flow (S2) Through flow calculations can be used in design (or inverse) mode to determine blade inlet and exit angles and velocity variation from a specified span-wise work distribution, or in analysis (or direct) mode when blade angles are specified and flow angles, work, and velocity distributions are predicted. Through flow calculation programs are probably the most important tool of the turbine aerodynamic designer. At the initial design stage a one-dimensional mean line calculation might be used to obtain estimates of blade height and so to lay out a first approximation to the annulus line. Such mean line calculations usually include estimates of blade loss and deviation, so that predictions of turbine performance can be obtained, but these must be based only on the blade geometry mid-height so high accuracy cannot be expected. Although span wise variations in flow are small for very high radius ratio turbines these variations become significant at radius ratios below about 0.9. It is well known that most turbine blades are remarkably tolerant to off-design incidences (compared to compressor blades), but even so optimum performance, particularly at off-design conditions, cannot be expected unless the blades are matched to the span wise variation in flow. The main objective of a through flow calculation is, therefore, to provide a prediction of this span wise variation so that suitable blade profiles can be selected to cope with the variations in inlet angle, turning, Mach number, etc. The main problem encountered when developing through flow calculations for turbines, as opposed to compressors, arises from the need to be able to calculate the flow through stages with high-pressure ratio and in particular with regions of transonic relative flow. The latter is much more easily handled by Streamline Curvature methods (SCM) than by stream function methods although

63

severe difficulties arise even for the former type of method. Time-marching methods are much better suited to calculating transonic flow but are not yet highly developed further use in through flow calculations. Problems with calculating transonic flow are currently much more severe in steam turbines than in gas turbines. The traditional use of streamline curvature method (SCM) approaches, as most often discussed in the literature during the preliminary design phase, are discussed in detail in49. The stream surface represented by

s(r, ψ, z)  0

(16.1)

As depicted in Figure 46. The through-flow solver provides a preliminary blade shape, continually refined through solutions from higher-order and secondary flow models. One way to calculate a 3-D flow field is to solve two sets of equations, one dealing with axis-symmetric flow in the meridional plane, commonly referred to as the “S2” surface, and the other with blade-to-blade flow on a stream

Figure 46

Streamline Curvature method

surface of revolution, the “S1” plane (see Figure 45). The traditional formulation for the governing momentum equation(s) is a first-order velocity gradient representation, one in the radial and one in the tangential direction approach for off-design analysis along an axis-symmetric S2 surface. It is generally accepted that any streamline curvature solution technique will yield satisfactory flow solutions as long as the deviation, losses, and blockages are accurately predicted50. 4.3.3 Stream Surface of First Kind (Blade 2 Blade – S1) These methods calculate the flow on a blade-to-blade (S1) stream surface given the stream surface shape with the objective with an associated stream surface thickness and of designing the detailed blade profile. The stream surface is best thought of as a stream tube radius which are obtained from the through flow calculation. Accurate specification of the radius and thickness variation is essential as they can have a dominant effect on the blade surface pressure distribution. As with through flow methods the calculation may be in either direct (or analysis) mode, when the blade shape is Chung-Hua Wu, “A General Theory of Three Dimensional Flow in Subsonic and Supersonic Turbomachines of Axial-Radial- and Mixed Flow Types”, National Advisory Committee for Aeronautics, Technical Note 260, 1952. 50 Boyer, K., M., “An Improved Streamline Curvature Approach for Off-Design Analysis of Transonic Compression Systems “, PhD. Dissertation, Virginia Polytechnic Institute and State University, 2001. 49

64

prescribed and its surface pressure distribution calculated, or in inverse mode, where the required blade surface pressure distribution is prescribed and a blade shape is sought. Many different numerical methods have been developed for this task. Initially streamline curvature (to be discussed later) and stream function methods were popular, but both have difficulty coping be made to calculate transonic flows with weak shock with transonic flow and they have now largely been abandoned. Velocity potential methods can waves but they have seen limited use in turbomachinery. The numerical methods described above are inviscid and need to be coupled to a boundary layer calculation if they are to be used to predict blade loss. For com pressor blades the boundary layer blockage must be included in the inviscid calculation as it significantly affects the blade surface pressure distribution51. For most turbine blades the boundary layer is so thin that it may be calculated separately after obtaining the surface pressure distribution from an inviscid calculation. A recent alternative (N–S) equations which predict the boundary native to coupled inviscid/boundary layer calculations is the direct solution of the Navier– layer growth as part of the main calculation. These demand a much finer grid near to the blade surfaces than do inviscid calculations and so are considerably more ‘expensive’. Nevertheless the N–S equations for blade to-blade flow are now routinely solved as part of the design process, requiring only a few minutes CPU time on a modern workstation. There remains controversy about the best turbulence and transition models to use and about how many mesh points are necessary within the boundary layer. A variety of blade–to-blade solvers are currently available in the design system. They range from potential and streamline curvature method up to fully viscous, time marching solvers. The main use of the blade-to-blade codes is to ensure that the vector diagrams set by thorough Flow are achievable and within the bounds of blade thickness, loading and efficiencies. For examples, in turbine design the suction surface diffusion is taken as a primary indicator as to the condition of the boundary layer. The blade-to-blade code solves for the suction surface velocity ratio, or diffusion factor, and the geometry is adjusted accordingly. Most of these codes are very similar to those available in other design systems and have also been described elsewhere. However, three codes (TAYLOR, AEGIS and NOVAKED2D) are different and worth mentioning52. 4.3.2 Theory of Radial Equilibrium in Through Flow (Cr = 0) Consider a small element of fluid of mass dm shown in Figure 47, of unit depth and subtending an angle dθ at the axis, rotating about the axis with tangential velocity, cθ, at radius r. The element is in radial equilibrium so that the pressure forces balance the centrifugal forces (cr = 0):

dmc θ2 1   p  dpr  dr  dθ  p r dθ   p  dp  dr dθ  2  r 

(16.2)

Writing dm = ρ r dϴ dr and ignoring terms of 2nd order we obtain:

1 dp cθ2  ρ dr r

(16.3)

For an incompressible fluid and using thermodynamic relations the Radial Equilibrium Equation can be written as: Calvert, W. J. and Ginder, R. B., “Quasi-3D calculation system for the flow within transonic compressor blade rows”, ASME paper 85-GT-22, 1985. 52 Ian K. Jennions, “Elements of a Modern Turbomachinery Design System”, GE Aircraft Engines, One Neumann Way, MD X409, Cincinnati, OH 45215-6301,United States. 51

65

(16.4)

dh 0 c d ds dc rcθ  or  T  cx x  θ dr dr dr r dr c d dc rcθ   0 cx x  θ dr r dr dc 1 dp 0 1 dp dc   c x x  cθ θ or ρ dr ρ dr dr dr c d 1 dp 0 dc rcθ   cx x  θ ρ dr dr r dr

Equation (2.4) clearly states that equal work is delivered at all radii and the total pressure losses across a row are uniform with radius. It may be applied to two sorts of problem: the design (or indirect) problem, in which the Figure 47 Radial Equilibrium tangential velocity distribution is specified and the axial velocity variation is found, or the direct problem, in which the swirl angle distribution is specified, the axial and tangential velocities being determined.

4.4

Governing Equation of Rotating Frame of Reference

Accounting for the particular flow situation in turbomachinery, it is necessary to be able to describe the flow behavior relatively to a rotating frame of reference that is attached to the rotor. Without loss of generality, it is assumed that the moving part of turbomachinery is rotating steadily with angular velocity ω around the machine axis along which a coordinate z is aligned. Define u as absolute velocity, w is relative velocity, and v is as rotating system or blade ω⨯r, we have,

u 

 w  

v 

Absolute

Relative

Coordinate

 w  ωr

(16.5)

Introducing this into the mass conversation and after some manipulation we obtain,

rρ    ρw   0 t

(16.6)

Comparing with non-inertia frame of reference, it seems to keep the same expression where subscript r refers to the rotating frame of reference. Without causing confusion, the subscript r can be omitted in general. The total derivative (acceleration) is also can be redefined as

Du w v    w.w   2w ω ω v  Dt t t Centrifuga l Coriiolis

(16.7)

The first item on right-hand side expresses the local acceleration of the velocity field within the rotating frame of reference. The second term and third item denote the angular velocity acceleration and the convective term within the rotating frame of reference, respectively. While, the fourth item and last item are the Coriolis acceleration and the Centrifugal acceleration, respectively, which are fictitious forces produced as a result of transformation from stationary frame to rotating frame of

66

reference. Figure 48 shows the directions of the velocity and the acceleration, and relationship between the absolute velocity, relative velocity and rotation (Schobeiri, 2005). Substituting the acceleration in Eq. 16.7 distinctly, for an incompressible flow equations of motion and energy, in rotating frame of reference can be obtained:

Figure 48

Coriolis and Centripetal forces created by the Rotating Frame of Reference

Momentum:

Energy :

 ( w )  ( v)   w.(w )  ω  v  2ω  w  μw  p  F t t 2 2    w v  D ρ h   2 2   p       kT     τ  w   w F  q H Dt t

(16.7)

Which can written in scalar form of (r, ϴ, and z) with the aid of cylindrical coordinates. It should be noted that WF is the work of body forces in rotating frame of reference, F is the body force, while the subscript r is omitted here. The detailed derivation process of governing equations in rotating frame of reference can be found in Schobeiri53. Alternatively, we can choose more compact form of integral representation with arbitrary control volume V and differential surface area dA in a relative frame of reference rotating steadily with angular velocity ω:

dW T V d t dV   F  G dA  VS dV where W  ρ , ρu , ρE and F  [ρv, ρu  v  p I, ρEv  pu]T G  [0 , τ , τ  v  q]T

v  u  rω

(16.8)

S  [0 , ρω  u , 0]T

Here F, G and S are respectively, the inviscid flux, viscous flux, and source vectors, and τ, I are stress and identity tensors respectively. In addition, ρ, u, E, and p are the density, absolute velocity, total

53

M. T. Schobeiri, “Turbomachinery: Flow Physics and Dynamic Performance”, Springer, Berlin, 2005.

67

enthalpy, and pressure, respectively and v is the relative velocity. Extended details in available in54.

4.5

Efficiency effects in Turbomachinery55

In the turbomachinery context a large number of efficiencies are defined such as thermodynamic or mechanical efficiency. In the sections below the focus is put on the thermodynamic efficiencies. For a given change of state of a fluid the efficiency is defined as the ratio between actual change in energy to ideal change in energy in case of expansion or the inverse in case of compression,

actual change in energy ideal change in energy ideal change in energy Compression : η  actual change in energy Expansion : η 

(16.9)

4.5.1 Isentropic Efficiency Depending on which process is taken as ideal process efficiencies are referred to as isentropic or polytrophic efficiencies. In case of an isentropic efficiency the ideal process is represented by an isentropic change of state from start to end pressure, i.e. the same pressures as for the real process. This is illustrated in Figure 50 for an expansion process by means of an enthalpy-entropy diagram (h-s diagram). In the above depicted process the changes in total energy are referred to, which is expressed by indexing the efficiency by “tt”, i.e. “total-to-total”. With the aid of h0 = h + (1/2) c2 where c is the flow velocity, the total-to-total isentropic efficiency (expansion and compression) is thus given by

For Expansion :

η tt 

actual change in energy Δh 0 h 01  h 02   ideal change in energy Δh os h 01  h 02s

For Compression :

η tt 

ideal change in energy Δh 0s h 02s  h 01   actual change in energy Δh 0 h 02  h 01

Figure 50

Expansion process

Figure 49

(16.10)

Compression process

“Simulation of unsteady turbomachinery flows using an implicitly coupled onlinear harmonic balance method”, Proceedings of ASME Turbo Expo 2011, GT2011. 55 Damian Vogt,” Turbomachinery Lecture Notes”, 2007. 54

68

Note: For adiabatic real processes the entropy must always increase during the change of state. Due to this increase in entropy the real change in energy is smaller than the ideal during expansion. In other words, you get out less energy from the real process than you could have from an ideal one For the compression process the increase in entropy signifies that you need to put in more energy to compress a fluid than you would have in an ideal process Therefore the efficiency is always smaller or equal to unity The only way to reduce entropy would be to cool a process. However in such case we do no longer look into adiabatic processes. In certain cases the kinetic energy that is contained in the fluid (i.e. the amount of energy that is due to the motion) cannot be used at the end of a process. An example for such a process is the last stage of an energy producing turbine where the kinetic energy in the exhaust gases is not contributing to the total energy produced. In such case a so-called total-to-static isentropic efficiency is used, identified by indexing the efficiency by “ts”, i.e. “total-tostatic”. Note that it is necessary to include total and static states in this case. The total-to-total isentropic efficiency (expansion) is thus given by:

actual change in energy h 01  h 02 ηts    ideal change in energy h 01h 2s

1 c 22      c2 η 2h 0  Δh 0s  2  tt 2 Δh 0

1

(16.11)

This relation shows that for values of c2 > 0 the total-to-static efficiency is always smaller than the total-to-total efficiency. For further detailed aspects of efficiency in turbomachines the readers should consult with 56-57.

S.L. Dixon, B.Eng., PH.D., “Fluid Mechanics, Thermodynamics of Turbomachinery”, Senior Fellow at the University of Liverpool, UK. 57 Damian Vogt, “Efficiencies”, Turbomachinery Lecture Notes, 2007. 56

69

5 5.1

Complex flow in Turbomachinery Key Features of Transonic Fan (Turbine) Field

These features include highly 3-D flow fields, complex shock systems, and strong interactions between the shock, boundary layer, and secondary flows (like the tip-leakage vortex). The goal is to provide a basic understanding so that proper assessment of the chosen numerical approach can be performed. As suggested by Figure 51, the flow fields of fan designs are complex and highly threedimensional, and almost always unsteady. The flow-path hub contour shown in Figure 51 suggests

Figure 51

Complex Flow phenomena compressors

significant radial velocity components, especially at the fan entrance and strong interactions between the shock, boundary layer, and secondary flows (like the tip-leakage vortex). Secondary flows and their interactions with other phenomena are another major source of flow complexity. Indeed, Denton and Dawes, 1999, suggest the prediction of blade surface and end-wall corner separations to be one of the most challenging tasks of 3-D, viscous solvers, largely due to the obvious dependence on turbulence model. Additionally, the use of blade twist, sweep (viewed from the meridional plane) and lean (observed looking axially through the machine) contributes to the 3-D flow effects. A significant consideration in the design of transonic fan blades is the control of shock location and strength to minimize aerodynamic losses without limiting flow. Custom-tailored airfoil shapes are required to “minimize shock losses and to provide desired radial flow components. Figure 52 shows features of the tip section geometry typical of a transonic fan. The shape of the suction surface is key as it:

70

 

Influences the Mach number just ahead of the leading edge passage shock, and Sets the maximum flow rate.

As noted by Wisler, 1987, the cascade passage area distribution is chosen to provide larger-thancritical area ratios; thus, maximum flow is determined by the first captured Mach wave, location determined by the forward suction surface (induction surface). This maximum flow condition is often referred to as leading edge choke, or in cascade parlance, “unique incidence” (note that “unique” incidence is really a misnomer; here, “choking” incidence will be used). The flow induction surface and fan operating condition (incoming relative Mach number at the airfoil leading edge) set the average Mach number just ahead of the leading edge passage shock. A “traditional” convex suction surface results in a series of Prandtl-Meyer expansion waves as the flow accelerates around the leading edge. Increasing the average suction surface angle (relative to the incoming flow) ahead of the shock reduces the average Mach number, and presumably reduces the shock losses. Common for modern transonic fan tip sections is a concave induction surface, the so-called “pre-compression” airfoil. As indicated in previous chapter, there are four major area of research going on in turbomachinery, namely: Unsteady Flow, Film cooling, Turbulence and 3-D flow. We start with the unsteadiness first.

Figure 52

5.2

Fan Tip section geometry

Sources of Unsteadiness in Turbomachinery

Turbomachinery flows are among the most complex flows encountered in fluid dynamic practice (Lakshminarayana,)58. The internal flows within a blade passage of turbomachinery are strongly three dimensional, viscous flows which may include laminar flow, turbulent flow and transitional flow. Moreover, they are fully unsteady due to the interactions between blade rows in a stage or multistage machine. There also exist secondary flows including the flows due to passage vortices in Lakshminarayana, B. “An assessment of computational fluid dynamic techniques in the analysis and design of turbomachinery”, the 1990 freeman scholar lecture, J. Fluids Engineering Vol. 113(No. 3): 315-352, 1991. 58

71

the end-wall range, radial flow near blade surfaces, and tip leakage flow and leakage vortex, shock and shock boundary layer interaction in high speed conditions, wakes flows, even some specific flows, for instance film cooling flows nearby the cooling holes. The complexity is mainly reflected in the following areas: 1. Various forms of secondary flow caused by viscosity and complex geometry, which is dominated by vortex flows: passage, leakage, corner, trailing, horseshoe and scraping vortices, etc. These form three- dimensional and rotational nature of the flow. 2. Inherent unsteadiness (see below) due to the relative motion of rotor and stator blade rows in a multi stage environment. 3. The flow pattern in the near-wall region includes: laminar, transitional and turbulent flows; besides separated flows are often exist. 4. The flow may be incompressible, subsonic, transonic or supersonic; some turbomachinery flows include all these flow regimes. 5. Due to the limitation of flow space, there are strong interactions of the solid wall surfaces with above complicated phenomena. Besides, in gas turbines, the use of cooling gas makes the flow more complex. A good understanding of the unsteady flow in turbomachinery is necessary for advanced design as it shown in Figure 53 with broad spectrum. According to Greitzer59, the unsteady flow in turbomachinery can be classified into two groups: inherent unsteadiness and conditional unsteadiness. The conditional unsteadiness is mainly caused by the sudden changes of the working condition. For example when turbomachinery is working on the start stage, acceleration stage or offdesign condition, the fluctuation of working condition might lead to the unsteady rotating stall, surge, flutter and flow distortion of turbomachines. Sometimes, the distortion of inlet flow or the asymmetric outlet condition of vector nozzle also might lead to the unsteadiness. The inherent unsteadiness is mainly due to the relative motion and interaction between rotor and stator and, generally speaking, it could be divided as: 1. Interaction of potential flows in adjacent blade rows including Transient Fan. 2. Interaction between the wake flow and blade rows downstream. 3. Interaction between the secondary flows and blade rows. 4. Interaction wake-boundary layer. 5. Un-shrouded tip leakage flow interaction. 6. Film Cooling effects.

59

E. M. Greitzer, “Thermoaldynamics and fluid mechanics of turbomachinery”, AS1/E 9713, NATO, 1985.

72

Figure 53

5.3

Flow structures with 5 to 6 orders of magnitudes variations in length and time scales (LaGraff et al., 2006)

Interaction of Potential flows in adjacent blade rows

The first part comes from the changing of the relative position of rotor to stator which results in the periodic fluctuation of the pressure or shocks. This fluctuation is propagated both upstream and downstream as disturbance waves. 5.3.1 Interactions in Transonic Fan The shock structure associated with transonic fans is complicated by the 3-D nature of the flow field and operating range over which the fan must operate60. Figure 54 (A-B-C) illustrates some typical features – leading edge oblique shock, aft passage normal shock below peak efficiency, and a near-normal, detached bow shock near peak efficiency (and higher) loading conditions. Note that throughout this report, loading refers to flow turning. For high tip-speed fans (inlet relative Mach numbers greater than 1.4), the trend seems to be to design for an oblique leading edge shock through higher loading conditions (near and at peak efficiency). This trend seems reasonable given the continued need to reduce losses. Other flow field considerations in transonic fans include the interrelationship between the rotor tip-clearance vortex structure and passage shock, high Mach number stator flow, most notably in the hub region, and strong shock – boundary layer interaction.

Boyer, K., M., “An Improved Streamline Curvature Approach for Off-Design Analysis of Transonic Compression Systems “, PhD. Dissertation, Virginia Polytechnic Institute and State University, 2001. 60

73

A - Mach number contours

B - Install

C - Chocking

Figure 54

5.4

D - Near Pick Effeciency

Shock Structure in Transonic Fan

Interaction between Wake Flow and Blade Rows

The second part, unsteady wake, is a quite common flow phenomenon, not only in turbomachinery. Due to the thickness of the trailing edge of blade, the flows after the blade generate a high dissipation region, called wake, which is similar to the flow passed a circular cylinder where a famous wake flow Von Karman Vortex Street can be observed. When a viscous flow passes a cylinder or an airfoil, a regular vortex shedding can be found behind the cylinder, which results in a zone with fully turbulent flow and high dissipation. The pressure on the surface of cylinder will fluctuate with the vortex shedding. A similar flow phenomenon exists in the bypass flow after a blade. Figure 55 (Wang and He, 2001), shows the results of unsteady simulation performed by Wang and He, in which the

74

instantaneous pressure contour patterns of wake for turbulent flow through unsteady simulations are presented clearly. The wake flow in multi-stage turbomachinery is more complicated than vortex shedding after circle cylinder since it will be distorted and deformed by the blade when flows through the blade row downstream as shown clearly in Figure 56 by (Smith, 1966; Stieger & Hodson, 2005). This unsteady transport process could last to the next few blade rows and mix with new wake flows to forming highly non-uniform unsteady flow in blade passage.

5.5 Interaction between Secondary Flows and Blade Rows

Figure 55

Pressure contour of wake flow

The third part is similar to the second one, in which the second flows are also sheared by the blade rows downstream during the transport process. The distortion and mixing of these vortices will enhance the non-uniformity of the flow. Schlienger et al. investigated the interaction between secondary flows and blade rows through experiments on a low speed turbine with two stages. It is

Figure 56

Unsteady wakes convecting in blade passage

found that the characteristic of the unsteady flow field at the rotor hub exit is primarily a result of the interaction between the rotor indigenous passage vortex and the remnants of the secondary flow

75

structures that are shed from the first stator blade row. Moreover, there exist interactions among secondary flows, wake and blade rows, which results in more complicated unsteady flow. Matsunuma61 investigated this interaction effect on a low speed turbine of single stage, with the instantaneous absolute velocity contour pattern at the nozzle exit shown in Figure 57 (Matsunuma, 2006). The experimental results suggest that the secondary vortices are periodically and threedimensionally distorted at the rotor inlet. A curious tangential high turbulence intensity region spread at the tip side is observed at the front of the rotor, which is because of the axial stretch of the nozzle wake due to the effects of the nozzle passage vortex and rotor potential flow field.

Figure 57

5.6

Instantaneous absolute velocity contour pattern at nozzle exit

Wake-Boundary Layer Interaction

In low-pressure turbines, the wakes from upstream blade rows provide the dominant source of unsteadiness. Under low Reynolds number conditions, the boundary-layer transition and separation play important roles in determining engine performance. An in-depth understanding of blade boundary layer spatial-temporal evolution is crucial for the effective management and control of boundary layer transition or separation, especially the open separation, which is a key technology for the design of low-pressure turbines with low Reynolds number. Thus it is very important to research the wake-boundary layer interaction. In low-pressure turbines with low Reynolds number, boundary layer separation may occur as the blade load increases. Rational use of the upstream

T.Matsunuma, “Unsteady flow field of an axial-flow turbine rotor at a low Reynolds number”, ASME-GT06, number 90013, Spain, 2006. 61

76

periodic wakes can effectively inhibit the separation by inducing boundary layer transition before laminar separation can occur, so as to control loss generation. A comprehensive and in-depth research of wake boundary layer interactions in low-pressure turbines is given by Hodson & Howell (2005). They summarized the processes of wake-induced boundary-layer transition and loss generation in low-pressure turbines. The periodic wakeboundary layer interaction process is as follows: 

5.7

When the wake passes, the wake-induced turbulent spots form within attached flows in front of the separation point, the turbulent spots continue to grow and enter into the separation zone, and consequently inhibit the formation of separation bubble. The calmed region trails behind the turbulent spots. It is a laminar-like region, but it has a very full velocity profile. The flow of the calmed region is unreceptive to disturbances. Consequently, it remains laminar for much longer than the surrounding fluid and can resist transition and separation. It is the combination of the calming effect and the more robust velocity profile within the calmed region that makes this aspect of the flow so important. After the interaction of the wake, boundary layer separation occurs in the interval between the two wakes.

Unshrouded Tip Leakage Flow Interaction

The tip leakage flow is important in most turbomachinery, where a tip clearance with a height of about 1-2% blade span exists between the stationary end wall and the rotating blades. An unshrouded tip design is widely employed for a low stress and/or a better cooling in modern highpressure turbines. Pictorial representation of the tip leakage flow in unshrouded blades is given in Figure 58. The leakage flow over unshrouded blades occurs as a result of the pressure difference between the pressure and suction surfaces and is dominated by the vortex shed near the blade tip. The tip leakage flow has significant effects on turbomachinery in loss production, aerodynamic efficiency, turbulence generation, heat protection, vibration and noise. As a consequence of the viscous effects, significant losses are generated by the tip leakage flow in regions inside and outside the tip gap. And the entropy creation is primarily due to the mixing processes that take place between the leakage flow and the mainstream Figure 58 Flow over an unshrouded tip gap flow. Denton (1993) gave a simple prediction model for the tip leakage loss of unshrouded blades. So far, there are many researches about the leakage flow unsteady interactions in compressor. For example, Sirakov & Tan (2003) investigated the effect of upstream unsteady wakes on compressor rotor tip leakage flow. It was found that strong interaction between upstream wake and rotor tip leakage vortex could lead to a performance benefit in the rotor tip region during the whole operability range of interest. The experimental result of Mailach et al. (2008) revealed a strong periodical interaction of the incoming stator wakes and the compressor rotor blade tip clearance vortices. As a result of the wake influence, the tip clearance vortices are separated into different segments with higher and lower velocities and flow turning or subsequent counter-rotating vortex pairs. The rotor performance in the tip region periodically varies in time. Compared with in compressor, very little published literature is available on the unsteady interactions between leakage flows and adjacent blade rows in turbine. Behr et al. (2006) indicated that the pressure field of the

77

second stator has an influence on the development of the tip leakage vortex of the rotor. The vortex shows variation in size and relative position when it stretches around the stator leading edge.

5.8

Film Cooling Effects

According to the theory of Carnot cycle, increasing the inlet temperature of gas turbine is an effective way to increase the efficiency and capacity of a turbine. In order to enhance the performance of jet engine and gas turbine, the temperature of the gas flowing into a turbine blade passage has been raised continually in recent years, which might result in the damage of blades, especially the leading edge (LE) which is exposed to the hot gas directly. Although new high temperature materials have been investigated and used constantly, it is obvious that they couldn’t follow the rising pace of the inlet temperature. Four types of cooling methods, such as Convection cooling, Impingement cooling, Film cooling and Effusion cooling, and their hybrid methods are used in practical engineering. Usually, the effusion cooling can provides the best cooling among these four methods, while it is seldom used because it will weaken the structure strength of blades greatly. Convection cooling and impingement cooling are usually used in conditions where the temperature is lower than 1600˚K since they cannot provide protection to the surface of blades. Film cooling is the only way can be used in whole range of the temperature is higher than 1600˚K. Figure 59 (Owen, 2009), illustrates a typical high-pressure gas turbine Figure 59 Typical high-pressure turbine stage stage showing the rim seal and the wheel-space showing rim seal and wheel-space between the stator and the rotating turbine disc. It is curved downstream under the press and friction of hot main flow colored in pink in the figure, then forms a thin cooling film on the surface which separates the blade surface from hot gas. Meanwhile, it takes the sporadic flames and radiant heat to downstream. Hence, it can protect the blade surface effectively. In the next section we divert our attention to the Secondary Flow which is another cause of unsteadiness and complication in Turbomachinery.

5.9

General Review on Secondary Flows

The important 3D viscous flow phenomena within a blade passage of turbomachinery are boundary layers and their separations, tip clearance flows and wakes, which are most responsible of energy losses existing in blade passage. Hence, the losses in an axial compressor or turbine can be mainly classified as62:   

Profile losses due to blade boundary layers and their separations and wake mixing; in high speed condition, shock/boundary layer interaction may exist. End-wall boundary layer losses, including secondary flow losses and tip clearance losses. Mixing losses due to the mixing of various secondary flows, such as the passage vortex and

Sh. Kang, “Investigation on the Three Dimensional within a Compressor Cascade with and without Tip Clearance”, PhD thesis, Vrije Universiteit Brussel, September 1993. 62

78

tip leakage vortex. Among all these losses, the most complex one is the secondary flow loss. That is why considerable research on the secondary flow phenomena has been done in last decades. Secondary flow is defined as the difference between the real flow and a primary flow, which is related to the development of boundary layer on end-wall and blade surface, the evolution of vortices in passage, and detached flows or simply, the secondary flow in a blade row can be defined as any flow, which is not in the direction of the primary or stream wise flow63. Based on topology analysis and experiments, as well as the numerical simulations in recent decades, a couple of secondary flow models are proposed which are presented below. 5.9.1 Classical View The so-called classical secondary flow model, as illuminated in Error! Reference source not found. (a-b), is proposed by Hawthorne64 for the first time according to the theory of inviscid flow in 1955. This model presents the components of vorticity in the flow direction when a flow with inlet vorticity is deflected through a cascade. The main vortex, so-called passage vortex, represents the distribution of secondary circulation, which occurs due to the distortion of the vortex filaments of the inlet boundary layer passing with the flow through a curved surface. The vortex sheet at the trailing edge is composed of the trailing filament vortices and the trailing shed vorticity whose sense of rotation is opposite to that of the passage vortex. The classical vortex model attributes the secondary flow losses to the generation and evolution of vortex passage. However, this model is relatively simple, in which the interaction between the inlet boundary layer and blade force was not considered. Moreover, the vortex system within passage is only single passage vortex in half of the passage height range with other vortices absences. The secondary flow losses can be visualized by absence/presence of secondary vortex on Figure 60 (b). 5.9.2 Modern View When a shear flow along the solid wall approaches a blade standing on the wall, the shear flow will be separated from the wall and roll up into a vortex in front of the blade leading edge. This vortex is called horseshoe vortex due to its particular shape. This well-known phenomenon is firstly observed in the flow around cylinders. The oil flow visualizations by Fritsche65 show the evidence of the horseshoe vortex in accelerating cascades. In 1966, Klein presents a finer cascade vortex model with both the passage and horseshoe vortices as depicted in Error! Reference source not found.(a). While, the pioneering work for detailed analysis of secondary flow patterns in turbine cascades in general is done in 1977 by Langston et al 66 who proposed the well-known modern vortex model in cascade. Three vortices are presented in this model, as depicted in Error! Reference source not found.(b). Langston explains the interaction between the horseshoe vortex and the passage vortex, and the development of the passage vortex. The big differences between Langston’s model and Klein’s model exist in twofold67: by Langston et al68 who proposed the well-known modern vortex model in cascade.

Lei Qi and Zhengping Zou, “Unsteady Flows in Turbines”, Beihang University China. Hawthorne,” Rotational flow through cascades part 1: the components of vorticity.” Journal of Mechanics and Applied Mathematics, 8(3):266–279, 1955. 65 A. Fritsche. Str¨omungsvorg¨ange in schaufelgittern. Technische Rundschau Sulzer, 37(3), 1955. 66 L. S. Langston, “Three-dimensional flow within a turbine blade passage”, Journal of Engineering for Power, 99(1):21–28, 1977. 67 C. H. Sieverding, “Recent progress in the understanding of basic aspects of secondary flows in turbine blade passages”, Journal of Engineering for Gas Turbines and Power, 107(2):248–257, 1985. 68 L. S. Langston, “Three-dimensional flow within a turbine blade passage”, Journal of Engineering for Power, 99(1):21–28, 1977. 63

64 W. R.

79

Three vortices are presented in this model, as depicted in Error! Reference source not found.(b). Langston explains the interaction between the horseshoe vortex and the passage vortex, and the development of the passage vortex. The big differences between Langston’s model and Klein’s model exist in twofold69:

(a) Classical View (Hawthorne, 1955)

(b) Secoundary Losses in presence of secoundary vortex flow in classical view Figure 60

Classical Secondary Flow Model

C. H. Sieverding, “Recent progress in the understanding of basic aspects of secondary flows in turbine blade passages”, Journal of Engineering for Gas Turbines and Power, 107(2):248–257, 1985. 69

80





Langston clearly postulates that the pressure side leg of the leading edge horseshoe vortex, which has the same sense of rotation as the passage vortex, merges with and becomes part of the passage vortex Langston clarifies that the suction side leg of the leading edge horseshoe vortex which rotates in the opposite sense to the passage vortex, continuing in the suction side endwall corner, while the presentation of Klein suggests that this vortex is gradually dissipated in contact with the passage vortex.

(a) Kline 1966

(b) Langston, 1977 Figure 61

Modern Secondary Flow Model

The first point from Langston is supported by the light sheet experiment by Marchal and Sieverding70 in 1977. While, the results of this experiment also show the counter-rotating vortex, called counter vortex by Langston, in the trailing edge plane on the mid span side of the passage vortex rather than in the corner, which is not consistent with the second point from Langston. 5.9.3 Latest View In 1987, Sharma and Butler71 proposed a secondary flow pattern which is slightly different to that from Langston. This pattern, shown in Error! Reference source not found. (a), demonstrates that the suction side leg of the horseshoe vortex wraps itself around the passage vortex instead of adhering

P. Marchal and C. H. Sieerding, “Secondary flows within turbomachinery blading’s”, CP 214, AGARD, 1977. O. P. Sharma and T. L. Butler, “Prediction of the end wall losses and secondary flows in axial flow turbine cascade. Journal of Turbomachinery”, 109:229–236, 1987. 70 71

81

to the suction side. This result is similar to the results of Moore72 and Sieverding73. However, in 1988, another pattern is given by Goldstein and Spores74, shown in Error! Reference source not found. (b), which is different to Sharma’s again. Based on mass transfer results, they suggested that the suction side leg of the horseshoe vortex stays above the passage vortex and travels with it. This flow pattern is similar to that suggested by Jilek75 in 1986. The major difference among these three models is the location of the suction side leg of the horseshoe vortex. Since it is difficult to be detected due to the small size, most literatures cannot (a) Sharma and Butler, 1987 demonstrate develop of this vortex clearly. In 1997, a very detailed secondary flow visualization study was performed by Wang76. They proposed a more comprehensive but more complicated secondary flow the passage vortex and travels with it. This flow pattern is similar to that suggested by Jilek77 in 1986. The major difference among these three models is the (b) Goldstein and Spores, 1988 location of the suction side leg of the horseshoe Figure 62 Vortex pattern of Latest secondary flows vortex. Since it is difficult to be detected due to the J. Moore and A. Ransmayr, “Flow in a turbine cascade part 1: losses and leading edge effects”, ASME-GT83, number 68, 1983. 73 C. H. Sieverding and P. Van den Bosch,” The use of colored smoke to visualize secondary flows in a turbine-blade cascade”, Journal of Fluid Mechanics, 134:85–89, 1983. 74 R. J. Goldstein and R. A. Spores, “Turbulent transport on the end wall in the region between adjacent turbine blades”, Journal of Heat Transfer, 110:862–869, 1988. 75 J. Jilek, “An experimental investigation of the three-dimensional flow within large scale turbine cascades”, ASMEGT86, number 170, 1986. 76 H. P. Wang, S. J. Olson, R. J. Goldstein, and E. R. G. Eckert, “Flow visualization in a linear turbine cascade of high performance turbine blades”, Journal of Turbomachinery, 119(1):1–8, 1997. 77 J. Jilek, “An experimental investigation of the three-dimensional flow within large scale turbine cascades”, ASMEGT86, number 170, 1986. 72

82

small size, most literatures cannot demonstrate develop of this vortex clearly. In 1997, a very detailed secondary flow visualization study was performed by Wang78. They proposed a more comprehensive but more complicated secondary flow pattern, as illustrated in which includes the passage vortex, the horseshoe vortex, the wall vortex and the corner vortex. The development of the horseshoe vortex nearby the end-wall is effected by the boundary layer on end wall and the blade surface. In modern advanced blade, the leading edge radius of blade is so small that can Figure 63 Turbine Secondary Flow Model after Takeishi et al. be compared with the thick of boundary layer. Hence, the separation of boundary layer on end wall generates the multivortex structures at the leading edge of blade. Due to a strong pressure gradient the pressure side leg of the horseshoe vortex moves toward the suction side after it enters the passage. Meanwhile it entrains the main flow and the inlet boundary layer forming a multi-vortex leg. In 2001, Langston79 reviewed these new models after the Sieverding’s review. Laster in the same year, Zhou and Han80 gave a more comprehensive review of all these models. They concluded that the good understanding of the secondary flow in turbomachinery can help greatly to control the vortices within passage and decrease the losses, help greatly to control the vortices within passage and decrease the losses. 5.9.4 Comparing and Contrasting Secondry Flow in Turbine and Compressors Another view begins by comparing and contrasting turbine and compressor secondary flows, together with conclusions on the way forward to design in compressors81. A large amount of material has been published on secondary flow effects in axial flow turbomachinery, both turbines and compressors. Only a brief summary of these is given here. As will be seen in the next section, non-

H. P. Wang, S. J. Olson, R. J. Goldstein, and E. R. G. Eckert, “ Flow visualization in a linear turbine cascade of high performance turbine blades”, Journal of Turbomachinery, 119(1):1–8, 1997. 79 L. S. Langston, “Secondary flows in axial turbines: a review”, Annals of the New York Academy of Sciences, 934 (Heat Transfer in Gas Turbine System):11–26, 2001. 80 X. Zhou and W. J. Han, “A review of vortex model development for rectangular turbine cascade”, (in Chinese). Journal of Aerospace Power, 16(3):198–204, 2001. 81 N W Harvey, “Some Effects of Non-Axisymmetric End Wall Profiling on Axial Flow Compressor Aerodynamics. Part I: Linear Cascade Investigation”, Proceedings of GT2008. 78

83

axisymmetric end wall profiling has been pursued in recent years principally in the field of axial flow turbines. Consequently, it is useful to compare and contrast turbine and compressor secondary flows. Comprehensive reviews of turbine secondary flows are given in Sieverding [4] and Langston [5], and of secondary loss generation in Denton [6]. Whilst secondary flows are induced by any total pressure profile that enters a blade row and is subsequently deflected by it, the clearest understanding has been obtained for the case when the total pressure profile is just due to the incoming end wall boundary layers. Figure 63 shows a diagrammatic representation of turbine end wall secondary flows taken from Takeishi et al. [3] (noting that the rotation of the vortices is generally exaggerated) which has been describe this more fully, but the basic elements are: 

Rolling up of the inlet boundary layer into the horseshoe vortex at the airfoil leading edge. The pressure surface side leg of this becomes the core of the passage vortex. The passage vortex is the dominant part of the secondary flow and beneath it on the end wall a new boundary layer is formed, referred to as cross-flow "B" in Figure 63, which starts in the pressure side end wall corner.



Upstream of this the inlet boundary layer is deflected across the passage (over turned), referred to as cross-flow "A". The end wall separation line marks the furthest penetration of the bottom of the inlet boundary layer into the passage and divides it from the new boundary layer forming downstream of it. The dividing streamline between the suction and pressure side flows is shown as the attachment line in Figure 63. It intersects with the separation line at the saddle point.



The new end wall boundary layer, cross-flow "B", carries up onto the airfoil suction surface until it separates (along the airfoil "separation line") and feeds into the passage vortex. The suction side leg of the horseshoe vortex, referred to as the counter vortex in Figure 63, remains above the passage vortex and moves away from the end wall as the passage vortex grows.



A small corner vortex may occur in the suction surface/ end wall corner rotating in the opposite sense to the passage vortex. This has the effect of opposing the overturning at the end wall, although at the cost of additional loss.

One additional source of “classical” secondary flow that must be mentioned is the trailing edge vorticity that originates as a vortex sheet downstream of the blade trailing edge due to the variation in circulation along the span of the airfoil (and not shown). The scope for reducing this by modifying the end wall flows does not appear to be great and has not been part of this study. The basic features of compressor secondary flows are the same as those in a turbine blade row. However, there are a number of important differences in the details between the two, Cumpsty82:

82



The turning in a compressor blade row is much lower; typically 30 – 40 deg , compared to 100 deg in a turbine.



From classical secondary flow theory, this would be expected to result in lower secondary flows in a typical compressor row, for a comparable inlet total pressure profile.



An additional feature, often overlooked, for turbine secondary flows is that once they have

Cumpsty N. A.,, (2004), “Compressor Aerodynamics”, Krieger Publishing Company.

84

rolled up into vortices any further acceleration of the flow will stretch them feeding in more kinetic energy (of rotation), Patterson [10]. This may have the effect of amplifying the benefit of anything that delays the initial development of secondary flows on the end walls. 

Since the flow through a compressor blade row diffuses such vortex stretching will not occur. Rather the diffusion will encourage more rapid mixing out of the vortices. It is suggested that this is the reason why the smaller vortices (counter and corner) seen in turbine rows are not often identified for compressor ones. In addition end wall over-turning in a compressor row will be much more likely to result in flow separation, especially when the static pressure rise across the row increases if the compressor moves up its characteristic.

5.9.5 3D Separation A number of different flow regimes come under the heading of “three-dimensional separation”:   

If the aerodynamic loading is low enough, then the low momentum fluid in the airfoil suction side/ end wall corner will separate off the blade surfaces (as in turbine secondary flows) but will still have forward momentum. Where the loading is such that reverse flow does occur, then this may initially only be on one of either the end wall or the airfoil suction surface refers to the former as “wall stall” and the latter as “blade stall”. The combination of these two is known as “corner stall”. The resulting flow patterns are illustrated in Figure 64. where the illustration of formation of hub corner stall together with limiting streamlines and separation lines, (Lei et al.).

Distinct features of this are the reverse flow on both walls and the decrease of the chord wise extent of this flow away from the end wall. In terms of secondary loss, it is difficult to generalize on its magnitude in compressor rows. This depends on the details of the design; of which diffusion factors, DeHaller numbers and aspect ratio are just a few. One example may serve to indicate the potential for losing aerodynamic performance. With a small leakage flow present, which suppressed the corner stall, the 54% was reduced to 13% (about 11% of the total). For a turbine row with a similar aspect ratio, the secondary losses may be expected to be at least 20% of the total, but again this depends on the design details. From the above it is concluded that the scope for Figure 64 Illustration of formation of hub corner stall together with reducing secondary loss in a limiting streamlines and separation lines well-designed compressor row

85

at its design condition (without corner stall) is likely to be less than for a typical turbine one. Rather, reducing or mitigating penalizing features such as corner stall may be of more importance to the compressor aerodynamic designer.

5.10

Turbulence Consideration

Recent advancements in computer improvements in turbulence modeling have brought computational fluid dynamics improvements in turbulence improvements in improvements in turbulence modeling have brought computational fluid dynamics (CFD) to the improvements in turbulence modeling have brought computational fluid improvements in turbulence modeling have brought computational fluid dynamics (CFD) to the forefront of turbo-machinery design and analysis. The development, improvement, and application of turbo-machinery CFD dominate the literature. Today, 3-D Euler, quasi-3-D viscous, and 3-D full Navier-Stokes analyses are integral parts of turbomachinery design. Fan rotors are designed using viscous 3D CFD models using these models the blade geometry is tailored to control shock location, boundary layer growth and end-wall blockage. The complexity of the turbo-machinery flow field limits CFD simulations to Reynolds averaged (RANS) approximations. The flow field of a transonic fan over its entire operating range is particularly troublesome; it contains all the flow aspects most difficult to represent – boundary layer transition and separation, shock-boundary layer interactions, and large flow unsteadiness. Multistage configurations further the complexity as “neither in the stator nor rotor frame of reference is the deterministic flow steady in time”. Direct Numerical Simulations (DNS) and Large-Eddy Simulations (LES) are not currently practical for the fan/compressor flow field. The DNS explicitly solves for the instantaneous flow field and requires extremely fine gridding to resolve the smallest length scales – on the order of Re9/4. Thus, state-of-the-art turbo-machinery CFD involves solution of the RANS equations and hence, some modeling of the physics. The Reynolds-averaging process-the decomposition of the instantaneous flow field into mean and fluctuating components and subsequent temporal averaging introduces more unknowns than available equations for solution. Key modeling aspects are associated with this so-called “turbulent closure problem.” To obtain mathematical closure, the Reynolds stress terms must be related to mean flow properties either empirically or through a flow model which allows calculation of this relationship (eddy “viscosity,” mixing length, transport equations). As noted by Simpson, 2000, “all the efforts of experimental turbulent shear flow research are aimed at this central problem…” This closure issue is no different than that required of 1st order models. For example, through flow methods using the semi-actuator disk approach (like SLC) require loss and flow angle relationships (empirically or through analytical models). The use of RANS codes requires extensive computational resources. A viscous calculation with shock waves and tip leakage typically requires about 300,000 grid points (Denton and Dawes, 1999), although as many as 500,000 points may be needed (AGARD-AR- 355, 1998), per blade passage. In a recent multistage application, Rhie, et al., 1998, used approximately 1.5 million grid points to represent three stages (seven blade rows), taking advantage of the axisymmetric assumption (i.e., one modeled passage per blade row). The principal aerodynamic characteristics of most turbomachine flows are governed mainly by a balance between pressure gradient and convection, while turbulence tends to affect mainly secondary flow features and the losses83. This is at least so in low-load conditions in which the boundary layers are relatively thin and attached. In high-load and off design conditions, however, turbulence can contribute substantially to the aerodynamic balance and is thus a process of major practical interest. In such circumstances, the boundary layers grow rapidly, separation can ensue on W.L. Chen, F.S. Lien, M.A. Leschziner, “Computational prediction of flow around highly loaded compressor cascade blades with non-linear eddy-viscosity models”, International Journal of Heat and Fluid Flow 19 (1998) 307-319. 83

86

both suction and pressure sides (depending on the blade geometry and the incidence angle) and stream wise vorticity is intense ± all processes interacting strongly with the turbulence structure. The sensitivity of major mean flow features to turbulence is especially high when the flow enters the blade passage at an angle which departs materially from the design value, thus causing leading-edge separation and high flow displacement, followed by transition in the separated shear layer. More generally, transition tends to be a highly influential process in the majority of off-design flows in that details of the location and evolution of transition can dictate the sensitive response of the boundary layers to pressure gradients. The large majority of computational schemes for turbomachinery currently involve the use of the linear (Boussinesq) relationships between stresses and strains,

 u u j  2   ρκδij  ρui uj  μ T  i   x x  3 i   j

(.)

coupled with algebraic expressions or, at most, differential equations for the turbulent velocity and length scales to which the turbulent viscosity is related. This framework is accepted as being adequate for thin shear flows and is able to reproduce transition in simple boundary layers, if combined with appropriately constructed and calibrated transport equations for the variation of the scales in low-Reynolds-number conditions. However, it fails to resolve turbulence anisotropy and to represent correctly the effects of normal straining and curvature on the turbulent stresses. The last two deficiencies are especially important in blade flows; first, because the state of turbulence at the leading-edge impingement region is crucially important to the transitional behavior further downstream, and second, because the blade curvature causes significant damping or augmentation of turbulence transport in the boundary layers on the suction and pressure sides, respectively. It is now generally accepted that the substantial variability in the strength of the interaction between different strain types and the turbulent stresses can only be resolved, in a fundamentally rigorous sense, through the use of second-moment closure, in which separate transport equations are solved for all Reynolds-stress components. In particular, the very different stress-generation terms contained in these equations give rise to that closure's ability to resolve anisotropy and hence the influence of curvature, rotation and normal straining on the stresses. However, this type of closure is complex, poses particular challenges in respect of its stable integration into general computational schemes and is costly to apply in practice (Lien and Leschziner)84. A simpler and more economical alternative, albeit one which rests on a weaker fundamental foundation, is to use nonlinear stress /strain relations which can be made to return, upon the introduction of physical constraints and careful calibration, some of the predictive capabilities of second-moment closure.

5.11 Case Study - Heat Transfer in Separated Flows on the Pressure Side of Turbine Blades 5.11.1 Statement of Problem Heat transfer in separated flows on the pressure side of a typical high lift turbine profile is numerically investigated85. The numerical code was first validated on attached flows in turbine blades. To obtain flow separation cases, the profile is subject to large negative incidences so that a separation bubble is obtained at the pressure side. The numerical results are compared to available Lien, F.S., Leschziner, M.A. “Second-moment closure for three dimensional turbulent flow around and within complex geometries”. Computers and Fluids 25, 237, 1996. 85 P. De La Calzada, M. Valdes, and M. A. Burgos, “Heat Transfer in Separated Flows on the Pressure Side of Turbine Blades”, Industria de Turbopropulsores S. A., Madrid, Spain. 84

87

experimental data for code validation. It is shown how local minima and maxima values of the heat transfer coefficient are related to the separation and reattachment points, where the velocity component perpendicular to the wall is shown to have a significant effect on the heat transfer. The increasing demand of more efficient gas turbine engines is further stressing the physical understanding of aerothermal phenomena occurring in turbines. Turbine Inlet Temperature (TIT) has increased rapidly in the last decades enabled by the extensive use of increasingly effective cooling technologies. Further reductions in weight and cost targets have also required the development of thin low pressure turbine (LPT) profiles where flow separation might occur at the pressure side even at design conditions. These operating conditions of LPT have introduced new challenges in terms of understanding the aerothermal phenomena, as well as in the development of simulation tools able to predict these phenomena. In particular, the accurate prediction of thermal effects due to separation and reattachment of the flow on LPT profiles is an important new requirement. The aim of the present investigation is to perform a detailed numerical study of the heat transfer phenomena in separated flows at flow conditions representative of LPT airfoils. A comparison with experimental data is performed, hence allowing the validation of the code and the confirmation of the main flow features. Based on these numeric results, an attempt is made to understand and explain the flow physics in the vicinity of separation and reattachment points that can influence the heat flux. In particular, the relationship between the dynamic and thermal boundary layers and the importance of the velocity component perpendicular to the wall in creating injection of flow towards the wall or ejection of flow from the wall and their effect in the heat transfer is analyzed. 5.11.2 Literature Survey Much attention has been paid to the investigation of large flow separation in simple cases, including both velocity related measurements and heat transfer measurements. These include experimental investigations of backward-facing steps as Vogel and Eaton 86 or Sparrow et al.87, where the relationship between the separation region and the heat transfer features was studied. Corresponding numerical investigations have been performed on similar configurations like the one by Kaminejad et al.88 where only laminar conditions and very low Reynolds numbers are considered. The effect of turbulence was taken into account for example by Rhee and Sung89, where good agreement with experimental data was also found for very low Reynolds numbers. More recently, Rhee and Sung also investigated the effect of local forcing on the separation and reattaching flow. However, very little attention has been paid to the heat transfer in large separated flow regions in turbine representative conditions. Bassi et al.90 present CFD results on the separated flow region of a HPT airfoil with cutter trailing edge with no cooling ejection, but only a short discussion about the separated flow physics is included. Regarding experimental investigations, Rivir et al.91 have measured the flat plate heat transfer in a region of turbulent separation, and Bellows and Mayle 92 86J.

C. Vogel and J. K. Eaton, “Combined Heat Transfer and Fluid Dynamic Measurements Downstream of a Backward-Facing Step “, Heat and Mass Transfer, vol. 107, pp. 922-929, 1985. 87 E. M. Sparrow, S. S. Kang, and W. Chuck, Relation Between the Points of Flow Reattachment and Maximum Heat Transfer for Regions of Flow Separation, Int. J. Heat Mass Transfer, vol. 30, no. 7, pp. 1237-1246, 1987. 88 H. Kazeminejad, M. Ghamari, and M. A. Yaghoubi, “A Numerical Study of Convective Heat Transfer from a Blunt Plate at Low Reynolds Number”, Int. J. Heat Mass Transfer, vol. 39, no. 1, pp. 125-133, 1996. 89 G. H. Rhee, and H. J. Sung, “A Low-Reynolds Number, Four Equation, Heat Transfer Model for Turbulent Separated and Reattaching Flows”, Int. J. Heat Fluid Flow, vol. 18, pp. 38-44, 1997. 90 F. Bassi, S. Rebay, M. Savini, S. Colantuoni, and G. Santoriello, “A Navier-Stokes Solver with Different Turbulence Models Applied to Film-Cooled Turbine Cascades”, Paper No. 41, AGARD-CP-527, 1993. 91 R. B. Rivir, J. P. Johnston, and J. K. Eaton, “Heat Transfer on a Flat Surface under a Region of Turbulent Separation”, Turbomachinery, vol. 116, pp 57-62, 1997. 92 R.J. Bellows and R. E. Mayle, “Heat Transfer Downstream of a Leading Edge Separation Bubble,”, Turbomachinery, vol. 108, pp. 131-136, 1986.

88

have measured the heat transfer on a blunt body leading edge separation bubble both for cases of high Reynolds number93. More recently, De la Calzada and Alonso94 performed a numerical investigation of large flow separation region at the pressure side of a turbine profile but not comparison with experimental results was included. Lutum and Cottier presented a similar investigation, but results indicated that simulations were not able to reproduce experimental heat transfer results at the pressure side separation region especially for low turbulence levels. From experimental investigations, it is known qualitatively that separated flow regions are characterized by large and rapid variations of the heat transfer (e.g., Rhee and Sung). Furthermore, the heat transfer presents a local minimum and a local maximum in the vicinity of separation and reattachment points respectively, with regions where the heat transfer coefficient (HTC) is much larger than that of attached flows95. Taking into account that separated flow regions are usually characterized by high turbulence levels and large scale unsteadiness, there is a tendency in the heat transfer community to explain the heat transfer phenomena in separated flows in terms of the generation of turbulence rather than in terms of the dynamic and thermal boundary layers relationship. 5.11.3 CFD Modeling In the present investigation, an in-house CFD solver is used for calculations. This code solves the RANS equations written in conservative form in an absolute frame of reference. The scheme used is based upon Jameson et al96. Convective terms are discretized using a cell vertex scheme, and the viscous terms are computed by means of the Hessian matrix. Integration in time is performed using an explicit five stage Runge-Kutta scheme where the viscous and artificial dissipation terms are evaluated in the first, third, and fifth stages. The code runs on unstructured meshes which are built by a quasi-structured layer all along the walls, where viscous effects are expected to be dominant and by a fully triangular unstructured mesh in the rest of the flow domain obtained by Steiner triangulation97. For turbulence simulation, the two equations κ-ω model from Wilcox98 is implemented. More details of the numerical code can be found in Corral and Contreras99. Numerical results are post processed to obtain heat and mass transfer relevant parameters at the walls. This is performed by computing velocity and temperature variation in the direction perpendicular to the wall so that heat transfer and friction coefficient as well as Stanton number can be computed, as defined below. The local Stanton number is the equivalent for the temperature to the local skin-friction coefficient for the velocity. Although the local Stanton number variations do not represent variations in heat flux alone but also take into account the local velocity value, it is the most adequate parameter to describe the thermal boundary layer behavior and to develop special correlations for heat transfer estimation (i.e., Reynolds-Colburn analogy).

W. Merzkirch R. H. Page, and L. S. Fletcher, “A Survey of Heat Transfer in Compressible Separated and Reattached Flows”, AIAA Journal, Vol. 26, no. 2, pp. 144-150, 1988. 94 P. De La Calzada and A. Alonso, “Numerical Investigation of Heat Transfer in Turbine Cascades with Separated Flows”, Turbomachinery, vol. 125, no. 2, pp. 260-266, 2003. 95 R. B. Rivir, J. P. Johnston, and J. K. Eaton, “Heat Transfer on a Flat Surface under a Region of Turbulent Separation”. Turbomachinery, vol. 116, pp 57-62, 1997. 96 A. Jameson, W. Schmidt, and E. Turkel, “Numerical Solution of the Euler Equations by Finite Volume Method using Runge-Kutta Time Stepping Schemes”, AIAA, Paper 81-1259, 1981. 97 R. Corral and J. Fernandez-Castañeda, “Surface Mesh Generation by Means of Steiner Triangulation”, Proc. 29th AIAA Fluid Dynamics Conference, vol. 39, pp. 176-180, Albuquerque, New Mexico, 1998. 98 D. C. Wilcox, “Reassessment of the Scale Determining Equation for Advanced Turbulence Models”, AIAA J., vol. 26, pp. 1299-1310, 1988. 99 R. Corral and J. Contreras, “Quantitative Influence of the Steady Non-Reflecting Boundary Conditions on Bladeto-Blade Computations”, Proc. 45th ASME Gas Turbine and Aero engine Congress, Exposition and Users Symposium, ASME Paper 2000-GT-515, Munich, 2000. 93

89

 T   k  HTCx  n  w Ch x   ρ e C p u e (T0  Tw )ρ e C p u e

,

Cf x 

τw 1 ρ e u e2 2

(.)

Note, that the total temperature is used in the definitions instead of the adiabatic wall temperature, even though compressible effects and therefore viscous dissipation may be important since the representative cases for LPT usually imply an exit Mach number of around 0.5, as we have in our study. However, the difference between the aforementioned coefficients and the corresponding compressible definitions can be kept sufficiently low if the wall temperature for the computations is properly chosen. In our particular cases, the total temperature is defined as in the experiments and the wall temperature is taken around 25 K higher than the fluid temperature, which keeps the difference between compressible and incompressible heat and mass transfer coefficient values lower than 2% even at regions with Mach numbers around 0.5. This wall temperature value also develops a thermal boundary layer whose magnitude is large enough to avoid high sensitivity to any random numerical errors in the resolution of the temperature field around the wall. 5.11.4 Description of the Blade and Computational Grids, and Results for Attached Flow The T106-300 blade section has been used as a generic geometry representative of a typical highly loaded LPT airfoil100 (see Figure 65 for cascade geometry and conditions details). In this investigation, the T106 blade profile is subject to extremely large negative incidences in order to have a large separation bubble on the pressure side. Mach and Reynolds numbers are varied around typical LPT values. The generated grid is hybrid in nature with higher definition in regions adjacent to the wall, trailing edge and leading edge, as shown in Figure 66. Due to the expected flow separation at the pressure side when the profile is subject to high negative incidence, on this investigation the viscous mesh is extended to a region larger than attached flows would require for this Reynolds number. The objective of this large region Figure 65 T106-300 Cascade geometry and aerodynamic design with high definition is to conditions capture the shear layers and flow features on the pressure side large bubble. However, in order to avoid any mesh sensitivity the same grid consisting of 8,623 nodes was kept unchanged for all cases, including the attached flow 100 H. Hoheisel, “Test Case E/CA-6, Subsonic Turbine Cascade T106, Test Cases for Computation of Internal Flows

in Aero Engine Components”, AGARD-AR-275, 1990.

90

achieving a range of y+ values at the pressure side in the order of y+< 3. Results at design conditions are shown pressure distribution is considered to match well with the experiments, in particular on the major part of the suction side. Since we are interested mainly in the flow along the pressure side, no attention will be paid to the separation bubble at the back suction surface that the code does not predict probably due to a too soon turbulence generation and boundary layer transition. Although the level of pressure achieved by the numerical results at the pressure side of the profile is lower than the experimental data, the heat transfer level matches well with the experiments. However, more HTC oscillations are found in the experiments compared with the smoother results predicted by the numerical simulation. It is interesting to note that the heat transfer measurements at the acceleration region of the leading edge decrease to lower values than the CFD results. This might indicate that the profile is subject to a slightly larger negative incidence in the experiments, hence creating an acceleration-deceleration behavior achieving a higher final pressure as shown by the results. The final acceleration region towards the trailing edge has a more pronounced effect on the numerical simulation, where the heat transfer value shows higher increase due to the expected thinning of the boundary layer with the increase in the external velocity. 5.11.5 Separated Flow with Large Separation Bubble Results at the extreme conditions of 37.7° negative incidence (i.e., inlet angle β1 = 90°) are shown first. The comparison between numerical and experimental results in terms of pressure distribution along the airfoil is presented in Figure 67. The separation region is characterized by low velocities and a fairly constant pressure distribution. However, at the reattachment region the static pressure increases reaching a local maximum (i.e., local minimum value of Cp in Figure 67), which indeed indicates the reattachment point. The experimental results indicate, to some extent, a shorter separation bubble which reattaches earlier, hence starting earlier also the acceleration towards the trailing edge. This may be related to the already identified higher pressure at the pressure side predicted by the CFD, which might indicate some slight difference in local incidence angle between the experiments and the simulations. Some more detail about the flow can be identified by comparing experimental and numerical heat transfer results shown in Figure 67. Both experimental and numerical results show two local minima and maxima between the extreme values achieved at leading and trailing edges (these extreme values are not shown in the graph). The first minimum occurring at around 0.03 x/L corresponds to the expected reduction in heat transfer rate. In Figure 68 (A-D) the Mach number, total Pressure, Temperature, Velocity vectors fields are plotted where the large bubble at the pressure side can be clearly identified. Helped by the streamlines traces, the multiple Figure 66 2-D hybrid mesh around the T106 blade bubble configuration can be also identified. In this particular case, two bubbles appear. As confirmed in Figure 68(D) by the velocity vectors, one small bubble is stretched towards the pressure wall, developing at the center of the full separation region whose vortex is rotating

91

counterclockwise, and one large bubble, rotating clockwise is extending up to the external shear layer along the major part of the pressure side, having its vortex core at the rear part of the separation region while extending its vortex influence also to the front part. Detail of the temperature field and flow velocities in the regions of flow separation and reattachment are plotted in Figure 68 (C-D). At points 1 and 3, the flow is separating and a large component of the velocity perpendicular and directed away from the wall exists. This flow configuration takes heat from the side walls and ejects it, creating an ejection stagnation or fountain-like region where the wall thermal field is penetrating the main flow helped by the perpendicular component of the velocity, hence increasing the effective thermal boundary layer and decreasing the heat transfer rate.

Figure 67

Blade profile pressure coefficient

This phenomena is particularly clear in front of point 3, where the increase in the thermal boundary layer thickness can be easily identified by the extension of the high temperature region close to the wall in Figure 68. Point 3 corresponds to the separation of an internal second bubble, which must also exist in the experiment configuration since the local minimum can be also identified in measurements in Figure 9. Points 2 and 4 correspond to reattachment points where there is an important component of the velocity perpendicular and towards the wall, hence taking fresh fluid to the wall and creating an injection stagnation region where the thermal boundary layer is reduced and heat transfer is increased. To further investigate the thermal boundary layer developing through the separation region the temperature profiles developing along straight lines perpendicular to the wall, marked a-d in Figure 68 (B). Note, that the y coordinate is non-dimensionalized with the thermal boundary layer thickness, which is basically coincident with the thickness of the separated region. Dotted lines represent the temperature distribution of the corresponding adiabatic wall case where static temperature only varies as a result of the velocity profile (being the stagnation temperature fundamentally constant), while solid lines show the temperature distribution within the recirculation region at different distances from the wall in the case with heat transfer and heated wall.

92

The lowest wall temperature gradient is obtained at the leading edge separation point 1 (line a), where even with the thermal boundary layer being relatively thin the fluid temperature shows a low gradient specially close to the wall driven by the ejection of heated flow from the wall through the ejection stagnation region configuration. On the contrary, the highest heat flux is achieved at the main bubble reattachment point 4 (line d) where, additionally to the thin thermal boundary layer thickness, the fluid temperature variation is mainly concentrated at the wall in a region about 10% of that thickness, hence increasing the temperature gradient at the wall. This reduction of the effective boundary layer thickness is driven by the injection stagnation region configuration, where the velocity component perpendicular to the wall is forcing the thermal boundary layer to be squeezed towards the wall. As an additional proof showing that there is low coupling between the dynamic and thermal boundary layers and their gradients in separated regions, the relationship between the velocity parallel to the wall and temperature gradients at the wall is investigated. It is widely accepted that the Reynolds-Colburn analogy is only reliable in attached flows only for modest, near-zero, pressure

(B) Pressure Contours (A) Mach No.

(C) Temperature

Figure 68

(D) Velocity vectors

Flow field at the front and middle parts of the separation bubble

93

gradients, and with a constant wall temperature. The computed local skin-friction coefficient (absolute value), the Stanton number, and the Reynolds-Colburn analogy are shown in Figure 69 to further demonstrate that the analogy between dynamic and thermal boundary layer is not valid for separated flows even when no pressure gradient exists. Only at the rear acceleration region where attached flow is ensured, the Reynolds analogy tends to follow the correlation showing a conventional relationship between dynamic and thermal boundary layers and their gradients at the wall. Furthermore, unlike the Stanton number, the skin friction approaches zero not only at the separation and reattachment regions but also along the major part of the separated flow region, hence confirming that the Reynolds-Colburn analogy is not applicable. This is clear proof that there is a very weak coupling between velocity parallel to the wall and thermal boundary layers in separated flows. On the contrary, it is the convective transport of fluid in a direction normal to the wall and the fluid conduction effects in low velocity regions what drive the heat transfer phenomenon, hence supporting once again the prime role of the stagnation region configurations on the heat transfer mechanism.

Figure 69

Heat transfer coefficient for different negative incidences

5.11.5.1 Inlet Flow Angle Effects Inlet flow angles of 90°, 100°, 110° (i.e., -37.7, -27.7°, and -10.7° incidence angle, all with separated flows at pressure side), and 127.7° (i.e., 0° incidence angle, with pressure side attached flow) have been simulated for the nominal isentropic exit Re = 1.5 x 105 and an isentropic exit Mach number of 0.5. The results in terms of HTC and Stanton number are presented in Figure 69 and Figure 70. As expected, the size of the bubble is decreasing with the reduction of the negative incidence angle as can be concluded from the location of the maximum values of Stanton numbers in Figure 70. All the

94

I separated flow cases show relatively large bubbles varying the reattachment points from 0.5 x/L for -17.7° incidence up to 0.6 x/L for -37.7° incidence. Unlike the HTC whose local maximum value at reattachment point is maintained almost constant along the attached acceleration region up to the trailing edge region, the Stanton number clearly generates a more pronounced local maximum value at the reattachment point driven by the combination of maximum heat flux and static pressure (i.e., minimum external velocity). It is noticeable that in all separated flow cases the same multiple bubble configuration is obtained as indicated by the presence, within the separated region, of one additional local minimum and one additional local maximum in heat transfer parameters although it is less evident in the slight negative incidence case (i.e., -17.7° incidence). Generally, it can be concluded that the separated region always generates a redistribution in the heat flux by decreasing the value at the front separation region and by increasing it at the rear reattachment region. The higher or lower surface averaged effective value will depend on the particular geometry and conditions.

Figure 70

Stanton number for different negative incidences

5.11.5.2 Reynolds Number Effect Reynolds number effect is investigated by simulating different cases with the same incidence and exit Mach numbers but different fluid conditions so that the Reynolds number is changed. In order to achieve the required effect in the simulations, only the pressure level is modified. Figure 71 and Figure 72 present the results when the Reynolds number is varied between 150,000 and 400,000. The dependence of heat flux on Reynolds number at separating and impingement regions can be obtained analytically on simple cases. At impingement points the case of plane and axisymmetric laminar flows can be integrated to obtain the known dependence of the heat flux on the Reynolds number to the power of 0.5101. Similarly, at separating points expansion equations can be obtained 101

F. M. White, “Viscous Fluid Flow”, McGraw-Hill, pp. 162 and 248, 1991.

95

which also show a dependence on Reynolds number to the power of 0.5 in simple cases as wedge and Howarth's decelerating flow 102. However, these methods are of difficult application to complex cases as presented here where a shear flow impinges on the wall with an inclination angle (i.e., the bubble reattachment occurring in our case), or where the separation occurs within a region of already separation bubble (i.e., the secondary bubble appearing in our case). In our simulation cases, the HTC (i.e., heat flux) also increases with Reynolds number as expected. However, the maximum values at the reattachment point in these cases increases with an exponent approximately equal to 0.3. It is interesting to note that the Stanton number varies inversely with the

Figure 71

Heat transfer coefficient for different Reynolds number

Reynolds number, as shown in Figure 72. By applying the definition relationship between HTC and Stanton number Ch in Eqs. (3) and (4), it can be seen that the ratio HTC/Ch must retain a dependence on Reynolds to the power of 1. Therefore, the Stanton number dependence on the Reynolds number should vary with and exponent of -0.7 in these cases according to the exponent 0.3 found for the HTC, which is indeed confirmed by the maximum values at the reattachment point shown in Figure 72. One interesting feature is that, for all Reynolds numbers investigated, the size of the bubble and the internal structure (i.e., multiple bubble configuration) is the same, as can be concluded from the location of local maxima and minima in the figures. Although it could be expected that increasing the Reynolds number would reduce the size of the separation bubble, in this particular case the reattachment is driven by the acceleration of the flow and the role played by the Reynolds and the corresponding boundary layer instability and potential transition is expected to be very minor. This is a completely different behavior compared to cases in which there is no flow acceleration, and the reattachment is driven by boundary layer transition.

H. W. Kim and D. R. Jeng, “Convective Heat Transfer in Laminar Boundary Layer Near the Separation Point”, ASME Proc. of the 1988 National Heat Transfer Conference, vol. 3, pp. 471-476, 1988. 102

96

In these latter cases, the increase of turbulence produces an early transition and reattachment and an increase in heat flux due to the stronger reattachment vortex on a blunt flat plate subject to pulsating conditions. Although the implemented numerical turbulence model was able to produce high turbulence and the corresponding boundary layer transition on the suction surface to avoid the back surface separation, at the pressure side the turbulence generation is concentrated on the external shear layer and from there it is convected downstream to the trailing edge and the downstream wake. Therefore, it is thought that in cases like this the turbulence is not a strong enough mechanism to force sufficient flow entrainment and perturbation to the shear layer to produce an early reattachment of the boundary layer, and it is then expected that the size of the separation bubble will depend weakly on the Reynolds number and turbulence.

Figure 72

Stanton number for different Reynolds numbers

5.11.6 Concluding Remarks A better understanding of the flow physics and the heat transfer mechanisms in large separated flow regions have been achieved by means of a numerical investigation on the T106-300 typical LPT airfoil subject to large negative incidence. Flow separation is characterized by a pronounced reduction in HTC at the separation region, close to the leading edge where the minimum value is achieved, and by an increase at the reattachment region where the maximum value is achieved. Those are extreme values, much lower and higher than the ones obtained for attached flows. It is concluded that the velocity component perpendicular to the wall is the main contributor to the generation of ejection and impingement stagnation configurations, where the flow is taken from or towards the wall, hence affecting the thermal field in those regions and contributing to create a lower or higher temperature gradient at the wall and the corresponding HTC values. By analyzing the Reynolds-Colburn analogy all along the pressure side of the profile, the low coupling between the velocity component parallel to the wall and the thermal field and their gradients within the separation region is confirmed. Additionally, it is also shown that an important variation in HTC

97

values can occur within the separation region due to the presence of secondary separation bubbles which can create additional separation and reattachment points. This is confirmed by both numerical and experimental results for the high negative incidence (i.e.,-37.7° incidence), which show the presence of one additional local maximum and one local minimum in HTC values that must indicate the presence of additional corresponding reattachment and separation points, hence indicating the presence of and the additional secondary separation bubble. Moreover, it is also shown by the numerical results that the multiple bubble configuration is found for all separated cases investigated here (i.e., negative incidence varying from -17.7° to -37.7°). Finally, the variation of the heat transfer with the Reynolds number is investigated. The numerical results show no variation of the separation bubble size with Reynolds number varying from 150,000 to 400,000. A dependence of the HTC on the Reynolds number to the power of 0.3 is obtained in the separation region, in particular at the maximum value occurring at the main bubble reattachment point on the rear part of the separation bubble103.

P. De La Calzada, M. Valdes, and M. A. Burgos, “Heat Transfer in Separated Flows on the Pressure Side of Turbine Blades”, Industria de Turbopropulsores S. A., Madrid, Spain. 103

98

6 6.1

Rotor-Stator Interaction Treatment (RST) Physical Perspectives

Turbomachinery flows are naturally unsteady mainly due to the relative motion of rotors and stators and the natural flow instabilities present in tip gaps and secondary flows104. Full scale, time dependent calculations for unsteady turbomachinery flows are still too expensive to be suitable for daily design purposes. One of the reasons for this large cost is the fact that in practical turbomachinery of these reduced order models requires that the engineer/designer be aware of a method's capabilities as well as its limitations. The key trade off in the computation of unsteady turbomachinery flows is between the accuracy of the method and the cost or computational efficiency with which a solution can be obtained. Highly accurate and well resolved models tend to be limited by the available computing power, while most reduced-order models usually neglect a significant amount of the physics and are therefore not credible for the evaluation of the performance and heat transfer characteristics of a turbomachine. A balance between these extremes is clearly desirable. In order to include the unsteady effects while keeping the computational requirements reasonable, two types of approximations can be distinguished. The first approach involves rescaling

Figure 73

Schematics of 3-D concept at IGV/Rotor/Stator interface

the geometry (typically by altering the blade counts and their chords to maintain solidity) such that periodicity assumptions hold in an azimuthal portion of the domain that is much smaller than the full annulus. A second alternative involves the use of the original geometry but compromises the fidelity

Xiaodong Wang, “CFD Simulation of Complex Flows in Turbomachinery and Robust Optimization of Blade Design”, Submitted to the Department of Mechanical Engineering Doctor of Philosophy at the Vrije Universiteit Brussel July 2010. 104

99

of the time integration method105. Figure 73 shows a schematics of 3-D point of view in either case. All of these approximations can be considered to be different variations of reduced-order models. In order to use the same solver, the flows in stator and rotor should be calculated in the stationary frame of reference and the rotating frame of reference, respectively. However, a critical problem is how to

Figure 74

Interface between Rotor/Stator

transfer the information downstream and upstream at the interface of stator and rotor. The quality of the flow predictions for multistage turbomachinery strongly depends on the treatment of rotor/stator interaction. Figure 74 illustrates the interface between them. Two general approaches as steady and unsteady interactions are available as detailed in Table 3.

Steady Mixing Plane Frozen Rotor Table 3

Un-staedy Sliding Mesh Harmonic Balance Time Transformation

Rotor/Stator Interaction Schemes

6.2 Different Between Multi-Passage and MultiStages Before going any further, it is worth mentioning two terminology which is been used often in literature. They are Multi-Stage and MultiPassage. The difference been best expalne through the Figure 75. It could thought of a matrix notation. While

Figure 75

Difference between Passage and Stages

105 Arathi K. Gopinath_, Edwin van der Weidey, Juan J. Alonsoz, Antony Jamesonx, Stanford University, Stanford,

CA 94305-4035, Kivanc Ekici {and Kenneth C. Hallk, Duke University, Durham, NC 27708-0300, “ThreeDimensional Unsteady Multi-stage Turbomachinery Simulations using the Harmonic Balance Technique”

100

passages are the columan of matrix and usually treated the same in terms of gridding and analysis, the rows are stages and treated another way as they have usually different geometry and conditions. Adjacent blade rows contain unequal numbers of blades and shape, therefore, in principle, a proper simulation requires solution of all blades in each row. However, some vendors such as ANSYS© has developed a suite of tools that enables more efficient solution for a number of analysis types. The key attribute of these tools is that the full wheel solution can be obtained by solving only one or at most a few blades per row106.

6.2

Steady Treatment of Interface

6.2.1 Mixing Plane The simplest treatment of R/S interface is the stage or Mixing Plane method proposed by Denton107. This method assumes the exiting flows of stator become uniform flows before entering the inlet of domain of rotor. A block computational domain of Rotor, Guided Vanes, Mixing Planes and applied boundary is shown in Figure 77. A pitch wise averaging of the flow solution is needed at R/S interface before transferring the information of both sides. The essential idea behind the mixing plane concept is that each fluid zone is solved as a steady-state problem108. At some prescribed iteration interval, the flow data at the mixing plane interface are averaged in the circumferential direction on both the stator outlet and the rotor inlet boundaries. The averaging process could be choice of three types Figure 77 Block Computational domain for a of averaging methods: area-weighted Rotor with guiding vanes averaging, mass averaging, and mixed-out averaging. By performing circumferential averages at specified radial or axial stations, "profiles'' of boundary condition flow variables can be defined. These profiles, which will be functions of either the axial or the radial coordinate, depending on the orientation of the mixing plane, are then used to update boundary conditions along the two zones of the mixing plane interface. In the examples shown in Figure 76 profiles of averaged total pressure (P0), direction cosines of the local flow angles in the radial, tangential, and axial directions (αr, αt, αz), total Figure 76 Axial rotor/stator interaction (Schematics temperature (T0), turbulence kinetic illustrating the Mixing Plane concepts) energy (k), and turbulence dissipation Turbomachinery Simulation, ANSYS blog. J. D. Denton, “The calculation of three-dimensional viscous flow through multistage Turbomachinery”, Journal of Turbomachinery, 114(1):18–26, 1992. 108 Release 12.0 © ANSYS, Inc. 2009-01-22. 106 107

101

rate (ε) are computed at the rotor exit and used to update boundary conditions at the stator inlet. Likewise, a profile of static pressure (Ps), direction cosines of the local flow angles in the radial, tangential, and axial directions (αr, αt, αz), are computed at the stator inlet and used as a boundary condition on the rotor exit. Note that the meshes on both sides of the interface should cover the same range in span wise, the averaging is performed along the same azimuthal mesh lines. However, a full nonmatching mixing plane109 can be used to overcome this limitation. Better, the isolated simulation on single stator or rotor, the interaction of potential flows in considered in this method. However, the Figure 78 A compressor Pressure Distribution on a impact of secondary flows and separation surface using a Mixing Plane flow are erased. This physical approximation tends to become more acceptable as rotational speed is increased. The mixing plane method is by far the most often used R/S modeling in industry design and optimization. Unfortunately it doesn’t capture the whole physics. This is usually evident by visual inspection of in interface (mixing) plane as an imaginary line between the cascades. Figure 78 displays a compressor Pressure Distribution on a surface at constant radius half way between the hub and the casing using a Mixing Plane computation. 6.2.2 Frozen Rotor If the exchange of information at the interface is by interpolation directly without averaging, one has the Frozen Rotor method. The difference is, Mixing Plane mixes the flow and apply the average qualities on the interface for upstream and downstream components; while frozen rotor will pass the true flow to down steam and vice versa. So if you are interested in the wake effect on the downstream component performance then you should use frozen rotor method. Its disadvantage is that, if gives you the solution at the single relative position. So if you want to get the wake effect on the downstream component for all relative positions (as happens in reality) then you should go for the true transient method. As the name indicates, the relative position of rotor and stator is fixed. Hence, the result of the frozen rotor method is equivalent to a certain point of the unsteady simulation which means the flow solutions will dependent on the relative position between rotor and stator. Since the information exchange on R/S interface is through interpolation, the mesh on both sides of the R/S interface should cover the same pitch range. That means the periodic of the rotor domain and stator domain should be kept the same,

KSPS  K R PR

(18.1)

Where, KS and KR are relative prime which stand for the number of passages in the stator domain and rotor domain, respectively. Ps and PR denote the pitch of stator and rotor separately. An approximation of the blade number can be made if Ks and Kr are large in order to reduce the computational cost, which is called Domain Scaling. For instance a turbine with 29 blades of stator 109

NUMECA International, Brussels, “Fine/Turbo User Manual V8”, October 2007.

102

and 31 blades of rotor can be approximated by a turbine with 30 blades of both stator and rotor, then only one passage is needed to mesh for both stator and rotor. However, the simulation results are only the approximated result to the real model. The Frozen Rotor method is used firstly by Brost et al.110 in simulations of an axial turbine where the simulated results have a good accordance with the transient results of the measurement. While, the flow field in a passage usually changes a lot during the period. Therefore, this method is only used in some specific simulations. The information Figure 79 Predicted Total Pressure calculated by the frozen exchange processes of mixing rotor plane and frozen rotor methods depend on the boundary type of the R/S interface. The detail settings for different boundary types and the corresponding exchange strategies can be found in111.

6.3

Unsteady Treatment of Interface

6.3.1 Sliding Mesh (MRF) Full unsteady simulations that integrate the governing equations in time can be performed to model the nonlinear unsteady disturbances by marching time accurately from one physical time instant to the next. The flow fields within multiple blade rows are solved simultaneously and the meshes within adjacent rows are moved relative to one another with each time step. However, the computational expense of this approach can be significant. This is because sub-iterations are required at each time instant, the time step size is necessarily small to preserve time accuracy, and many time steps are required to reach a time periodic solution. Additionally, multiple passages must be meshed to achieve spatial periodicity, unless so-called phase-lagged boundary conditions are used to reduce the size of the computational domain to a single blade passage in each blade row112. For unsteady simulation, a natural idea is to simulate several different transient positions of rotor related to stator which leading to the traditional unsteady treatment of R/S interface is the Sliding Mesh method proposed by Rai113. For unsteady simulation, a natural idea is to simulate several different transient positions of rotor related to stator which leading to the traditional unsteady treatment of R/S interface is the Sliding

V. Brost, A. Ruprecht, and M. Maih, “Rotor-Stator interactions in an axial turbine, a comparison of transient and steady state frozen rotor simulations”, Conference on Case Studies in Hydraulic Systems-CSHS03, 2003. 111 NUMECA International, Brussels, “Fine/Turbo User Manual V8 (including Euranus)”, October 2007. 112 J. M. Weiss, K. C. Hall, “simulation of unsteady turbomachinery flows using an implicitly coupled nonlinear harmonic balance method”, Proceedings of ASME Turbo Expo 2011, GT2011. 113 M. Rai, “Application of domain decomposition methods to turbomachinery flows”, ASME Advances and Applications in Computational Fluid Dynamics, volume 66, 1988. 110

103

Mesh method proposed by Rai114. In this method, the computational domain is divided into two parts: rotor domain and stator domain. The mesh for rotor domain rotates with rotor. The R/S interface becomes a sliding face and the exchanges of solution information are through the interpolation to the dummy cells on both side without any averaging. At each time step, the rotor is set at its correct position and equations are solved for that particular time step for the whole computation domain. The final solution is therefore a succession of instantaneous solutions for each increment of the rotor position. More precisely to set up sliding mesh simulation115, 1. 2. 3. 4.

Create periodic zones. Set up the transient solver and cell zone and boundary conditions for a sliding mesh. Set up the mesh interfaces for a periodic sliding mesh model. Sample the time-dependent data and view the mean value.

The methodology is based on the use of Moving Least Squares (MLS) approximation in a high-order finite volume framework116. Here we present two different approaches based on MLS approximation for the transmission of information from one grid to another. The intersection approach: the flux at the interface edge is split between the cell having an interface edge coincident (Figure 80 A). The halo cell approach: a halo-cell is created as a specular image of the interface cell (Figure 80 B). Moreover, two kind of stencil has been tested: the half stencil which take in account only cells from the grid in which the cell is placed and the full stencil which includes cells from the two grids117.

Figure 80

Half stencil and full stencil reconstruction with: A) Intersection, B) Halo-cell

6.3.2 Non-Linear Harmonic Balanced Method (NLHB) The sliding mesh method simulates the full unsteady flow, which is still quite computational expensive for industrial requirements. In the past decade, a harmonic frequency-domain methods are developed, e.g., using potential flow model and Euler equations. However, all of the previous

M. Rai, “Application of domain decomposition methods to turbomachinery flows”, ASME Advances and Applications in Computational Fluid Dynamics, volume 66, 1988. 115 Reza Amini, “Using Sliding Meshes”. 116 S. Khelladi, X. Nogueira, F. Bakir and I. Colominas, “Toward a higher-order unsteady finite volume solver Based on reproducing kernel particle method”, Computer Methods in Applied Mechanics and Engineering, Vol. 200, pp. 2348-2362, 2011. 117 Hongsik, Xiangying Chen, Gecheng Zha, “Simulation of 3D Multistage Axial Compressor Using a Fully Conservative Sliding Boundary Condition”, multistage turbomachinery are developed and implemented; Proceedings of the ASME, 2011 International Mechanical Engineering Congress & Exposition IMECE2011, November 11-17, 2011, Denver, Colorado, USA. 114

104

harmonic methods adopt the linear assumption, so that the nonlinear interaction between unsteady disturbances and the time-averaged flow is completely neglected. A nonlinear harmonic method is developed by He118 following the framework of Giles119 which is based on an asymptotic theory. In this technique Figure 81 Relative velocities obtained using HB techniques convergence of Fourierbased time methods applied to turbomachinery flows. The focus is on the harmonic balance method, which is a timedomain Fourier-based approach standing as an efficient alternative to classical time marching schemes for periodic flows. Fourier series decomposes a periodic signal into a sum of an infinite number of harmonics (sine and cosine functions) of different frequencies and amplitudes. These frequencies are discrete, not all frequencies are present. Since it is impossible to estimate an infinite series, you choose the number of terms you wish to consider, starting from the first. More the number of terms considered, closer is the series to the original signal. In the literature, no consensus exists concerning the number of harmonics needed to achieve convergence for turbomachinery stage configurations. It is shown that the convergence of Fourier-based methods is closely related to the impulsive nature of the flow solution, which in turbomachines is essentially governed by the characteristics of the passing wakes between adjacent rows. As a result of the proposed analysis, a priori estimates are provided for the minimum number of harmonics required to accurately compute a given turbomachinery configuration. Their application to several contra-rotating open-rotor configurations is assessed, demonstrating the practical interest of the proposed methodology. This method solves the steady transport equations for the time-averaged flow and the time harmonics. For turbomachinery, the Blade Passing Frequencies (BPF) are the fundamentals in time domain of the periodic disturbances from the adjacent blade rows. The solving of the generated perturbation amplitudes in a row is performed in the frequency domain by a steady transport equation associated with BPFs and subharmonics. The deterministic stresses are calculated directly from the in-phase and out-of-phase components of the solved harmonics. Using this method, only one passage is needed that saves the computational cost greatly. He et al., Vilmin et al. validated this method with simulations on a 3D radial turbine and a multistage axial compressor. Therefore, this method is adopted in the unsteady simulation of a low speed axial turbine. The physical quantity can be decomposed into a time-averaged value and a sum of perturbations, which in turn can be decomposed into N harmonics120. Figure 81 displays Harmonic function method in obtaining

L. He, “Modelling issues for computation on unsteady turbomachinery flows. In Unsteady Flows in Turbomachines”, Von K´arm´an Institute for Fluid Dynamics, 1996. 119 M. B. Giles, “An approach for multi-stage calculations incorporating unsteadiness”, ASME-GT92, number 282, Cologne, Germany, 1992. 120 S. Vilmin, E. Lorrain, and Ch. Hirsch, ” Unsteady flow modeling across the rotor/stator interface using the non-linear harmonic method”, In ASME-GT06, number 90210, Spain, 2006. 118

105

relative velocities (courtesy of NUMECA.com). Since the Harmonic method is widely used, it is warranted a bit more exploring which will be dealt in the coming section. 6.3.3 Profile Transformation (Pitch Scaling) In typical turbomachinery applications, it is very common that one or both blade rows have a prime number of blades per wheel. Formerly in such cases, it was necessary to model the whole 360° wheel in order to attain the required level of accuracy. It is possible to reduce the size of the computational problem (memory and computational time) by solving the blade row solution for one or two passages per row, while still obtaining reasonably accurate solutions, therefore providing a solution to the unequal pitch problem between the blade passages of neighboring rows. This (ANSYS121, Galpin122), a scaling procedure applied automatically to Figure 82 Phase shifted Periodic Boundary solution profiles as part of the TRS implementation, whenever the rotor-stator pitch ratio is not unity. In this approximate method, single blade passages per row with different pitch lengths can be modeled without the need to geometrically scale or modify the blade geometry. Regular periodicity is imposed for each passage and flow profiles across rotor/stator interfaces are automatically stretched or compressed as needed according to the pitch ratio while maintaining full conservation. Multiple passages can be used to reduce pitch scaling errors for the ensemble. Since this implementation is fully implicit and conservative a fast and robust transient solution can be obtained at a fraction of the time for a full domain model. While in this method overall machine performance is usually predicted well, detailed flow features such as blade passing signals will be inaccurate due to imposing instantaneous periodicity on the phase-shifted boundaries.123 6.3.4 Time Transformation Method (TT) using Phase-Shifted Periodic Boundary Conditions124 Barrowing from ANSYS CFX©, the basic principle of a phase-shifted periodic condition is that the pitch-wise boundaries R1/R2 and S1/S2 are periodic to each other at different instances in time. For example the relative position of R1 and S1 at t0 is reproduced between sides R2 and S2 at an earlier time t0-Δt. Where Δt is defined by (PR-PS)/VR. Here PR and PS are rotor and stator pitches respectively, and VR is the rotor velocity as shown in Figure 83. The Time Transformation method handles the problem of unequal pitch described above by transforming the time coordinates of the rotor and stator in the circumferential direction in order to make the models fully periodic in “transformed” time. Let the r, ϴ, and z coordinate axis represent the radial, tangential (pitch wise) and axial directions of the problem described in Figure 83. Mathematically, the condition of

ANSYS CFX Version 12 documentation, ANSYS Inc., 2009. Galpin P.F., Broberg R.B., Hutchinson B.R., “Three-Dimensional Navier Stokes Predictions of Steady State Rotor/Stator Interaction with Pitch Change”, 3rd Annual Conference of the CFD Society of Canada, June 27-1995, Banff, Alberta, Canada. 123 “A comparison of advanced numerical techniques to model transient flow in turbomachinery blade rows”, Proceedings of ASME Turbo Expo 2011 GT2011. 124 ANSYS CFX-Solver Theory Guide, Release 15, 2013. 121 122

106

enforcing the flow spatial periodic boundary conditions on both rotor and stator passages, respectively, is given by

U R1 r, θ, z, t   U R2 r, θ  PR , z, t  Δt    U R1 r, θ, z, t   U R2 r, θ  PR , z, t  U S1 r, θ, z, t   U S2 r, θ  PS , z, t  Δt    U S1 r, θ, z, t   U S2 r, θ  PS , z, t 

(18.2)

Using the following set of space-time transformations to the problem above as:

r  r , θ  θ , z  z, t  t 

Figure 83

Δt PR  PS

(18.3)

Phase Shifted Periodic Boundary Conditions

The equations that are solved are in the computational (r’, ϴ', z’, t’) transformed space-time domain and need to be transformed back to physical (r, ϴ, z, t) domain before post-processing. The periodicity is maintained at any instant in time in the computational domain and it is evident that the rotor and stator passages are marching at different time step sizes. We have the time step sizes in the rotor and stator related by their pitch ratio as:

PR ΔtS  PS Δt R

(18.4)

Where nΔtS = PR/VR and nΔtR = PS/VR. The simulation time step size set for the run is used in the stator passage(s) ΔtS and program computes the respective rotor passage time step size ΔtP based on the rotor-stator interface pitch ratio as described above. When the solution is transformed back to physical time, the elapsed simulation time is considered the stator simulation time. Required that the pitch ratio fall within a certain range, as described by the inequality:

107

1

Mω P Mω  S  1 1  M θ PR 1  Mθ

(18.5)

Where Mω is the Mach number associated with the rotor rotational speed (or signal speed in the case of an inlet disturbance problem), Mϴ is the Mach number associated with the tangential Mach number, and the ratio of PS to PR is the pitch ratio between the stationary component and the rotating component. For most compressible turbomachinery applications (for example, gas compressors and turbines), Mω is in the range of 0.3-0.6, enabling pitch ratios in the range of 0.6-1.5. Note that according to ANSYS CFX© these limits are not strict, but approaching them can cause solution instability.

6. 4

Revisiting Non-Linear Harmonic Balance (NLHB) Methodology

Given the time periodic nature of these flows, one can model the unsteady flow in turbomachines using nonlinear, harmonic balance techniques. Roughly speaking, the family of nonlinear harmonic methods expands the unsteady flow field in a Fourier series in time and solves for the Fourier coefficients. He125, and Ning126 developed a harmonic method in which the unsteady harmonics are treated as perturbations. Hall, Thomas, and Clark127 developed a full harmonic balance method, which allows for arbitrarily large disturbances and any number of harmonics. The method is computationally efficient and stores the unsteady nonlinear solutions as the working variables at several time levels over one period of unsteadiness, rather than storing the Fourier coefficients themselves. Gopinath and Jameson128 and others have applied this approach to turbomachinery applications. For an excellent recent survey of Fourier methods applied to turbomachinery applications, see the survey paper by He129. In all these methods, the harmonic balance equations are solved by introducing a pseudo-time derivative term and then marching the coupled equations to a steady state. Using the frequency-domain or time-linearized technique, it is possible to first compute the time-mean (steady) flow by solving the steady flow equations using conventional CFD techniques. One then assumes that any unsteadiness in the flow is small and harmonic in time (eiωt). The governing fluid equations of motion and the associated boundary conditions are then linearized about the mean flow solution to arrive at a set of linear variable coefficients equations that describe the small disturbance flow. The time derivatives d/dt are replaced by jω where ω is the frequency of the unsteady disturbance, so that time does not appear explicitly. The resulting time-linearized equations can be solved very inexpensively, but unfortunately cannot model dynamic nonlinearities.

He, L., 1996. “Modelling issues for time-marching calculations of unsteady flows, blade row Interaction and blade flutter”, VKI Lecture Series “Unsteady Flows in Turbomachines”, von Karman Institute for Fluid Dynamics. 126 Ning, W., and He, L., 1998. “Computation of Unsteady Flows around Oscillating Blades Using Linear and NonLinear Harmonic Euler Methods”. Journal of Turbomachinery, 120(3), pp. 508–514. 127 Hall, K. C., Thomas, J. P., and Clark, W. S., 2002. “Computation of Unsteady Nonlinear Flows in Cascades Using a Harmonic Balance Technique”. AIAA Journal, 40(5), May, pp. 879–886. 128 Gopinath, A., and Jameson, A., 2005. “Time Spectral Method for Periodic Unsteady Computations over Two and Three- Dimensional Bodies”. AIAA Paper 2005-126. 129 He, L., 2010. “Fourier methods for turbomachinery applications”. Progress in Aerospace Sciences, 46(8), pp. 329 – 341. 125

108

6.4.1 Temporal and Spatial Periodicity Requirement Consider unsteady flows that are temporally and spatially periodic. In particular, temporal and spatial periodicity requires that

U (x , t)  U (x , t  T) U (x  G , t)  U (x , t  Δt)

(18.6)

Where T is the temporal period of the unsteadiness, G is the blade-to-blade gap and Δt is the time lag associated with the inter blade phase lag. Similarly, for cascade flow problems arising from vibration of the airfoils with fixed inter blade phase angles σ, or incident gusts that are spatially periodic. As an example, consider a cascade of airfoils where the source of aerodynamic excitation is blade vibration with a prescribed inter blade phase angle σ and frequency ω. Then T = 2π/ω and Δt = σ/ω. Because the flow is temporally periodic, the flow variables may be represented as a Fourier series in time with spatially varying coefficients. 6.4.2 Boundary Conditions We first consider the flow field kinematics of two adjacent blade rows where the first row has B1 blades spinning with rotational rate ω1 rad/s and the second has B2 blades spinning with rotational rate ω2 rad/s. The flow field within the stage can be decomposed into a Fourier series in the rotational direction characterized by a set of Nm1, m2 nodal diameters as

N m1,m2  m1B1  m2 B2

(18.7)

Where m1 and m2 can take on all integer values. In the frame of reference of the first and second blade row, the frequency of the unsteady disturbance associated with any nodal diameter is

ω1,m2  m2 B2 (ω1  ω2 )

,

ω2,m1  m1B1 (ω2  ω1 )

(18.8)

Note that in either row the unsteady frequency associated with a given nodal diameter is a function of the blade count and relative rotation rate of the adjacent row. Furthermore, associated with each unsteady frequency is an inter blade phase angle:

σ1,m2  m 2 2π

B2 B1

,

σ m1 ,2  m1 2π

B1 B2

(18.9)

In the frame of reference of the second row. Clearly the inter blade phase angles associated with a given nodal diameter are a function of the pitch ratios between the two rows. Note that the pitch in each row is given by G1 = 2π/B1 and G2 = 2π/B2 in the first and second rows, respectively. 6.4.3 Solution Method Since the solution U is periodic in time, we can represent it by the Fourier series:

109

U ( x, t) 

M

 Uˆ

m M

where

m

(x) e imt

(18.10)

N 1 ~ -imt n ˆ ( x)  1  U U m n ( x, t n ) e N n 0

can considered complex conjugate of each other. Here, ω is the fundamental frequency of the disturbance, M is the number of harmonics retained in the solution: Ûm are the Fourier coefficients, and Ũn are a set of N = 2M + 1 solutions at discrete time levels tn = nT/N distributed throughout one period of unsteadiness, T. At any U is vector of conserved variables and can be expressed as

ρ (x, t)   R n (x, t) eint , ρu (x, t)   U n (x, t) eint , v(x, t)   Vn (x, t) eint ,..... n

n

(18.11)

n

At any location in the flow field domain we can transform the time level solutions into Fourier coefficients and vice versa using a discrete Fourier transform operator [E] and its corresponding inverse E−1 as follows

~ ˆ EU U

or

~ ˆ U  E1 U

(18.12)

Where E and E−1 are square matrices of dimension N × N, and the Fourier coefficients and time level solutions have been assembled into the vectors Ũ as

~ ~ ~ ~ ~ U  [U0 , U1 , U 2 , ....... UN1 ]T

(18.13)

The solutions at each discrete time level are obtained by applying the governing equations to all the Ũ simultaneously

~    U ~ ~ ~ dV  [ F  G ]  d A   S dV V t  V

(18.14)

Where the flux and source vectors F͂͂,͂͂ G̃ , and S͂͂͂͂ are evaluated using the corresponding time level solution. The time derivative in Eqn. (18.14) is evaluated by differentiating Eqn. (18.10) with respect to time and then employing Eqn. (18.12) as follows:

~ U E 1 ˆ E 1 ~ ~  U U  [D] U t t t

(18.15)

Where [D] is the pseudo-spectral, N × N matrix operator. Substituting Eqn. (18.15) for the time derivative in Eqn. (18.14) yields the desired harmonic balance equations:



V

  ~ ~ ~ ~  [D] U dV   [F  G]  dA   S dV V

(18.16)

110

The harmonic balance equations are discretized using a cell centered, polyhedral-based, finitevolume scheme. Second order spatial accuracy is achieved by means of a multi-dimensional, linear reconstruction of the solution variables. The convective fluxes are evaluated by a standard upwind, flux-difference splitting and the diffusive fluxes by a second-order central difference. A pseudo-time derivative of primitive quantities, ∂Q/∂τ, with Q = {p, u, T}, is introduced into Eqn. (18.16) to facilitate solution of the steady harmonic balance equations by means of a time marching procedure. An Euler implicit discretization in pseudo-time130 produces the following linearized system of equations:

 U S U    Δτ [ A ]   [ D ]   ΔQ  Δτ R   Q  Q  Q   

(18.17)

where R' is the discrete residual of Eqn. (18.17), and ΔQ' are the resultant primitive variable corrections across one pseudo-time step, Δτ. Operator [A] is the Jacobian of the discrete inviscid and viscous flux vectors with respect to primitive variables Q and introduces both center coefficients as well as off-diagonals arising from the linearization of the spatially discretized fluxes. The coupled system given by Eqn. (18.17) contains equations from all time levels linked at every point in the domain by the pseudo-spectral operator [D]. The result is is a large system, and solving it all at once would be rather intractable. However, we can exploit the point coupled nature of the system and employ approximate factorization to produce the following two step scheme:

 U S  ~   Δτ [ A]   ΔQ  Δτ R  Q    Q

(18.18)

 U 1 U  ~ [D]  ΔQ  ΔQ [I]  Δτ Q Q  

(18.19)

Where ΔQ̃ ' represents provisional corrections to the solution. In the first step, Eqn. (18.18), the time levels are no longer coupled and we can solve for the ΔQ̃ ' one time level at a time. With the exception of the physical time derivative appearing in Eqn. (18.18), the evaluation of fluxes, accumulation of the residual, and the process of assembling and solving Eqn. (18.16) at each time level proceeds exactly as for a single, steady-state solution in the time domain. Here we employ an algebraic multigrid (AMG) method to solve the linear system (Eqn. 18.16) and obtain the provisional ΔQ̃ ’. In the second step the complete corrections ΔQ' for the current iteration are obtained by inverting Eqn. (18.19) at each point in the domain given all the ΔQ̃ ' computed in step one. 6.4.4 Fourier 'Shape Correction' for Single Passage Time-Marching Solution The Fourier modelling approach to nonlinear flows was proposed in 1990 foTr time-marching solutions of unsteady turbomachinery flows131. This was the first Fourier method for turbomachinery. The objective at the time was to enable an unsteady flow solution to be carried out

Weiss, J. M., Maruszewski, J. P., and Smith, W. A., 1999, “Implicit Solution of Preconditioned Navier-Stokes Equations Using Algebraic Multigrid”, AIAA Journal, 37(1), Jan., pp. 29–364 131 L. He, "An Euler Solution for Unsteady Flows around Oscillating Blades", ASME, Journal of Turbomachinery, Vol.112, No.4, pp.714-722, 1990. 130

111

in a single blade passage domain but without requiring a large amount of computer memory, as in the Erdos's Direct Store method. The main ingredient is to carry out the temporal Fourier transform at the ‘periodic boundaries of the single blade passage domain. Then the Fourier harmonics (temporal shape) are used to correct the corresponding boundaries according to the phase shift periodicity. The method was then called ‘Shape Correction’. The validity of the single passage ShapeCorrection method can be examined by comparing with the direct multi-passage solution. Figure 84 shows Stagnation Pressure contours under inlet distortion for NASA Rotor 67 where the Left shows whole passage annulus solution, and the Right, single passage solution as reconstructed. It was shown that the Fourier modelling as implemented in the Shape-Correction can capture flow disturbances and responses with large nonlinearity (e.g. a large scale shock oscillation in fan blade passage under an inlet distortion of long circumferential wave length. Given only 3-5 harmonics were required for capturing sufficiently accurately the temporal variation, the computer memory requirement is very low compared to the Erdos’s Direct Store approach. A key advantage of splitting flow components represented by Fourier harmonics is the ability in dealing with multiple disturbances with distinctive frequencies (He 1992). The generalized shape correction has been applied to unsteady flows in multi-rows (IGT-rotor-stator) with vibrating rotor blades for optimization of intra-row gap effects on both aerothermal performance and flutter stability,

Figure 84

Stagnation Pressure Contours under inlet distortion for NASA Rotor 67

6.4.4 Case Study 1 – 2D Compressor Stage In this section we compare results obtained from the implicitly coupled, non-linear harmonic balance method described above with solutions from a full, unsteady simulation based on the standard dual time-stepping approach. The test case consists of a model two-dimensional compressor stage; specifically, the first stator and second rotor rows of the five row. There are three stator blades to every four rotor blades. The two blade rows are separated by an axial gap equal to 0.25 times the aerodynamic chord of the rotor. The Mach number at the inlet to the stator is 0.68 and the relative Mach number entering the rotor is 0.71. The static-to-total pressure ratio across the stage is 1.2. Three separate Euler calculations are made using the nonlinear harmonic balance method in which one, two and three harmonics, respectively, are retained for the blade passing frequencies in both the stator and rotor. Contours of instantaneous pressure, representative of the flow field within the

112

compressor stage and computed using three harmonics in each blade row, are shown in Figure 86 using nonlinear harmonic balance method. Note that computations are performed on just the center blade passage outlined in each row. The solutions shown in the passages above and below are phase-shifted reconstructions included for clarity. 6.4.5 Case Study 2 - 3D Flow in Turbine Cascade 3D flow in turbine cascade in which the Harmonic Balance (HB) method is applied for modeling rotor/stator Figure 85 Computational mesh for HB and TRS methods interaction and pressure fluctuations near trailing edges. Computational results are compared with Transient Rotor/Stator (TRS) results which shows importance of unsteady effects132. The harmonic balance method requires only a single blade passage be meshed. A structured HOH mesh is generated for each of the two blade rows, as shown in Figure 85. The inlet and exit grid planes for each of the blade rows correspond to the axial planes where test data is available. The blade passage mesh is made up of 1.3 million cells with a near wall spacing of y+ = 1.0 - 2. The HB solver models the fluid as an ideal gas with turbulence closure provided by the SpalartAllmaras turbulence model. The solver is run with a CFL number of 5.0, and separate trials are conducted retaining one, three, and five modes. The solver has converted to a periodic, unsteady Figure 86 Instantaneous pressure distribution within the compressor stage using (NLHB) solution within 4000 - 5000 iterations. The TRS solver uses a time step is equal 510-5s. This value correspond 5 steps per vane passing (10 inner iterations per time step).

132 Grigoriev A.V., Iakunin A.I.,

Kuznechov N.B., Kondratiev V.F., Kortikov N.N., “Application of Harmonic Balance Method to The Simulation of Unsteady Rotor/Stator Interaction In The Single Stage”, JSC ‘Klimov’, St - Petersburg, Russia.

113

Assessment of the effectiveness of the two methods of calculation is carried out on the basis of the comparison of time required for obtaining of non-stationary periodic solutions on the interval of time, sufficient for the passage of at least one rotation of the impeller. The HB-results showed that CPU time is increased in 7 times for 5 modes compared time when calculating with one mode. Using 3 modes CPU time is increased (for one iteration) in 3.3 times in comparison with one-mode approximation. The acceleration of the calculation, which is defined as the ratio of the CPU time required to obtain a periodic solution using the TRS method to the CPU time of the decision on the HB method is 1:2 five modes, 1:1 - three modes and 3:1 - one mode. Hence, the substantial savings (three times) is observed only in the case of one – mode approximation. It is important to note that in all cases the calculations were carried out at the same calculation grid, including two Figure 87 Instantaneous predictions of turbulent blades. Figure 88, Figure 87 present viscosity at mid-span turbine for the TRS instantaneous predictions of turbulent viscosity at mid - span for the HB and TRS solutions. The stator wake enters the rotor passage and grows both laterally and in the stream wise direction. This process continues as the stator wake is “chopped” by the leading edge of the rotor blade and convects downstream. Figure 89 Illustrates the velocity magnitude change on the interface line between two rows. Velocity profile has two minima, one of them (with great shame) corresponds to edge wakes of the vane and the second minimum is associated with upstream acting of blade leading edge on flow in axial gap.

Figure 88 Instantaneous predictions of turbulent viscosity at mid-span turbine for the HB

Figure 89

velocity profile on interface line between two rows

114

115

7

Radial Flow

Up to now we were mostly concern with Axial flows. Now we pay homage to Radial flows which designed in many everyday life tools. According to dictionary, having the working fluid flowing mainly along the radii of rotation.

7.1

Centrifugal Compressor

Centrifugal compressors, as depicted in Figure 90, sometimes termed Radial compressors, are a sub-class of dynamic axisymmetric workabsorbing turbomachinery133. The idealized compressive dynamic turbo-machine achieves a pressure rise by adding kinetic energy/velocity to a continuous flow of fluid through the rotor or impeller. This kinetic energy is then converted to an increase in potential energy/static pressure by slowing the flow through a diffuser. The pressure rise in impeller is in most cases almost equal to the rise in the diffuser section. 7.1.1 Theory of operation In the case of where flow simply passes through a straight pipe to enter a centrifugal compressor; the flow is straight, uniform and has no vorticity. As illustrated below α1 = 0°. As the flow continues to pass into and through the centrifugal impeller, the impeller forces the flow Figure 90 Centrifugal impeller with a highly to spin faster and faster. According to a form of polished surface likely to improve performance Euler's fluid dynamics equation, known as pump and turbine equation, the energy input to the fluid is proportional to the flow's local spinning velocity multiplied by the local impeller tangential velocity. In many cases the flow leaving centrifugal impeller is near the speed of sound (340 m/s). The flow then typically flows through a stationary compressor causing it to decelerate. These stationary compressors are actually static guide vanes where energy transformation takes place. As described in Bernoulli's principle, this reduction in velocity causes the pressure to rise leading to a compressed fluid. 7.1.2 Similarities to Axial Compressor Centrifugal compressors are similar to axial compressors in that they are rotating airfoil based compressors as shown in the adjacent figure.134,135 It should not be surprising that the first part of the centrifugal impeller looks very similar to an axial compressor. This first part of the centrifugal impeller is also termed an inducer. Centrifugal compressors differ from axials as they use a greater change in radius from inlet to exit of the rotor/impeller. The 1940s-era German Heinkel HeS 011 experimental aviation turbojet engine was the first aviation turbojet design to have any sort of

Shepard, Dennis G. “Principles of Turbomachinery”, McMillan. ISBN 0-471-85546-4. LCCN 56002849, 1956. Lakshminarayana, B. (1996). “Fluid Dynamics and Heat Transfer of Turbomachinery”, New York: John Wiley & Sons Inc. ISBN 0-471-85546-4. 135 Japikse, David & Baines, Nicholas C., “Introduction to Turbomachinery”, Oxford: Oxford University press. ISBN 0-933283-10-5, 1997. 133

134

116

"mixed compressor" design in its fore-sections, as it had a single-stage "diagonal flow" main compressor ahead of a triple-stage axial unit, driven by a twin-stage turbine. 7.1.3 Components of a simple Centrifugal Compressor A simple centrifugal compressor has four components: inlet, impeller/rotor, diffuser, and collector. Figure 91 shows each of the components of the flow path, with the flow (working gas) entering the centrifugal impeller axially from right to left (blue). As a result of the impeller rotating clockwise when looking downstream into the compressor, the flow will pass through the volute's discharge cone moving away from the figure's viewer. The inlet to a centrifugal compressor is typically a simple pipe. It may include features such as a valve, stationary vanes/airfoils (used to help swirl the flow) and both pressure and temperature instrumentation. All of these additional devices have important uses in the control of the centrifugal compressor.

Figure 91

Cut-away view of a turbocharger showing the centrifugal compressor

7.1.3.1 Inlet The inlet to a centrifugal compressor is typically a simple pipe. It may include features such as a valve, stationary vanes/airfoils (used to help swirl the flow) and both pressure and temperature instrumentation. All of these additional devices have important uses in the control of the centrifugal compressor. 7.1.3.2 Centrifugal Impeller The key component that makes a compressor centrifugal is the centrifugal impeller, Figure 90, which contains a rotating set of vanes (or blades) that gradually raises the energy of the working gas. This is identical to an axial compressor with the exception that the gases can reach higher velocities and

117

energy levels through the impeller's increasing radius. In many modern high-efficiency centrifugal compressors the gas exiting the impeller is traveling near the speed of sound. Impellers are designed in many configurations including "open" (visible blades), "covered or shrouded", "with splitters" (every other inducer removed) and "w/o splitters" (all full blades). Figure 91 show open impellers with splitters. Most modern high efficiency impellers use "back sweep" in the blade shape136-137. Euler’s pump and turbine equation plays an important role in understanding impeller performance. 7.1.3.3 Diffuser The next key component to the simple centrifugal compressor is the diffuser. Downstream of the impeller in the flow path, it is the diffuser's responsibility to convert the kinetic energy (high velocity) of the gas into pressure by gradually slowing (diffusing) the gas velocity. Diffusers can be vaneless, vane or an alternating combination. High efficiency vane diffusers are also designed over a wide range of solidities from less than 1 to over 4. Hybrid versions of vane diffusers include: wedge, channel, and pipe diffusers. There are turbocharger applications that benefit by incorporating no diffuser. Bernoulli's fluid dynamic principle plays an important role in understanding diffuser performance.

Figure 92

Jet engine cutaway showing the centrifugal compressor and other parts.

7.1.3.4 Collector The collector of a centrifugal compressor can take many shapes and forms. When the diffuser discharges into a large empty chamber, the collector may be termed a Plenum. When the diffuser discharges into a device that looks somewhat like a snail shell, bull's horn or a French horn, the Japikse, David. “Centrifugal Compressor Design and Performance”. Concepts ETI . ISBN 0-933283-03-2. “Centrifugal Compressors, A Strategy for Aerodynamic Design and Analysis”. ASME Press. ISBN 0-7918-0093-8. 136

137 Aungier, Ronald H. (2000).

118

collector is likely to be termed a volute or scroll. As the name implies, a collector’s purpose is to gather the flow from the diffuser discharge annulus and deliver this flow to a downstream pipe. Either the collector or the pipe may also contain valves and instrumentation to control the compressor. 7.1.4 Applications Below, is a partial list of centrifugal compressor applications each with a brief description of some of the general characteristics possessed by those compressors. To start this list two of the most wellknown centrifugal compressor applications are listed; gas turbines and turbochargers. 7.1.4.1 In gas turbines and auxiliary power units In their simple form, modern gas turbines operate on the Brayton cycle. Either or both axial and centrifugal compressors are used to provide compression. The types of gas turbines that most often include centrifugal compressors include turboshaft, turboprop, auxiliary power units, and microturbines. The industry standards applied to all of the centrifugal compressors used in aircraft applications are set by the FAA and the military to maximize both safety and durability under severe conditions. Centrifugal impellers used in gas turbines are commonly made from titanium alloy forgings. Their flow-path blades are commonly flank milled or point milled on 5-axis milling machines. When tolerances and clearances are the tightest, these designs are completed as hot operational geometry and deflected back into the cold geometry as required for manufacturing. This need arises from the impeller's deflections experienced from start-up to full speed/full temperature which can be 100 times larger than the expected hot running clearance of the impeller. 7.1.4.2 Automotive engine and diesel engine turbochargers and superchargers Centrifugal compressors used in conjunction with reciprocating internal combustion engines are known as turbochargers if driven by the engine’s exhaust gas and turbo-superchargers if mechanically driven by the engine. Ideal gas properties often work well for the design, test and analysis of turbocharger centrifugal compressor performance. 7.1.4.3 Natural gas to move the gas from the production site to the consumer Centrifugal compressors for such uses may be one or multi-stage and driven by large gas turbines. The impellers are often if not always of the covered style which makes them look much like pump impellers. This type of compressor is also often termed an API-style. The power needed to drive these compressors is most often in the thousands of horsepower (HP). Use of real gas properties is needed to properly design, test and analyze the performance of natural gas pipeline centrifugal compressors. 7.1.4.4 Oil refineries, natural gas processing, petrochemical and chemical plants Centrifugal compressors for such uses are often one-shaft multi-stage and driven by large steam or gas turbines. Their casings are often termed horizontally split or barrel. Standards set by the industry (ANSI/API, ASME) for these compressors result in large thick casings to maximize safety. The impellers are often if not always of the covered style which makes them look much like pump impellers. Use of real gas properties is needed to properly design, test and analyze their performance. 7.1.4.5 Air-conditioning and refrigeration and HVAC Centrifugal compressors quite often supply the compression in water chillers cycles. Because of the wide variety of vapor compression cycles (thermodynamic cycle, thermodynamics) and the wide variety of workings gases (refrigerants), centrifugal compressors are used in a wide range of sizes and configurations. Use of real gas properties is needed to properly design, test and analyze the performance of these machines.

119

7.1.4.6 In industry and manufacturing to supply compressed air Centrifugal compressors for such uses are often multistage and driven by electric motors. Intercooling is often needed between stages to control air temperature. Note that the road repair crew and the local automobile repair garage find screw compressors better adapt to their needs Ideal gas relationships are often used to properly design, test and analyze the performance of these machines. Carrier’s equation is often used to deal with humidity. 7.1.4.7 In air separation plants to manufacture purified end product gases Centrifugal compressors for such uses are often multistage using inter-cooling to control air temperature. Ideal gas relationships are often used to properly design, test and analyze the performance of these machines when the working gas is air or nitrogen. Other gases require real gas properties. 7.1.4.8 Oil field re-injection of high pressure natural gas to improve oil recovery Centrifugal compressors for such uses are often one-shaft multi-stage and driven by gas turbines. With discharge pressures approaching 700 bar, casing are of the barrel style. The impellers are often if not always of the covered style which makes them look much like pump impellers. This type of compressor is also often termed API-style. Use of real gas properties is needed to properly design, test and analyze their performance.

7.2

Radial turbine

A radial turbine is a turbine in which the flow of the working fluid is radial to the shaft138. The difference between axial and radial turbines consists in the way the fluid flows through the components (compressor and turbine). Whereas for an axial turbine the rotor is 'impacted' by the fluid flow, for a radial turbine, the flow is smoothly orientated perpendicular to the rotation axis, and it drives the turbine in the same way water drives a watermill. The result is less mechanical stress (and less thermal stress, in case of hot working fluids) which enables a radial turbine to be simpler, more robust, and more efficient (in a similar power range) when compared to axial turbines. When

Figure 93

Ninety degree inward-flow radial turbine stage

it comes to high power ranges (above 5 MW) the radial turbine is no longer competitive (due to heavy and expensive rotor) and the efficiency becomes similar to that of the axial turbines.

138

From Wikipedia, the free encyclopedia.

120

7.2.1 Advantages and challenges Compared to an axial flow turbine, a radial turbine can employ a relatively higher pressure ratio (≈4) per stage with lower flow rates. Thus these machines fall in the lower specific speed and power ranges. For high temperature applications rotor blade cooling in radial stages is not as easy as in axial turbine stages. Variable angle nozzle blades can give higher stage efficiencies in a radial turbine stage even at off-design point operation. In the family of hydro-turbines, Francis turbine is a very wellknown IFR turbine which generates much larger power with a relatively large impeller. 7.2.2 Types of Radial Turbines Radial flow turbines may be classified as:  Inward flow radial (IFR) turbines  Cantilever turbine  90 degree turbine (see Figure 93)  Outward flow radial (OFR) turbines (see Figure 94) 7.2.2.1 Cantilever Radial Turbine In cantilever IFR turbine the blades are limited to the region of the rotor tip extending from the rotor in the axial direction. The cantilever blades are usually of the impulse type (or low reaction), such that there is little change in relative velocity at inlet and outlet of the rotor. Aerodynamically, the cantilever turbine is similar to an axial-impulse turbine and can even be designed by similar methods. The fact that the flow is radially inwards hardly alters the design procedure because the blade radius ratio r2/r3 is close to unity anyway. 7.2.2.2 90 Degree IFR Turbine The 90° IFR turbine or centripetal turbine is very similar in appearance to the centrifugal compressor, but with the flow direction and blade motion reversed.

Figure 94

Outward Flow Radial Turbine

121

7.2.2.3 Outward-flow radial stages In outward flow radial turbine stages, the flow of the gas or steam occurs from smaller to larger diameters. The stage consists of a pair of fixed and moving blades. The increasing area of crosssection at larger diameters accommodates the expanding gas. This configuration did not become popular with the steam and gas turbines. The only one which is employed more commonly is the Ljungstrom double rotation type turbine. It consists of rings of cantilever blades projecting from two discs rotating in opposite directions. The relative peripheral velocity of blades in two adjacent rows, with respect to each other, is high. This gives a higher value of enthalpy drop per stage. (see Figure 94).

122

8

Best Practice Guidelines for Turbo Machinery CFD

Here we pay attention to the summary of the most important knowledge and experience a CFD engineer needs in order to perform CFD simulations of turbo-machinery components139. The guide is mainly aimed at axial turbo-machinery. The goal is to give a CFD engineer, who has just started working with turbo-machinery simulations, a head start and avoid some of the most difficult pit-falls. Experienced turbo-machinery CFD engineers can also use the guidelines in order to learn what other experts consider best practice. The intended audience is expected to know basic CFD terminology and have basic turbo-machinery knowledge, but no detailed knowledge about CFD for turbomachinery is needed. Before starting a new turbo machinery simulation it is wise to think carefully of what it is that should be predicted and what physical phenomena that affect the results. This chapter contains a brief overview of the various types of simulations and some hints of what can be predicted with them.

8.1

Quasi-3D (Q3D) or 3D Simulation

8.1.1 2-D Simulations These are often used in the early design phase in order to obtain a typical 2D section of a blade. For cases with many long blades or vanes, like low-pressure turbines, a 2D simulation can also provide reasonable results. If the area of the flow-path changes significantly in the axial direction it might be necessary to instead make a quasi-3D simulation. 8.1.2 Quasi-3D (Q3D) Simulation Two-dimensional flow analyses in the hub-to-shroud and blade-to-blade surfaces to approximate the 3-D flow in a blade passage. It is a 2-D simulation in which extra source terms are used to account for the acceleration/deceleration caused by a changing channel height or growing end-wall boundary layers. Codes focused on turbomachinery applications often have the possibility to perform quasi-3D simulations, but most general purpose CFD codes cannot do this type of simulations, or require user coding to implement the correct source terms in the equations. 8.1.3 Full 3D simulations Are necessary if a true 3D geometry is needed to obtain correct secondary flows and/or shock locations. For low-aspect-ratio cases with only a few short blades, like for example structurally loaded turbine outlet guide vanes, the secondary flow development is important and a 3D simulation is often necessary in order to obtain reasonable results. For applications where the end-wall boundary layers grow 3D possibility and you require it. Many codes require special routines or hidden commands to enable very quickly and interact with a large part of the flow-field it is necessary to perform a full 3D simulation. This is often the case in compressors and fans, where the negative pressure gradients make the boundary layers grow much quicker than what they do in for example turbines. For cases where the shock location is very critical, like in transonic compressors, it is also often necessary to perform a 3D simulation in order to obtain reasonable shock locations. Figure 95 shows the flow range from 2D to 3D by different vendor codes.

139

CFD on line series.

123

3D transient Solver from ANSYS

Q3D Solver from NUMECA

Figure 95

8.2

2-D Steady state transonic viscous flow

Different Flow (2D, Q3D, and full 3D)

Single vs Multi-Stage Analysis

8.2.1 Single Stage Many single-stage computations are still performed for turbomachinery design and analysis, and before the introduction of multi row computations, CFD could only be applied to single blade rows in isolation. For such computations, it is essential to ensure that the boundary conditions applied are accurate. These can be extracted from a through-flow computation of the whole machine, and this is the normal approach for design work, or alternatively, experimental measurements of the inlet and exit flow field are applied as boundary conditions. The agreement between CFD and experimental data shown here is better than average. There is a close match in the shape of all the characteristic curves and the absolute levels of pressure ratio and choking mass flow are accurately reproduced.

124

However, the stall point is not predicted accurately, and should not be expected to be, since stall is inherently unsteady and involves the full-annulus flow field. Also, at part speeds, the predicted efficiency values are noticeably lower than the measured values. 8.2.2 Multi-Stage Analysis 8.2.2.1 Steady Mixing-Plane simulations Since the mixing-plane method was first introduced in [Denton & Singh 1979] it has become the industry standard type of rotor-stator simulations. A mixing-plane simulation is steady and only requires one rotor blade and one stator blade per stage. Between the rotating blade passage and the steady vane passage the flow properties are circumferentially averaged in a so-called mixing-plane interface. This will of course remove all transient rotor-stator interactions, but it still gives fairly representative results. In some commercial codes (CFX for example) mixing-plane interfaces are also called stage-interfaces. 8.2.2.2 Steady frozen rotor simulations In a frozen rotor simulation the rotating and the stationary parts have a fixed relative position. A frame transformation is done to include the rotating effect on the rotating sections. This will give a steady flow and no transient effects are included. With a frozen-rotor simulation rotating wakes, secondary flows, leading edge pressure increases etc. will always stay in exactly the same positions. This makes a frozen rotor simulation very dependent on exactly how the rotors and the stators are positioned. Most often a mixing-plane simulation gives better results. Frozen rotor simulations are mainly performed to obtain a good starting flow-field before doing a transient sliding-mesh simulation. 8.2.2.3 Unsteady Sliding Mesh stator-rotor simulations This is the most complete type of stator-rotor simulation, and very CPU intensive. In most engines the number of stators and rotors do not have a common denominator (to avoid instabilities caused by resonance between different rings). Hence, to make a full unsteady sliding-mesh computation it is necessary to have a mesh which includes the full wheel with all stators vanes and all rotor blades. This is often not possible, instead it is necessary to reduce the number of vanes and blades by finding a denominator that is almost common and then scales the geometry slightly circumferentially. Here is an example: Real engine: 36 stator vanes, 41 rotor blades Approximated engine: 41 stator vanes, 41 rotor blades, making it possible to simulate only 1 stator vane and 1 rotor blade Scaling of stator: All stator vanes are scaled by 36/41 = 0.8780 circumferentially. 8.2.2.4 Unsteady Harmonic Balance simulations To overcome the computational costs associated with sliding mesh, a technique called Harmonic Balance is used. The analysis exploits the fact that many unsteady flows of interest in turbomachinery are periodic in time. Thus, the unsteady flow conservation variables may be represented by a Fourier series in time with spatially varying coefficients. This assumption leads to a harmonic balance form of the Euler or Navier–Stokes equations, which, in turn, can be solved efficiently as a steady problem using conventional computational fluid dynamic (CFD) methods, including pseudo time marching with local time stepping and multigrid acceleration. Figure 96 Displays a full analyses blade solution using a harmonic balanced techniques, courtesy of (CD-Adapco.com). To relax the fundamental linear assumption while taking advantage of the high solution efficiency, a nonlinear harmonic method was proposed. Similarly to the time-domain Fourier model, the unsteadiness is represented by the

125

Fourier series. But now each harmonic will be balanced (‘harmonic balancing’) respectively in the nonlinear flow equations. Consequently, for a Fourier series retaining N harmonics, we will have 2N equations for the complex harmonics. In addition, the time-averaged flow will now be different from the steady flow due to the added deterministic stresses. So in total we have 2N+1 steady-like flow equations, which are solved simultaneously to reflect the interactions between the unsteady harmonics and the time mean flows. The interactions among the harmonics are included in a more complete nonlinear harmonic formulation by Hall’s harmonic balance formulations. The nonlinear harmonic approach have been extended to effectively solve rotor-rotor/stator-stator interactions in multistage turbomachines140.

Figure 96

Full Blade Simulation using Harmonic Balanced Method

8.2.2.5 Hybrid steady-unsteady stator-rotor simulations Hybrid steady-unsteady methods have been proposed in literature (Montomoli et al., 2011) in order to have an unsteady simulation embedded in a multistage steady study. There are several advantages related to this method: mainly grid size and number of iterations. 8.2.2.6 Other advanced multi-stage methods Time-inclined, Adamszyk stresses, etc.

8.3

Inviscid or Viscid

For attached flows close to the design point and without any large separations it is often sufficient 140 L. He, T. Chen, R.G.

Wells, Y.S. Li and W. Ning, ‘Analysis of Rotor-Rotor and Stator-Stator Interferences in Multistage Turbomachines’, ASME Journal of Turbomachinery, Vol.124, No.4, pp. 564-571, Oct, 2002.

126

with an in-viscid Euler simulation in order to obtain reasonable blade loadings and pressure distributions. Note that in-viscid Euler simulations should only be used if the boundary layers are judged to not have a significant effect on the global flow-field. A viscous Navier-Stokes simulation is necessary in order to predict losses, secondary flows and separations. As soon as separations are of interest it is of course also necessary to do a viscous simulation. Note that with today’s computers it is often not time and resources that make users run in-viscid Euler simulations. Running viscous Navier-Stokes simulations is now so quick that it is not a time problem anymore. Euler simulations are still interesting though, since with an in-viscid Euler simulation you don't have to worry about wall resolutions, y+ values, turbulence modeling errors etc.

8.4

Transient or Steady-State

Most turbo-machinery simulations are performed as stationary simulations. Transient simulations are done when some kind of transient flow behavior has a strong influence on the global flow field. Examples of transient simulations are detailed simulations of rotor-stator interaction effects, simulations of large unsteady separations etc. Sometimes when you perform a steady stationary simulation you can see tendencies of unsteady behavior like for example periodic vortex shedding behind blunt trailing edges. This is often first seen as periodical variations of the residuals. If the unsteady tendencies are judged to not Figure 97 Transient Blade Row extensions enable efficient multistage CFD simulation affect the overall simulation results it might be necessary to coarsen the mesh close to the vortex shedding or run a different turbulence model in order to make the simulation converge. Sometimes you are still forced to run a transient simulation and average the results if you don't obtain a converged steady solution. Figure 97 shows the transient blade row extensions enable efficient multi-stage CFD simulation ( courtsys of ANAYS.com).

8.5

Meshing

In turbomachinery applications structured multi-block hexahedral meshes are most often used for flow-path simulations. In most solvers a structured grid requires less memory, provides superior accuracy and allows a better boundary-layer resolution than an unstructured grid. By having cells with a large aspect ratio around sharp leading and trailing edges a structured grid also provides a better resolution of these areas. Many companies have automatic meshing tools that automatically mesh blade sections with a structured mesh without much user intervention. Unstructured meshes are used for more complex and odd geometries where a structured mesh is difficult to create. Typical examples where unstructured meshes are often used are blade tip regions, areas involving leakage

127

flows and secondary air systems, film cooling ducts etc. When meshing avoid to create large jumps in cell sizes. Typically the cell size should not change with more than a factor of 1.25 between neighboring cells. For structured meshes also try to create fairly continues mesh lines and avoid discontinuities where the cell directions suddenly change. For multiblock structured meshes avoid placing the singular points where blocks meet in regions with strong flow gradients since most schemes have a lower accuracy in these singular points. Figure 98 shows a typical meshing for a turbomachinery stage.

Figure 98

Typical meshing of a Turbomachinery stage

8.5.1 Mesh size Guidelines It is difficult to define, a priori, the mesh size. The required mesh size depends on the purpose of the simulation. If the main goal is to obtain static pressure forces a coarse mesh is often able to obtain a good solution, especially when an accurate resolution of the boundary layers is not required. For 2D in-viscid simulations of one blade a mesh with say 3,000 cells is most often sufficient. For 3D in-viscid blade simulations a mesh size of about 40,000 cells is usually sufficient. On in-viscid Euler simulations the cells should be fairly equal in size and no boundary layer resolution should be present. Avoid having too skewed cells. For loss predictions and cases where boundary layer development and separation is important the mesh needs to have a boundary layer resolution. The boundary layer resolution can either be coarse and suitable for a wall function simulation or very fine and suitable for a low-Re simulation. For further information about selecting the near-wall turbulence model please see the turbulence modeling section. In 3D singleblade simulations a decent wall-function mesh typically has around 100,000 cells. This type of mesh size is suitable for Figure 99 Multi-block grid for the space shuttle main engine fuel quick design iterations where it turbine is not essential to resolve all secondary flows and vortices.

128

A good 3D wall-function mesh of a blade section intended to resolve secondary flows well should have at least 400,000 cells. A good low-Re mesh with resolved boundary layers typically has around 1,000,000 cells. In 2D blade simulations a good wall-function mesh has around 20,000 cells and a good low-Re mesh with resolved boundary layers has around 50,000 cells. Along the suction and pressure surfaces it is a good use about 100 cells in the stream wise direction. In the radial direction a good first approach is to use something like 30 cells for a wall-function mesh and 100 cells for a low-Re mesh. It is important to resolve leading and trailing edges well. Typically at least 10 cells, preferably 20 should be used around the leading and trailing edges. For very blunt and large leading edges, like those commonly found on HP turbine blades, 30 or more cells can be necessary. Cases which are difficult to converge with a steady simulation and which show tendencies of periodic vortex shedding from the trailing edge, can sometimes be "tamed" by using a coarse mesh around the trailing edge. This, of course, reduces the accuracy but can be a trick to obtain a converged solution if time and computer resources do not allow a transient simulation to be performed. Figure 99 shows a multi-block grid for the space shuttle main engine fuel turbine (AIAA 98-0968). 8.5.2 Boundary Mesh Resolution For design iteration type of simulations where a wall function approach is sufficient y+ for the first cell should be somewhere between 20 and 200. The outer limit is dependent on the actual Re number of the simulations. For cases with fairly low Re numbers make sure to keep the maximum y+ as low as possible. For more accurate simulations with resolved boundary layers the mesh should have a y+ for the first cell which is below 1. Some new codes are now using a hybrid wall treatment that allows a smooth transition from a coarse wall-function mesh to a resolved low-Re mesh. Use some extra care when using this type of hybrid technique since it is still fairly new and unproven. Outside of the first cell at a wall a good rule of thumb is to use a growth ratio normal to the wall in the boundary layer of maximum 1.24. For a low-Re mesh this usually gives around 40 cells in the boundary layer whereas a wall-function mesh does not require more than 10 cells in the boundary layer. If you are uncertain of which wall distance to mesh with you can use a y+ estimation tool to estimate the distance needed to obtain the desired y+. These estimation tools are very handy if you have not done any previous similar simulations. As a rule of thumb a wall-function mesh typically requires around 5 to 10 cells in the boundary layer whereas a resolved low-Re mesh requires about 40 cells in the boundary layer. 8.5.3 Periodic Meshing To reduce the time, efforts and complexity of meshing the rotational periodicity of the impeller geometry is taken advantage. Axial machines and rotating fluid zone of radial & mixed flow machines are meshed using this approach. Choosing a single periodic flow passage is the first step in this approach. The periodic angle of the flow passage is decided by the number of vanes/blades present. For example, Periodic angle or Angle of Rotational Periodicity = 360°/number of blades.  

For a radial turbine with 16 blades, Angle of rotational periodicity → 360°/16 =22.5° (single blade passage) For a pump with 4 blades, Angle of rotational periodicity → 360°/4 =90° (single blade passage)

This periodic geometric sector can be chosen in two different ways.

129

 

Flow passage between two blades (suction side of first blade to the pressure side of next blade). To have one complete blade inside the periodic flow passage.

There are two different scenarios based on the flow physics. If the flow physics is also periodic (most axial flow machines), the mesh is generated only for a single blade fluid passage (ϴ), regardless of the number of blades and is directly used for simulation. But if the flow physics is not periodic (radial & mixed flow machines with volute), the mesh is generated for the single periodic flow passage / sector and is copy rotated to get mesh for the complete geometry (360°). Meshing software provides an option for periodic meshing to ensure both sides of periodic passage has same number of nodes and same node location with a rotational offset of ϴ.

8.6

Boundary Conditions

Turbomachinery CFD employs multi-region approach, the computational model is split into a number of regions. Any number of regions is allowed. Each region has its own independent mesh and case set-up. Regions are like serial connected and communicate via interfaces. Typically, velocity is prescribed at the inlet and pressure is prescribed at the outlet. Describing different types of boundary conditions and when they should be used not easy as it sound. For each of the analysis methods, boundary conditions must be specified at the inlet and exit of the computational domain. In addition, for averaging plane methods, average flow properties must be transferred between the blade rows at grid interfaces141. It is common practice to force the flow to be axisymmetric at these boundaries. Although axisymmetric boundary conditions are simple to apply and tend to be numerically robust, they can reflect outgoing waves and thereby hinder convergence and contaminate the interior solution. Axisymmetric boundary conditions can be particularly bad at the inlet of transonic compressors or at the exit of transonic turbines, and between closely-spaced Figure 100 Pressure contour plot, 2nd order spatial discretization scheme

Rodrick V. Chima, “Calculation of Multistage Turbomachinery Using Steady Characteristic Boundary Conditions”, AIAA 98-0968. 141

130

blade rows. Giles142 presented a unified theory for the construction of Non-reflecting boundary conditions for the Euler equations (NRBC’s). The boundary conditions are based on the linearized Euler equations written in terms of perturbations of primitive variables about some mean flow. Wave-like solutions are substituted into the flow equations, and the solution is circumferentially decomposed into Fourier modes. The zeroth mode corresponds to the mean flow and is treated according to one-dimensional characteristic theory. This allows average changes in incoming characteristic variables to be specified at the boundaries. Simply put, since the numerical solution is calculated on a truncated finite domain, and one must prevent any nonphysical reflections of outgoing waves at the far-field boundaries that could contaminate the numerical solution. This becomes essential in turbomachinery applications in which the boundaries are often not very far from the blades, because the physical spacing between the blade rows can be quite small. It therefore becomes highly important for an accurate simulation to construct nonreflecting boundary conditions (NRBCs). Preventing spurious reflections that would corrupt the solution is not only important to get an accurate prediction of the flow field, but also to get more efficient computations; convergence rate is enhanced due to an improvement of the transmission of outgoing waves, allowing smaller meshes to be used143. Figure 100 compares a contour plot the pressure Vs. y-coordinate for both Riemann BC and NRBC’s in a supersonic cascade for a 2-D flow (F. De Raedt, 2015). The most notable observation is that at the outflow, when Riemann BC are applied, the pressure lines diverge from the boundary and rarely cross that boundary. This is a direct result of the reflectivity of the boundary conditions. When the boundary is far away from the airfoil, the effectiveness of these reflections on the airfoil flow-field is minimal, as observed by comparing the long flow-field simulations of the Riemann BC and NRBC. However when the boundary is close to the airfoil, the simulations using Riemann BC become completely inaccurate. In contrast the short flow-field simulations using the NRBC result in very similar pressure contours to those of the long flow-field. This clearly demonstrates the effect of the NRBC implementation. One can have a closer look at the boundary itself to further clarify this comparison144.

8.7

Turbulence Modeling

Selecting a suitable turbulence model for turbo-machinery simulations can be a challenging task. There is no single model which is suitable for all types of simulations. Which turbulence model CFD engineers use has as much to do with beliefs and traditions as with knowledge and facts? There are many different schools. However, below follows some advices that most CFD engineers in the turbomachinery field tend to agree upon. For attached flows close to the design point a simple algebraic model like the Baldwin-Lomax model can be used. Another common choice for design-iteration type of simulations is the one-equation model by Spalart-Allmaras. This model has become more popular in the last years due to the many inherent problems in more refined two-equation models. The big advantage with both the Baldwin-Lomax model and the Spalart-Allmaras model over more advanced models is that they are very robust to use and rarely produce completely unphysical results. In order to accurately predict more difficult cases, like separating flows, rotating flows, flows strongly affected by secondary flows etc. it is often necessary to use a more refined turbulence model. Common choices Giles, Michael B., “Nonreflecting Boundary Conditions for Euler Equation Calculations,” AIAA Journal, Vol. 28, No. 12, Dec. 1990, pp. 2050-2058. 143 “Three-Dimensional Nonreflecting Boundary Conditions for Swirling Flow in Turbomachinery”, Journal of Propulsion and Power Vol. 23, No. 5, September–October 2007. 144 F. De Raedt, “Non-Reflecting Boundary Conditions for non-ideal compressible fluid flows”, Master of Science at the Delft University of Technology, 2015. 142

131

are two-equation models like the k-ε model. Two-equation models are based on the Boussinesq eddy viscosity assumption and this often leads to an over-production of turbulent energy in regions with strong acceleration or deceleration, like in the leading edge region, regions around shocks and in the suction peak on the suction side of a blade. To reduce this problems it is common to use a special model variant using, for example, Durbin's realizability constraint or the Kato-Launder modification. Note that different two-equation models behave differently in these problematic stagnation and acceleration regions. Worst is probably the standard κ-ε, model, κ-ω model are slightly better but still do not behave well. More modern variants like Menter's SST κ-ω model also has problems, whereas the v2f model by Durbin behaves better.

8.8

Aero-Mechanics

Now let’s look at the challenges of aeromechanics. Whereas the aerodynamicist generally prefers designs with very thin blades, the structural engineer prefers thick blades to minimize stress and optimize vibration characteristics. Those interested in material cost and weight would no doubt side with the aerodynamicist, whereas those responsible for honoring the machine warranty would favor the structural viewpoint. Achieving agreement requires a balance, and that is where the field of aeromechanics comes in. Aeromechanics is by no means new. What is new is the fidelity with which engineers can practically consider both the fluid mechanics and the structural aspects of the solution. The real behavior of rotating blades is indeed very complex, and the mechanical loads are very high. For example, a single low-pressure steam turbine blade rotating at operating speed generates a load of several hundred tons! Long, thin blades are susceptible to vibration. Engineers strive to design blades whose natural frequencies do not coincide with the disturbances that arise due to operating speed, etc. That is complicated enough, but there are also periodic disturbances that can originate from more distant blade rows or aerodynamic effects145.

Figure 101

145

ANSYS Blog.

Analysis provided vibration required for flutter analysis

132

In the past, analysis of fluids and structural dynamics was mostly separate and simplified. But for some time, at least in principle, the ability to perform high-fidelity coupled analysis has been available. In reality, solving for time-dependent, three-dimensional fluid-structure interaction is very time-consuming and expensive, even on today’s high performance computing systems. Engineers have opted for more practical, usually disconnected and often lower-fidelity analysis methods. Recently, practical yet high-fidelity multiple physics solution methods have emerged. Prediction of aerodynamic blade damping, or “flutter,” is one such method. The procedure is to first solve for the mechanical modes of vibration, and then feed that information to the CFD simulation. The unsteady CFD simulation deforms the blade in the presence of the flow field and predicts whether the blade is aerodynamically damped, and hence stable, or not. This high-fidelity approach is practical because it provides a solution to the full wheel (all of the many blades in a given row) by solving only for one or at most a few blades in the blade row of interest. Cyclic symmetry is the enabling structural technology here, while the Fourier Transformation method is key on the CFD side. Tightly coupled these two efficient methods provides great advances in computing fidelity and speed. Predicting forced response is essentially the inverse workflow to flutter. Figure 101 shows where analysis provides the mechanical modes of blade vibration required for flutter analysis. First, the unsteady fluid dynamic loads are predicted, and made available to the structural solver. After a mechanical harmonic response simulation, the engineer evaluates the results for acceptable levels of blade displacement, strain and stress. The concept of Nodal Diameter is explained next. 8.8.1 Nodal Diameter Natural frequency is the frequency at which an object vibrates when excited by force. At this frequency, the structure offers the least resistance to a force and if left uncontrolled, failure can occur. Mode shape is deflection of object at a given natural frequency. A guitar string is a good example of natural frequency and mode shapes. When struck, the string vibrates at a certain frequency and attains a deflected shape. The eigenvalue (natural frequency) and the accompanying eigenvector (mode shape) are calculated to define the dynamics of a structure. A turbine bladed disk has many natural frequencies and associated mode shapes. In the case of a bladed disk, the mode shapes have been described as Figure 102 Examples of Nodal Diameter nodal diameters. The term nodal diameter is derived from the appearance of a circular geometry, like a disk, vibrating in a certain mode. Mode shapes contain lines of zero out-of-plane displacement which cross the entire disk as shown in Figure 102. In other words, a node line is a line of zero displacement and the displacement is out of phase on the sides of the line represented by white and gray shades in Figure 102. These are commonly called nodal diameters. Hence the natural frequency and nodal diameter are required to describe a bladed disk mode146.

8.9

Near Wall Treatment

For on-design simulations without any large separated regions it is often sufficient to use a wallMohamed Hassan, “Vibratory Analysis of Turbomachinery Blades”, Master of Mechanical Engineering, Rensselaer Polytechnic Institute, Hartford, Connecticut, December, 2008. 146

133

function model close to the wall, preferably with some form of non-equilibrium wall-function that is sensitized to stream wise pressure gradients. For off-design simulation, or simulations involving complex secondary flows and separations, it is often necessary to use a low-Re model. There exist many low-Re models that have been used with success in turbo machinery simulations. A robust and often good choice is to use a one-equation model, like for example the Wolfstein model, in the inner parts of the boundary layer. There are also several Low-Re κ-ε models that work well. Just make sure they don't suffer from the problem with overproduction of turbulent energy in regions with strong acceleration or deceleration. In the last few years Menter's low-Re SST κ-ω model has gained increased popularity.

8.10

Transition Prediction

Transition refers to the process when a laminar boundary layer becomes unstable and transitions to a turbulent boundary layer. There are two types of transition - natural transition, where inherent instabilities in the boundary layer cause the transition and by-pass transition, where convection and diffusion of turbulence from the free-stream into the boundary layer cause the transition. Most transitions in turbo machinery are by-pass transitions caused by free-stream turbulence and other external disturbances like wakes, vortices and surface defects. Simulating transition in a CFD code accurately is very difficult. Often a separate transition model needs to be solved in order to specify the transition location and length. Predicting natural transition in a pure CFD code is not possible. Predicting by-pass transition in a pure CFD code is almost impossible, although there are people who claim to be able to predict by-pass transition with low-Re two-equation models. However, this is usually on special test cases and with simulations that have been tuned for these special cases, see for example [Saville 2002]. In reality transition is a very complex and sensitive process where disturbances like incoming wakes and vortices from previous stages, surface roughness effects and small steps or gaps in the surfaces play a significant role. The turbo machinery codes that have transition prediction models often use old ad-hoc 147 models like the Abu-Ghannam and Shaw model [Abu-Ghannam 1980] or the Mayle model [Mayle 1991]. These models can be quite reliable if they have been validated and tuned for a similar application. Do not trust your transition predictions without having some form of experimental validation. Menter has also recently developed a new form of transition model that might work fairly well, but it is still too new and untested. For some turbo machinery applications, like modern high-lift low-pressure turbines, transition is critical. For these applications a CFD code with a transition model that has been tuned for this type of applications should be used.

8.11

Numerical Consideration

Use at least a second order accurate scheme for the flow variables. Some codes require a first order scheme for the turbulent variables (κ - ε) in order to converge well. It might be sufficient with a first order scheme only on the turbulence variables, but a second order scheme is of course preferable.

8.12

Convergence Criteria

To know when a solution is converged is not always that easy. You need some prior experience of your CFD code and your application to judge when a simulation is converged. For normal pure aero

147

Latin phrase meaning “for this purpose”.

134

simulations without resolved walls, i.e. with wall functions or in-viscid Euler simulations, convergence can most often be estimated just by looking at the residuals. Exactly what the residuals should be is not possible to say, it all depends on how your particular code computes and scales the residuals. Hence, make sure to read the manuals and plot the convergence of a few global parameters before you decide what the residuals should be for a solution to converge. Note also that many manuals for general purpose CFD codes list overly aggressive convergence criteria that often produce un-converged results. For simulations with resolved walls it is good to look at the convergence of some global properties, like total pressure losses from the inlet to the outlet. For heat transfer simulations it is even trickier since the aerodynamic field can look almost converged although the thermal field is not converged at all. If doing heat transfer simulations make sure to plot the heattransfer, run for some time, and plot it again to make sure that it doesn't change anymore. With very well resolved walls and heat transfer it can sometimes take 10 times longer for the thermal field to converge.

8.13

Single or Double Precision

With today’s computers and cheap memory prices it often does not cost much extra to run in double precision. Before using single precision you should first investigate how your software and hardware works with double precision. If the extra time and memory needed for double precision is negligible you should of course always run in double precision. With double precision you never have to worry about round-off errors. Always using double precision is one way of avoiding one type of pit-falls in the complex world of CFD simulations. Use double precision when you have resolved boundary layers (Y+ around 1) and when you use advanced physical models like combustion, free-surface simulations, spray and transient simulations with quick mesh motions.

8.14

Heat Transfer Prediction

Besides listing the general heat transfer mechanisms involved (namely conduction, convection, radiation) heat transfer prediction in CFD may be seen as or split into two cases. Mesh consists of fluid domain(s): you want to know how heat inserted into the fluid domain (e.g. via the flowing medium) changes the temperature field along the flow path. Be it a steady or transient run, a fluid which enters with a given temperature will usually experience temperature variations, for instance, caused by convective boundary conditions, prescribed temperature profiles at flow obstacles etc. Mesh consists of fluid and solid domain(s): additionally to the above, you want info too w.r.t .the (spatial, temporal or even spectral) temperature field distribution in surrounding, confining or immersed solids like channel walls or heat exchanger tubes. This is also called conjugate heat transfer CHT in the CFD context. CHT requires a good boundary layer resolution; usually the wall mesh needs to be rather refined, to obtain realistic heat flux results at the fluid/solid interface. Flow and heat transfer convergence require different time step settings, to properly capture changes in flow and heat quantities respectively. In either case, verify (strict necessity depends on CFD code used, CFX for instance checks and assists in regard) that model dimensions, boundary conditions and properties are in consistent units, hold appropriate values. Check temperature-dependence of properties and other numbers before the run. In heat transfer predictions (depending on the CFD code in use) besides the flow solver, you may have to activate the thermal solver too, as a job specification.

135