Content uploaded by Ideen Sadrehaghighi
Author content
All content in this area was uploaded by Ideen Sadrehaghighi on Jan 19, 2024
Content may be subject to copyright.
Content uploaded by Ideen Sadrehaghighi
Author content
All content in this area was uploaded by Ideen Sadrehaghighi on Mar 07, 2023
Content may be subject to copyright.
Multiphase
Flow
Multicomponent
Flow
Multiscale Flow
CFD Open Series/Patch 2.35
Multiphase/Multicomponent &
Multiscale Flows with Case
Studies
Adapted and Edited by : Ideen Sadrehaghighi
Table of Contents
1 Introduction ............................................................................................................................... 10
1.1 Multiphase Flow .................................................................................................................................................. 10
1.1.1 Solids Phase ............................................................................................................................................... 11
1.1.2 Liquids Phase ............................................................................................................................................ 11
1.1.3 Gases Phase ............................................................................................................................................... 11
1.1.4 Phase Rule .................................................................................................................................................. 11
1.1.4.1 Pure Substances (one component)............................................................................................ 12
1.2 Multicomponent Flow ....................................................................................................................................... 12
1.2.1 Multiphase vs Multicomponent ........................................................................................................ 13
1.3 Multiscale Flow .................................................................................................................................................... 13
2 Multiphase Flows ...................................................................................................................... 15
2.1 Preliminaries ......................................................................................................................................................... 15
2.2 Equations of Multiphase Flow ....................................................................................................................... 15
2.3 Multiphase Coupling .......................................................................................................................................... 16
2.4 Examples of Multiphase Flow ........................................................................................................................ 16
2.5 Guidelines for Selecting a Multiphase Model ........................................................................................... 18
2.6 Volume Averaging Formulation .................................................................................................................... 18
2.6.1 Constitutive Relations ........................................................................................................................... 20
2.7 Modeling Approach Defined Based on Interface Physics ................................................................... 21
2.7.1 Comparison of Computational Multiphase Flows ..................................................................... 23
2.7.2 Physics of Eulerian Multiphase Models ......................................................................................... 25
2.7.3 Volume of Fluid (VOF) Model ............................................................................................................ 25
2.7.3.1 Case Study 1 - VOF Simulation for Stratified Oil-Water Two-Phase Flow in a
Horizontal Pipe .................................................................................................................................................... 27
2.7.3.1.1 Introduction ............................................................................................................................ 27
2.7.3.1.2 Literature Survey .................................................................................................................. 27
2.7.3.1.3 Numerical Simulation (Geometry and Mesh) ........................................................... 28
2.7.3.1.4 Boundary Conditions .......................................................................................................... 28
2.7.3.1.5 Solution Strategy And Convergence ............................................................................. 29
2.7.3.1.6 Results ....................................................................................................................................... 29
2.7.3.1.7 Grid Independent Study ..................................................................................................... 30
2.7.3.1.8 Pressure Prediction at Different Flow Velocity ....................................................... 30
2.7.3.1.9 Conclusions ............................................................................................................................. 30
2.7.3.1.10 Reference ................................................................................................................................. 31
2.7.3.2 Case Study 2 - Application of Volume Of Fluid (VOF) Method for Prediction of
Wave Generated by Flow around Cambered Hydrofoil on a Free Surface ................................. 32
2.7.3.2.1 Introduction ............................................................................................................................ 32
2.7.3.2.2 Theoretical Formulation.................................................................................................... 33
2.7.3.2.3 Numerical Simulation ......................................................................................................... 35
2.7.3.2.4 Results and Discussion ....................................................................................................... 36
2.7.3.2.5 Conclusions ............................................................................................................................. 39
2.7.3.2.6 References ............................................................................................................................... 39
2.7.3.3 Case 3 - Numerical Simulations of Submarine Self-propulsion Flows near the Free
Surface 40
2.7.3.3.1 Abstract .................................................................................................................................... 40
2.7.3.3.2 Introduction ............................................................................................................................ 40
2.7.3.3.3 Methodology ........................................................................................................................... 41
2.7.3.3.4 Submarine and Propeller Geometries.......................................................................... 41
2.7.3.3.5 Governing Equations and Turbulence Model ........................................................... 42
2.7.3.3.6 Free Surface Model .............................................................................................................. 43
2.7.3.3.7 Computational Domain and Boundary Conditions ................................................. 43
2.7.3.3.8 Self-Propulsion Simulation Method .............................................................................. 43
2.7.3.3.9 Mesh Generation and Validation .................................................................................... 44
2.7.3.3.10 Results and Discussions ..................................................................................................... 45
2.7.3.3.11 Hydrodynamic Forces ........................................................................................................ 45
2.7.3.3.12 Wave-Making Characteristics .......................................................................................... 45
2.7.3.3.13 Flow Field Characteristics ................................................................................................ 46
2.7.3.3.14 Vortex Structures ................................................................................................................. 47
2.7.3.3.15 Conclusions ............................................................................................................................. 47
2.7.3.3.16 References ............................................................................................................................... 49
2.8 Eulerian Multiphase Model ............................................................................................................................. 50
2.8.1 Case Study 3 - Comparison of Eulerian and VOF Models ...................................................... 51
2.8.1.1 Introduction & Literature Survey .............................................................................................. 52
2.8.1.2 Theoretical Frame ............................................................................................................................ 53
2.8.1.2.1 Flow Patterns ......................................................................................................................... 53
2.8.1.2.2 Mathematical Models .......................................................................................................... 54
2.8.1.2.3 Eulerian Model ...................................................................................................................... 54
2.8.1.2.4 VOF Model ............................................................................................................................... 55
2.8.1.2.5 Turbulence Model ................................................................................................................ 55
2.8.1.2.6 Methodology ........................................................................................................................... 56
2.8.1.2.7 Test Matrix .............................................................................................................................. 56
2.8.1.3 Mesh Generation ............................................................................................................................... 56
2.8.1.4 Stability Criterion ............................................................................................................................. 57
2.8.1.5 Results and Analysis ........................................................................................................................ 57
2.8.1.5.1 Geometry Meshing ............................................................................................................... 57
2.8.1.5.2 Case Studies ............................................................................................................................ 58
2.8.1.6 Conclusions ......................................................................................................................................... 60
2.8.1.7 References ........................................................................................................................................... 61
2.9 Multiphase Flow Instability Mechanisms.................................................................................................. 62
2.10 3 - Phase Flow ....................................................................................................................................................... 62
2.11 Poly-Dispersed Flow .......................................................................................................................................... 62
2.12 Homogeneous & Inhomogeneous Multiphase Flow ............................................................................. 62
2.13 Multi-Component Multiphase Flow ............................................................................................................. 63
2.14 Free Surface Flow ................................................................................................................................................ 63
2.15 Surface Tension.................................................................................................................................................... 63
2.16 Mixture Model ...................................................................................................................................................... 63
2.17 Dispersed Phase Model (DPM) ...................................................................................................................... 63
2.18 Porous Bed Model ............................................................................................................................................... 64
2.19 Some Thought in Multiphase CFD for Industrial Processes .............................................................. 64
3 Multicomponent Flow ............................................................................................................. 68
3.1 Preliminary ............................................................................................................................................................ 68
3.2 Integral and Differential Balances on Chemical Species ..................................................................... 70
3.2.1 Molar Basis ................................................................................................................................................ 70
3.2.2 Mass Basis .................................................................................................................................................. 71
3.3 Diffusion Fluxes ................................................................................................................................................... 72
3.4 Fick's Law ............................................................................................................................................................... 73
3.4.1 Species' Balances for Systems Obeying Fick's Law ................................................................... 74
3.5 Case Study - Assessment of an Open-Source Pressure-Based Real Fluid Model for Trans-
critical Jet Flows............................................................................................................................................................... 74
3.5.1 Abstract ....................................................................................................................................................... 75
3.5.2 Introduction .............................................................................................................................................. 75
3.5.3 Case Setup .................................................................................................................................................. 76
3.5.4 Model Description & Governing Equations .................................................................................. 77
3.5.5 Results and Discussion ......................................................................................................................... 77
3.5.6 Conclusions ............................................................................................................................................... 81
3.5.7 References.................................................................................................................................................. 81
4 Multiscale Modeling ................................................................................................................. 84
4.1 Traditional Approaches to Modeling .......................................................................................................... 84
4.2 Multiscale Modeling ........................................................................................................................................... 85
4.2.1 Sequential Multiscale Modeling ........................................................................................................ 86
4.2.2 Concurrent Multiscale Modeling ...................................................................................................... 86
4.2.3 Two Types of Multiscale Problems .................................................................................................. 86
4.2.4 Modeling Approach defined based on Length Scale ................................................................. 86
4.2.4.1 Micro Approach (Fluid–Micro, Particle-Micro) .................................................................... 87
4.2.4.2 Meso Approach (Fluid–Meso, Particle-Meso) ....................................................................... 87
4.2.4.3 Macro Approach (Fluid–Macro, Particle-Macro) ................................................................. 87
4.2.4.4 MacroMicro Approach (Fluid–Macro, Particle-Micro) .................................................... 87
4.2.4.5 MesoMicro Approach (Fluid–Meso, Particle-Micro) ........................................................ 88
4.2.5 Block-Spectral Method of Solution .................................................................................................. 89
5 Case Studies for Composite Fluid ........................................................................................ 90
5.1 Case Study 1 - Liquid-Particle Suspension ............................................................................................... 90
5.2 Case Study 2 - Two Fluid Flow ....................................................................................................................... 90
5.2.1 Mixture Viscosity .................................................................................................................................... 90
5.2.2 Drag force ................................................................................................................................................... 90
5.3 Case Study 3 - Unsteady MHD Two Phase Flow of Fluid-Particle Suspension Between Two
Concentric Cylinders ..................................................................................................................................................... 92
5.3.1 Literature Survey and Background ................................................................................................. 92
5.3.2 Mathematical Formulation ................................................................................................................. 93
5.3.3 Analytical Approach ............................................................................................................................... 95
5.3.4 Comparison with Numerical .............................................................................................................. 95
5.4 Case Study 4 - Simulation of Compressible 3-Phase Flows in an Oil Reservoir ........................ 97
5.4.1 Mathematical Modeling ........................................................................................................................ 97
5.4.2 Temporal and Spatial Discretization Methods ........................................................................... 98
5.4.3 Results and Discussion ......................................................................................................................... 99
5.5 Case Study 5 - Effects of Mass Transfer & Mixture of Non-Ideality on Multiphase Flow ... 100
5.5.1 Mathematical Model ........................................................................................................................... 100
5.5.1.1 Bulk Species Transport ............................................................................................................... 101
5.5.1.2 Interphase Mass Transfer .......................................................................................................... 101
5.5.2 Simulation Procedure ........................................................................................................................ 102
5.5.3 Results and Discussion ...................................................................................................................... 102
5.5.4 Concluding Remarks ........................................................................................................................... 103
5.6 Case Study 6 - Numerical Study of Turbulent Two-Phase Coquette Flow ................................ 103
5.6.1 Motivation and Literature Survey ................................................................................................. 103
5.6.2 Objectives ................................................................................................................................................ 105
5.6.3 Problem Statement.............................................................................................................................. 105
5.6.4 Governing Equations and Numerical Method .......................................................................... 105
5.6.5 Initial and Boundary Conditions.................................................................................................... 106
5.6.6 Grid Resolution and Time Step Requirement .......................................................................... 106
5.6.6.1 Turbulent Length Scale ............................................................................................................... 106
5.6.6.2 Interface Length Scale .................................................................................................................. 106
5.6.7 Results ...................................................................................................................................................... 107
5.6.8 Influence of the Water Depth .......................................................................................................... 109
5.6.9 Conclusions ............................................................................................................................................ 109
5.7 Case Study 7 - Slug Flow in Horizontal Air and Water Pipe Flow ................................................ 110
5.7.1 Slug Flow and Slug Formation in Pipe......................................................................................... 111
5.7.2 Baker Chart ............................................................................................................................................. 111
5.7.3 Problem Formulation ......................................................................................................................... 112
5.7.3.1 Boundary Condition...................................................................................................................... 113
5.7.4 Volume of Fluid (VOF) ....................................................................................................................... 114
5.7.5 Results and Discussion ...................................................................................................................... 115
5.7.5.1 Slug Initiation .................................................................................................................................. 115
5.7.5.2 Slug Length ....................................................................................................................................... 115
5.7.5.3 Slug Volume Fraction ................................................................................................................... 116
5.8 Case Study 8 – Physical & Numerical Modeling of Unsteady Cavitation Hydrodynamics . 117
5.8.1 Background and Literature Survey .............................................................................................. 117
5.8.2 Physical Modeling ................................................................................................................................ 119
5.8.3 Numerical Modeling............................................................................................................................ 119
5.8.4 Modified Volume-of-Fluid Method (VOF) for Simulation of Cavitation Clouds ......... 119
5.8.5 Numerical Results for Unsteady Cavitation Flow Over NACA 0015 Hydrofoil .......... 123
5.8.6 Variation of Location of σref Without Free Surface ................................................................ 123
5.8.7 Interaction of Free Surface and Cavitation Dynamics .......................................................... 125
5.9 Case Study 9 - Distribution of 3 - Phase Flow in Vertical Pipe ...................................................... 125
5.9.1 Introduction & Literature Survey ................................................................................................. 125
5.9.2 Numerical Simulation ........................................................................................................................ 126
5.9.3 Mixture Properties .............................................................................................................................. 126
5.9.4 Solving Continuity Equation ............................................................................................................ 127
5.9.5 Momentum Equation .......................................................................................................................... 127
5.9.6 Energy Equation ................................................................................................................................... 127
5.9.7 Boundary Conditions .......................................................................................................................... 127
5.9.8 Numerical Results ................................................................................................................................ 127
5.9.9 Conclusion............................................................................................................................................... 128
5.10 Case Study 10 - A Study of the Impact of Mesh Configuration on 3D Fluidized Bed
Simulations ..................................................................................................................................................................... 129
5.10.1 Introduction ........................................................................................................................................... 129
5.10.2 Hydrodynamic Modeling and Governing Equations ............................................................. 131
5.10.3 Closure Modeling ................................................................................................................................. 132
5.10.3.1 Drag Model ....................................................................................................................................... 132
5.10.4 Experimental Setup ............................................................................................................................. 133
5.10.5 Numerical Setup ................................................................................................................................... 133
5.10.5.1 Simulation Parameters ................................................................................................................ 133
5.10.6 Boundary and Initial Conditions.................................................................................................... 134
5.10.6.1 Fluid Volume Fraction ................................................................................................................. 134
5.10.6.2 Solid Volume Fraction .................................................................................................................. 134
5.10.6.3 Pressure ............................................................................................................................................. 134
5.10.6.4 Temperature .................................................................................................................................... 134
5.10.6.5 Granular Temperature ................................................................................................................ 134
5.10.6.6 Fluid Velocity ................................................................................................................................... 134
5.10.6.7 Solid Velocity ................................................................................................................................... 134
5.10.7 Domain Discretization ....................................................................................................................... 134
5.10.8 Approach ................................................................................................................................................. 135
5.10.9 Result ........................................................................................................................................................ 136
5.10.9.1 Fluidized Bed Behavior ............................................................................................................... 136
5.10.10 Mesh Sensitivity Studies ................................................................................................................... 139
5.10.10.1 Curved Cartesian...................................................................................................................... 139
5.10.10.2 Cut cell .......................................................................................................................................... 139
5.10.10.3 Cylindrical ................................................................................................................................... 139
5.10.10.4 Hybrid........................................................................................................................................... 139
5.10.11 Mesh Geometry Efficiency ................................................................................................................ 140
5.10.12 Conclusion............................................................................................................................................... 141
5.11 Case Study 11 - Cavitation Characteristics Around a Sphere: An LES Investigation ............ 143
5.11.1 Introduction ........................................................................................................................................... 143
5.11.2 Literature Survey ................................................................................................................................. 144
5.11.3 Numerical Method ............................................................................................................................... 146
5.11.3.1 Governing Equations .................................................................................................................... 146
5.11.3.2 Volume of Fluid Model ................................................................................................................. 146
5.11.3.3 Large Eddy Simulation ................................................................................................................ 147
5.11.3.4 K- ω SST Turbulence Model ...................................................................................................... 148
5.11.3.5 Mass Transfer Modeling.............................................................................................................. 148
5.11.4 Numerical Setup ................................................................................................................................... 149
5.11.4.1 The interPhaseChangeFoam Validation for Cavitation ................................................... 149
5.11.4.2 Discretization and Code Validation ........................................................................................ 150
5.11.4.3 Pressure-Velocity Coupling: PIMPLE Algorithm............................................................... 150
5.11.4.4 The Sphere Problem ..................................................................................................................... 152
5.11.4.5 Grid Sensitivity Analysis ............................................................................................................. 153
5.11.4.6 Comparison with the Experiments ......................................................................................... 154
5.11.4.7 Cavitation Regimes ....................................................................................................................... 155
5.11.4.8 Turbulent Kinetic Energy in the Cavity ................................................................................ 156
5.11.4.9 Cavity Leading Edge ..................................................................................................................... 159
5.11.4.10 Re-Entrant Jet Analysis ......................................................................................................... 160
5.11.4.11 LES vs. k- ω SST Approach ................................................................................................... 161
5.11.4.12 Vorticity and Velocity Fields ............................................................................................... 161
5.11.4.13 Features of the Cavitating Flow ......................................................................................... 162
5.11.5 Conclusions ............................................................................................................................................ 163
List of Tables
Table 2.4.1 Single and Multi-Phase Flow vs. Single and Multi-Component .............................................. 17
Table 2.7.1 Modeling Available for Multi-Phase Flows...................................................................................... 22
Table 2.7.2 Choosing Guide According to Ansys Fluent .................................................................................... 23
Table 2.7.3 Parameters Considered Within Multiphase Flow Models ........................................................ 24
Table 2.7.4 Fluid Phases Physical Properties ........................................................................................................ 28
Table 2.7.5 Different Boundary Types of The Domain ...................................................................................... 35
Table 2.7.6 Difference of Lift And Drag Coefficients Between Different Grids ........................................ 36
Table 2.7.7 Lift And Drag Coefficients For Different Submergence Depths of Cambered Hydrofoil
NACA 4412 ............................................................................................................................................................................... 38
Table 2.7.8 The main parameters of the submarine and propeller models. ............................................ 41
Table 2.7.9 The results of mesh dependence validation. .................................................................................. 44
Table 2.7.10 The results of mesh dependence validation. ............................................................................... 45
Table 2.8.1 Geometries and Operating Conditions .............................................................................................. 56
Table 2.8.2 Results of Cases A, B, C And D Using Eulerian Model And VOF Model ................................. 59
Table 5.3.1 Comparison of Numerical Velocity (Riemann Sum vs. Finite Difference) ......................... 96
Table 5.7.1 Slug length at different air-water velocities ................................................................................ 116
Table 5.9.1 Boundary Conditions – Courtesy of [I.M. Abed] ........................................................................ 127
Table 5.10.1 Simulation Parameters & Closure Model Summary .............................................................. 133
Table 5.10.2 Computational Performance Candidates ................................................................................... 140
Table 5.10.3 Computational Performance ........................................................................................................... 141
Table 5.11.1 Summary of Discretization Schemes used ................................................................................. 150
Table 5.11.2 Grid sensitivity study on the cavity length and diameter (σ = 0.5) ................................. 155
List of Figures
Figure 1.1.1 Example of Multi-Phase Flow ............................................................................................................. 10
Figure 1.1.2 Carbon Dioxide (CO2) Pressure-Temperature Phase Diagram Showing the Triple
Point and Critical Point of CO2......................................................................................................................................... 12
Figure 1.2.1 Multi-gas separated by a wall ............................................................................................................. 13
Figure 1.3.1 Theories and Methods for Different Temporal and Spatial Scales ...................................... 14
Figure 2.1.1 Description of Multiphase Flow ......................................................................................................... 15
Figure 2.2.1 Coupling in multiphase flows ............................................................................................................. 16
Figure 2.4.1 Shock Wave in a Gaseous Medium (Courtesy of MacPhee et al.) ......................................... 17
Figure 2.5.1 Schematic guide for the selection of Multiphase Models ........................................................ 18
Figure 2.6.1 Average Volume V and Three phases α, β, γ ................................................................................. 19
Figure 2.7.1 Multi-Fluid in 2-Phase Flow and Transport Analysis Between Them ............................... 22
Figure 2.7.2 Transient Simulation of a Dam Break (Courtesy of Bakker) ................................................. 26
Figure 2.7.3 Schematic Representation of Pipe Flow and cross-sectional Mesh ................................... 28
Figure 2.7.4 Oil Volume Fraction Contours At Pipe Length (Z = 0.5 M) of Different Size Mesh ....... 29
Figure 2.7.5 Stratified Oil-Water Flow Simulation .............................................................................................. 30
Figure 2.7.6 Grid Independency Check According To Wave Height ............................................................. 36
Figure 2.7.7 Grid Independence Study of Airfoil Forces ................................................................................... 37
Figure 2.7.8 Comparison of Wave Elevations For NACA 4412 Hydrofoil At Various H/C Ratios .... 37
Figure 2.7.9 (A) Contour of Velocity Magnitude Around The Hydrofoil At H/C=1 ; (B) Velocity
Vectors Around The Hydrofoil At H/C=1 .................................................................................................................... 38
Figure 2.7.10 Contour of Static Pressure Near NACA 4412 Hydrofoil And Free Surface At H/C = 1
....................................................................................................................................................................................................... 38
Figure 2.7.11 The submarine and propeller model ............................................................................................ 42
Figure 2.7.12 The computational domain ............................................................................................................... 42
Figure 2.7.13 The process of PI controller simulation ....................................................................................... 44
Figure 2.7.14 The details of the mesh in the midship section ........................................................................ 45
Figure 2.7.15 The waves on the free surface in different cases ..................................................................... 46
Figure 2.7.16 The velocity nephograms at the midship section in different cases ................................ 47
Figure 2.7.17 The vortex structures in different cases ...................................................................................... 48
Figure 2.8.1 Mixing of Brine(Salt Water) with Fresh Water ........................................................................... 51
Figure 2.8.2 Flow patterns in vertical pipes. a) Bubbly & mist flow. b) Slug flow. c) Churn flow. d)
Annular flow. Source: (Bratland, 2010). ...................................................................................................................... 53
Figure 2.8.3 Experimental conditions plotted on Hewitt et al. (1986) flow pattern map .................. 54
Figure 2.8.4 Orthogonal (Butterfly) Mesh ............................................................................................................... 56
Figure 2.8.5 Mesh Independence Test – Experimental And CFD Results ................................................... 57
Figure 2.8.6 Mesh Independence Test – Simulation Time................................................................................ 58
Figure 2.8.7 VOF Model And Eulerian Model Predictions For Cases A, B, C And D ................................ 60
Figure 2.8.8 Void Fraction For The Cases Studies By VOF Model And Eulerian Model (1.74 M Of
Pipe) ............................................................................................................................................................................................ 60
Figure 3.1.1 Binary System of Gases .......................................................................................................................... 68
Figure 3.1.2 Volumetric Flux ........................................................................................................................................ 68
Figure 3.1.1 Divergence Theorem Applied to Chemical Species (Same Source) .................................... 70
Figure 3.2.2 Volume Swept ............................................................................................................................................ 70
Figure 3.5.1 Schematic of the case geometry and boundary conditions .................................................... 76
Figure 3.5.2 Instantaneous fields of axial and transverse velocities, density and pressure for the
DNS case (from top to bottom and from left to right), at 1.25 ms. .................................................................... 78
Figure 3.5.3 Instantaneous fields of hydrogen mass fractions, temperature and scatter plot of
temperature versus mass-fraction of hydrogen, at 1.25 ms ................................................................................ 78
Figure 3.5.4 Transverse cuts of Mean (Top) and RMS (Bottom) axial, transverse velocity,
pressure, density, temperature and oxygen mass fraction .................................................................................. 79
Figure 3.5.5 Influence of SGS modeling on the Reynolds stresses ................................................................ 80
Figure 3.5.6 Instantaneous fields of molecular (DNS and LES), turbulent and effective viscosity
(from left to right and from top to bottom) ................................................................................................................ 81
Figure 4.1.1 Illustration of the multi-physics hierarchy ................................................................................... 85
Figure 4.2.1 Modeling Scales in Fluid-Particle Systems .................................................................................... 88
Figure 5.2.1 Contour plots for particle volume fraction.................................................................................... 91
Figure 5.2.2 Sketch of the problem ............................................................................................................................ 91
Figure 5.3.1 Schematic diagram of the problem .................................................................................................. 94
Figure 5.4.1 Sketch of the reservoir with the four injection wells at the corners and the
production well in the center ........................................................................................................................................... 98
Figure 5.4.2 Cumulative flow in the production well for a production day .............................................. 99
Figure 5.5.1 Contour of gas volume fraction at different time levels ....................................................... 103
Figure 5.6.1 Schematic illustration of the flow geometry .............................................................................. 105
Figure 5.6.2 Turbulent statistics: time- and stream wise-averaged velocity field .............................. 108
Figure 5.6.3 Snapshots of the Air-Water Interface at Different Times (same source) ...................... 108
Figure 5.6.4 Turbulent Statistics for Two-Phase Couette Flow .................................................................. 109
Figure 5.6.5 Air-Water Interface at Fully Developed State ........................................................................... 110
Figure 5.7.1 Hydrodynamic slug formation (Courtesy of Z. I. Al-Hashimy et al.) ................................. 111
Figure 5.7.2 Baker chart where (.) Operating conditions of water–air two-phase flow .................. 112
Figure 5.7.3 Boundary condition for water-air slug flow through a pipe ............................................... 113
Figure 5.7.4 Slug initiation of the air-water slug flow ..................................................................................... 115
Figure 5.7.5 Slug length calculation of air-water slug flow ........................................................................... 116
Figure 5.7.6 Cross section of the fluid domain for the extraction of volume fraction for Case 3 .. 117
Figure 5.8.1 Distribution of the Gaseous Phase in a Computational ......................................................... 120
Figure 5.8.2 Number of Bubbles Depending on ................................................................................................. 121
Figure 5.8.3 Geometry and Boundary Conditions for Simulation of Cavitation Flows* ................... 123
Figure 5.8.4 One Cycle of the Periodic Unsteady Cavitation Flow over a NACA- 0015 Hydrofoil.
Vapor Fraction Distribution and Velocity Vectors ................................................................................................ 124
Figure 5.9.1 Distributions at 35 C – Courtesy of [I.M. Abed] ....................................................................... 128
Figure 5.10.1 Different Meshing Topologies ....................................................................................................... 135
Figure 5.10.2 Instantaneous Void Fraction ......................................................................................................... 136
Figure 5.10.3 Three-Dimensional Iso-Surfaces of Void Fraction (αg= 0.7) ............................................ 137
Figure 5.10.4 Time-Averaged Void Fraction ....................................................................................................... 138
Figure 5.10.5 Curved Cartesian Grid Resolution ............................................................................................... 139
Figure 5.10.6 Void Fractions for Mesh Efficiency (Sensitivity) Study ...................................................... 140
Figure 5.10.7 Axial Time-Averaged Void Fraction ............................................................................................. 141
Figure 5.11.1 Cp Distribution Over the Hemisphere Head-Form Body at σ = 0.2 ............................... 149
Figure 5.11.2 The Power spectrum density (PSD) analysis for the drag coefficient over the sphere
for cavitating at σ = 0.5 and non-cavitating flow. .................................................................................................. 151
Figure 5.11.3 Flowchart of the PIMPLE solution procedure ........................................................................ 152
Figure 5.11.4 Computational domain and boundary conditions ................................................................ 153
Figure 5.11.5 The structured meshes around the sphere ............................................................................. 153
Figure 5.11.6 3D views of cavity cloud (iso surface of the vapor volume fraction) over the sphere
at various cavitation numbers: experimental results taken by the low-speed photographer, Re = 1.5
×10 6 ( Brandner et al., 2010 ) (right frames), numerical result- LES/Sauer models (left frames),
numerical result- LES/Sauer models for super cavitating flow (two last frames). ................................. 154
Figure 5.11.7 The depiction of three different modes of cavitation around the sphere from the
inception cavitation to super cavitation, left: numerical data, right: experimental images ( Brandner
et al., 2010 ). .......................................................................................................................................................................... 156
Figure 5.11.8 Nine consecutive frames of temporal variation of the cavity cloud .............................. 157
5.11.9 Time evolution of cavitation patterns obtained from the simulation, left: 3D contours of
vapor volume fraction, right: in plane cavity boundary (solid line) and flood contours of turbulence
kinetic energy (TKE), LES, Sauer, σ = 0.1. ................................................................................................................. 158
Figure 5.11.10 (a , b) separation point for cavitating (Left frame) and non-cavitating flows (right
frame) ...................................................................................................................................................................................... 159
Figure 5.11.11 Formation of the re-entrant jet (red lines) at different cavitation numbers. (For
interpretation of the references to color in this figure legend, the reader is referred to the web
version of this article.) ...................................................................................................................................................... 159
Figure 5.11.12 Comparison of different turbulence models (LES/ k- ω SST): Instantaneous volume
fraction contours ................................................................................................................................................................ 160
Figure 5.11.13 Comparisons of the velocity streamlines of cavitating flow with the non-cavitating
flow conditions .................................................................................................................................................................... 161
Figure 5.11.14 Comparisons of mean pressure coefficient over a broad range of cavitation
number .................................................................................................................................................................................... 162
Figure 5.11.15 Distribution of the mean values of water volume fraction at various cavitation
numbers.................................................................................................................................................................................. 162
1 Introduction
1.1 Multiphase Flow
The term Multi-phase flow is used to refer to any fluid flow consisting of more than one phase or
component. For brevity and because they are covered in other texts, we exclude those circumstances
in which the components are well mixed above the molecular level. Consequently, the flows
considered here have some level of phase or component separation at a scale well above the
molecular level. This still leaves an enormous spectrum of different multiphase flows. One could
classify them according to the state of the different phases or components and therefore refer to
gas/solids flows, or liquid/solids flows or gas/particle flows or bubbly flows and so on. Many texts
exist that limit their attention in this way
1
. Consequently, the flows considered here have some level
of phase separation at a scale well above the molecular level. Some treatises are defined in terms of
a specific type of fluid flow and deal with low Reynolds number suspension flows, dusty gas dynamics
and so on. Others focus attention on a specific application such as slurry flows, cavitation flows,
aerosols, debris flows, fluidized beds
and etc. Again there are many such
texts and here, we attempt to identify
the basic fluid mechanical phenomena
and to illustrate those phenomena
with examples from a broad range of
applications and types of flow (see
Figure 1.1.1).
Virtually every processing technology
must deal with multiphase flow, from
activating pumps and turbines to
electro photographic processes.
Clearly the ability to predict the fluid
flow behavior of these processes is
central to the efficiency and
effectiveness of those processes. For
example, the effective flow of toner is a
major factor in the quality and speed of electro-photographic printers. Multi-Phase flows are also a
pervasive feature of our environment whether one considers rain, snow, fog, avalanches, mud slides,
sediment transport, debris flows, and countless other natural phenomena. Very critical biological and
medical flows are also multiphase, from blood flow to the bends to lithotripsy to laser surgery
cavitation and so on. No single list can adequately illustrate the diversity; consequently any attempt
at a comprehensive treatment of multiphase flows is flawed unless it focuses on common
phenomenological themes and avoids the temptation to deviate into lists of observations. Be aware
that there are situations in which the Multi-Phase homogeneous and Multi-Component cases are
overlap and hard to distinguished. The difference is the Multi-Component model assumes they mix
into a single phase, which can be represented by a bulk density, viscosity etc. and the components
are mixed on a microscopic scale. On the other hand, Multi-Phase homogeneous means you have
multiple phases (e.g., gas and liquid) and they are separated on a resolvable scale. Some
commercial software (i.e., Ansys CFX®) simulating it as multiphase homogenous flow it solves for
volume fractions, after that calculates density (mean density?) and then solves momentum equations.
If it is multicomponent than it solves for mass fractions, after that calculates mean density and
momentum and so on in the end.
1
Christopher E. Brennen, “Fundamentals of Multiphase Flows”, Cambridge University Press 2005.
Figure 1.1.1 Example of Multi-Phase Flow
Two general topologies of multiphase flow can be usefully identified at the outset, namely Disperse
flows and Separated flows. By disperse flows we mean those consisting of finite particles, drops or
bubbles (the disperse phase) distributed in a connected volume of the continuous phase. On the other
hand separated flows consist of two or more continuous streams of different fluids separated by
interfaces. In multiphase flows, solid phases are denoted by the subscript S, liquid phases by the
subscript L and gas phases by the subscript G. Some of the main characteristics of these three types
of phases are as follows:
1.1.1 Solids Phase
In a multiphase flow, the solid phase is in the form of lumps or particles which are carried along in
the flow. The characteristics of the movement of the solid are strongly dependent on the size of the
individual elements and on the motions of the associated fluids. Very small particles follow the fluid
motions, whereas larger particles are less responsive.
1.1.2 Liquids Phase
In a multiphase flow containing a liquid phase, the liquid can be the continuous phase containing
dispersed elements of solids (particles), gases (bubbles) or other liquids (drops). The liquid phase
can also be discontinuous, as in the form of drops suspended in a gas phase or in another liquid phase.
Another important property of liquid phases relates to wettability. When a liquid phase is in contact
with a solid phase (such as a channel wall) and is adjacent to another phase which is also in contact
with the wall, there exists at the wall a triple interface, and the angle subtended at this interface by
the liquid-gas and liquid-solid interface is known as the Contact Angle.
1.1.3 Gases Phase
As a fluid, a gas has the same properties as a liquid in its response to forces. However, it has the
important additional property of being (in comparison to liquids and solids) highly compressible.
Notwithstanding this property, many multiphase flows containing gases can be treated as essentially
incompressible, particularly if the pressure is reasonably high and the Mach Number, with respect to
the gas phase, is low (e.g., < 0.2).
1.1.4 Phase Rule
Gibbs's phase rule
2
was proposed by Josiah Willard Gibbs in his landmark paper titled On the
Equilibrium of Heterogeneous Substances. The rule applies to non-reactive multi-component
heterogeneous systems in thermodynamic equilibrium and is given by the equality
phases ofnumber P
components ofnumber C
freedom of degrees ofnumber F where
2PCF
→
→
→
+−=
Eq. 1.1.1
The number of degrees of freedom is the number of independent intensive variables, i.e. the largest
number of thermodynamic parameters such as temperature or pressure that can be varied
simultaneously and arbitrarily without affecting one another. An example of one-component system
is a system involving one pure chemical, while two-component systems, such as mixtures of water
and ethanol, have two chemically independent components, and so on.
2
Gibbs, J. W., Scientific Papers (Dover, New York, 1961).
1.1.4.1 Pure Substances (one component)
For pure substances C = 1 so that F = 3 − P. In a single phase (P = 1) condition of a pure component
system, two variables (F = 2), such as temperature and pressure, can be chosen independently to be
any pair of values consistent with the
phase. However, if the temperature and
pressure combination ranges to a point
where the pure component undergoes a
separation into two phases (P = 2), F
decreases from 2 to 1. When the system
enters the two-phase region, it becomes
no longer possible to independently
control temperature and pressure.
If the pressure is increased by
compression, (see Figure 1.1.2) some of
the gas condenses and the temperature
goes up for CO2. If the temperature is
decreased by cooling, some of the gas
condenses, decreasing the pressure.
Throughout both processes, the
temperature and pressure stay in the
relationship shown by this boundary
curve unless one phase is entirely
consumed by evaporation or
condensation, or unless the critical point
is reached. As long as there are two
phases, there is only one degree of freedom, which corresponds to the position along the phase
boundary curve.
The critical point is the black dot at the end of the liquid–gas boundary. As this point is approached,
the liquid and gas phases become progressively more similar until, at the critical point, there is no
longer a separation into two phases. Above the critical point and away from the phase boundary
curve, F = 2 and the temperature and pressure can be controlled independently. Hence there is only
one phase, and it has the physical properties of a dense gas, but is also referred to as a supercritical
fluid. Of the other two-boundary curves, one is the solid–liquid boundary or melting point curve
which indicates the conditions for equilibrium between these two phases, and the other at lower
temperature and pressure is the solid–gas boundary. Even for a pure substance, it is possible that
three phases, such as solid, liquid and vapor, can exist together in equilibrium (P = 3). If there is only
one component, there are no degrees of freedom (F = 0) when there are three phases. Therefore, in
a single-component system, this three-phase mixture can only exist at a single temperature and
pressure, which is known as a triple point. In the diagram for CO2 (see Figure 1.1.2), the triple point
is the point at which the solid, liquid and gas phases come together, at 5.2 bar and 217 K. It is also
possible for other sets of phases to form a triple point, for example in the water system there is a
triple point where ice I, ice III and liquid can coexist
3
.
1.2 Multicomponent Flow
The multi-component or Multi-species model assumes they mix into a single phase, which can be
represented by a bulk density, viscosity etc. The components are mixed on a microscopic scale. The
multi-component flow (species transport) refers to flow that the components are mixed at molecular
3
From Wikipedia, the free encyclopedia.
Figure 1.1.2 Carbon Dioxide (CO2) Pressure-
Temperature Phase Diagram Showing the Triple Point
and Critical Point of CO2
level and can be characterized
by a single velocity and
temperature field for all
species
4
. A simple example of
such a multicomponent system
is a binary (two component)
solution consisting of a solute in
an excess of chemically different
solvent. (
Figure 1.2.1).
1.2.1 Multiphase vs
Multicomponent
According to (Amir Faghri & Yuwen Zhang, in Transport Phenomena in Multiphase Systems,
2006), a multiphase system is one characterized by the simultaneous presence of several phases,
the two-phase system being the simplest case. The term ‘two-component’ is sometimes used to
describe flows in which the phases consist of different chemical substances. For example, steam-
water flows are two-phase, while air-water flows are two-component. Some two-component flows
(mostly liquid-liquid) technically consist of a single phase but are identified as two-phase flows in
which the term “phase” is applied to each of the components. Since the same mathematics
describes two-phase and two-component flows, the two expressions will be treated as
synonymous. Here, we deal with a variety of multiphase systems, in which the phases passing
through the system may be solid, liquid or gas, or a combination of these three.
1.3 Multiscale Flow
Multiscale modeling refers to a style of modeling in which multiple models at different scales are used
simultaneously to describe a system. The different models usually focus on different scales of
resolution. They sometimes originate from physical laws of different nature, for example, one from
continuum mechanics and one from molecular dynamics. In this case, one speaks of multi-physics
modeling even though the terminology might not be fully accurate. The need for multiscale modeling
comes usually from the fact that the available macroscale models are not accurate enough, and the
microscale models are not efficient enough and/or offer too much information. By combining both
viewpoints, one hopes to arrive at a reasonable compromise between accuracy and efficiency. The
subject of multiscale modeling consists of three closely related components: multiscale analysis,
multiscale models and multiscale algorithms. Multiscale analysis tools allow us to understand the
relation between models at different scales of resolutions. Multiscale models allow us to formulate
models that couple together models at different scales. Multiscale algorithms allow us to use
multiscale ideas to design computational algorithms. Figure 1.3.1 summarizes theories and typical
numerical methods for different temporal and spatial scales. When the continuum assumption breaks
down, the fluid has to be described by atomistic point of view, such as the molecular dynamics as a
microscopic method or statistical rules for molecular groups, i.e. kinetic theories, as the mesoscopic
methods for a larger scale. If the characteristic length is smaller than 1 nm (1 Nano-meter is 1×10−9 m)
or the characteristic time is shorter than 1 fs (1 femtosecond is equal to 10−15 seconds), the quantum
effect may be not negligible for the concerned system and the quantum mechanics has to be brought
in to describe the transport as a result. In fact modeling from a smaller scale may lead to a more
4
Associate Professor Britt M. Halvorsen Amaranath S. Kumara, ”Computational Fluid Dynamics (CFD) and
Multiphase Flow Modelling”, Telemark University College, Porsgrunn, Norway.
Figure 1.2.1 Multi-gas separated by a wall
accurate description of the problem, but will bring much more computational cost as well. Therefore
we may have to find an appropriate tradeoff for our concerned fluid behaviors in engineering
5
.
5
Shiyi Chen, Moran Wang, Zhenhua Xia, “Multiscale fluid mechanics and modeling”, Procedia IUTAM 10 ( 2014).
Figure 1.3.1 Theories and Methods for Different Temporal and Spatial Scales
2 Multiphase Flows
2.1 Preliminaries
Up to this point we were dealing with single phase flows. To get matters complicated, we now
concern ourselves with multi-phase flows which exist in many industrial applications such as Oil &
Gas, Power Generation, Biomedical, Automotive, Chemical Processing and Aerospace among others.
Multiphase flows refer to flows of several fluids in the domain of interest. In general, we associate
fluid phases with gases, liquids or solids and as such some simple examples of multi-phase flows are:
air bubbles rising in a glass of water, sand particles carried by wind, rain drops in air. In fact, the
definition of ‘phase’ can be generalized and applied to other fluid characteristics such as size and
shape, density, temperature, etc. With this broader definition, multiple phases can be used to
represent the entire size distribution of particles in several size groups or ‘phases’ of a multi-phase
model.
In fluid mechanics, multiphase flow is simultaneous flow of (a) materials with different states
or phases (i.e. gas, liquid or solid), or (b) materials with different chemical properties but in the
same state or phase (i.e. liquid-liquid systems such as oil droplets in water). Generally, a
multiphase fluid is composed of two or more distinct phases which themselves may be fluids, gases
or solids, and has the characteristic properties of a fluid. Within the discipline of multi-phase flow
dynamics the present status is quite different from that of the single phase flows. The theoretical
background of the single phase flows is well
established and apparently the only outstanding
practical problem that still remains unsolved is
turbulence, or perhaps more generally, problems
associated with flow stability. Generally, a phase is a
class of matter, with a definable boundary and a
particular dynamic response to the surrounding
flow and potential field. Phases are generally
identified by solid, liquid or gaseous states of matter
but can also refer to other forms: Materials with
different chemical properties but in the same state
or phase (i.e. liquid-liquid, such as, oil-water). The
fluid system is defined by a primary and multiple
secondary phases (See Figure 2.1.1). There may be
several secondary phase denoting particles with
different sizes.
2.2 Equations of Multiphase Flow
While it is rather straightforward to derive the equations of the conservation of mass, momentum
and energy for an arbitrary mixture, no general counterpart of the Navier-Stokes equation for
multiphase flows have been found. Using a proper averaging procedure it is however quite possible
to derive a set of Equations of Multiphase Flow which in principle correctly describes the dynamics
of any multiphase system and is subject only to very general assumptions
6
. A direct consequence of
the complexity and diversity of these flows is that the discipline of multiphase fluid dynamics is and
may long remain a prominently experimental branch of fluid mechanics. Preliminary small scale
model testing followed by a trial and error stage with the full scale system is still the only conceivable
solution for many practical engineering problems involving multiphase flows. Inferring the necessary
constitutive relations from measured data and verifying the final results are of vital importance also
6
Multiphase flow Dynamics, Theory and Numeric.
Figure 2.1.1 Description of Multiphase Flow
within those approaches for which theoretical modeling and subsequent numerical solution is
considered feasible.
2.3 Multiphase Coupling
Phase coupling, in terms of momentum, energy,
and mass, is a basic concept in the description of
any multiphase flow. The coupling can occur
through exchange of momentum, energy, and
mass among phases as shown in Figure 2.2.1.
In principle, fluid‐particulate properties can be
described by position, velocity, size,
temperature, and species concentration of fluid
and/or particle. While the phenomenological
description of multiphase flow can be applied to
classify flow characteristics, it also can be used to
determine appropriate numerical formulations.
In various modes of coupling, depending on the
contribution of phases and phenomena, different
coupling schemes can be adapted. This may allow
independent treatment of phases or
simultaneous integration of momentum, heat,
and mass exchanges between phases. In general,
modeling complexity increases as more effects
associated with time and length scales are
included in the simulation. In general, coupling
depends on particle size, relative velocity,
volume fraction. Three ways that coupling could
be presents as shown in Figure 2.2.1:
1. One-way coupling: Sufficiently dilute
such that fluid feels no effect from
presence of particles. Particles move in dynamic response to fluid motion.
2. Two-way coupling: Enough particles are present such that momentum exchange between
dispersed and carrier phase interfaces alters dynamics of the carrier phase.
3. Four-way coupling: Flow is dense enough that dispersed phase collisions are significant
momentum exchange mechanism
7
.
2.4 Examples of Multiphase Flow
While the modeling and numerical simulation of multiphase and multicomponent flows poses far
greater challenges than that of single-phase and single-component flows, their accessibility in nature
is numerous. Rain and snow, and a vaporing tea pot is among prime example of multiphase flow.
Others include, Spray drying, Pollution control, Pneumatic transport, Slurry transport, Fluidized
beds, Spray forming, Plasma spray coating, Abrasive water jet cutting, Pulverized coal fired furnaces,
Solid propellant rockets, Fire suppression and controls
8
. These challenges are due to interfaces
between phases and large or discontinuous property variations across interfaces between phases
and/or components. High-pressure and supersonic multiphase and multicomponent jet flow is one
7
Ken Kiger, “Multiphase Turbulent Flow”, UMCP presentation.
8
Grétar Tryggvason, “Multiphase Flow Modeling”, spring 2010.
Figure 2.2.1 Coupling in multiphase flows
One Way
Two Way
Four Way
of the most challenging problems in
multiphase flow due to the
complexity of the dynamics of the jet.
For example, the presence of
cavitation and gas entrapment inside
the nozzle orifice can greatly affect
the development and formation of
the external jet. Another case
involves high-pressure fuel spray has
never been recognized as supersonic
under typical fuel injection
conditions
9
-
10
.
Recently, [MacPhee et al]
11
have used
a synchrotron x-radiography and a
fast x-ray detector to record the time
evolution of the transient fuel sprays
from a high-pressure injector. In
their experiment, the propagation of the spray-induced shock waves in a gaseous medium were
captured and the complex nature of the spray hydrodynamics were revealed. They have found out
that under injection conditions similar to those in operating engines, the fuel jets can exceed
supersonic speeds and result an oblique shock wave in the gaseous medium
12
, see Figure 2.4.1.
However, the effect of this shock wave to the atomization of the fuel and the combustion processes is
currently not known. There are four distinctive new attitude which cover the following flow
regimes
13
in Table 2.4.1. Another example would be dynamic adaptive mesh optimization for
complex multi-phase free-bubbling flow modelling in 3D (see following short video).
https://media-exp1.licdn.com/dms/image/C4D22AQGfhzYoBZwWag/feedshare-shrink_1280-
alternative/0?e=1600905600&v=beta&t=-kZtXIj7_CsN_qsMekpKmsFLferVBydTZllvnlvutvc
9
T. Nakahira, M. Komori, K. Nishida, and K. Tsujimura. Shock W aves, K. Takayama, Ed., 2:1271–1276, 1992
10
H.H. Shi, K. Takayama, and O Onodera. JSME Intl. J. Ser. B, 37:509, 1994.
11
A.G. MacPhee, M.W. Tate, C.F. Powell, Y. Yue, M.J. Renzi, A. Ercan, S. Narayanan, E. Fontes, J. Walther, J. Schaller,
S.M. Gruner, and J. Wang, ”X-ray imaging of shock waves generated by high pressure fuel spray”, Science,
295:1261–1263, 2002.
12
Shock Wave in a Gaseous Medium due to a high pressure and supersonic jet flow. The image of shock wave
is captured using synchrotron x-radiography.
13
Randy S. Lagumbay, “Modeling and Simulation of Multiphase/Multicomponent Flows”, A thesis submitted to
the Faculty of the Graduate School of the University of Colorado in partial fulfillment of the requirements for
the degree of Doctor of Philosophy Department of Mechanical Engineering -2006.
Figure 2.4.1 Shock Wave in a Gaseous Medium (Courtesy of
MacPhee et al.)
Single - Component
Multi - Component
Single - Phase
Water flow
Pure Nitrogen flow
Air flow
H20 + Oil blends
Multi - Phase
Steam bubble in H20
Freon-Freon
Vapor flow
Ice Slurry flow
Coal particles in air
Sand particle in H20
Table 2.4.1 Single and Multi-Phase Flow vs. Single and Multi-Component
It is using an integrated modelling framework with force-balancing and interface capturing for initial
generation of Taylor bubbles injecting air into a vertical glycerol-filled pipe [A. Obeysekara]
14
.
2.5 Guidelines for Selecting a Multiphase Model
In selecting the best multiphase model, the first step is to identify the porous domains and attribute
appropriate flow models to each area. The second step is to characterize the flow as segregated or
dispersed. Other parameters that are important in selecting the best model are the particle loading
and the Stokes number. The particle
loading will give an estimate for the
number of particles and the probability
of particle–particle collisions. The
Stokes number predicts how
independently the dispersed phase
behaves relative to the continuous
phase. The scheme in Figure 2.5.1
gives an elementary view of the choices.
However, the choices are not clear-cut
insofar as there might be other reasons
for selection of models. Very often it is
the stability of the solution and
available data that decide the
selection
15
.
2.6 Volume Averaging
Formulation
In this section we shall derive the
’equations of multiphase flow’ using
the volume averaging method. To this
end, we first define appropriate volume
averaged dynamic flow quantities and
then derive the required flow equations
for those variables by averaging the
corresponding physical equations.
While ensemble averaging may appear
as the most elegant approach from the
theoretical point of view, volume
averaging provides perhaps the most
intuitive and straight forward
interpretation of the dynamic
quantities and interaction terms
involved. Volume averaging also
illustrates the potential problems and
intricacies that are common to all
averaging methods within Eulerian
14
Asiri Obeysekara, Scientist | Research software engineering | Computational physics | High performance
computing.
15
Bengt Andersson, Ronnie Andersson, Love Ha° Kansson, Mikael Mortensen, Rahman Sudiyo, and Berend Van
Wachem, “Computational Fluid Dynamics For Engineers”, Cambridge University Press, ISBN 978-1-107-01895-
2, 2012.
Figure 2.5.1 Schematic guide for the selection of
Multiphase Models
approach. Volume averaging is based on the assumption that a length scale Lc exists such that l < Lc
< L, where 1 is the ’macroscopic’ length scale of the system and L is a length scale that we shall call
mesoscopic in what follows Figure 2.5.1. The mesoscopic length scale is associated with the
distribution of the various phases within the mixture. (The ’microscopic’ length scale would then be
the molecular scale). To begin with, we consider a representative averaging volume V Lc3 contains
distinct domains of each phase such
that V = ∑α Vα where Vα is the volume occupied by phase α
within V. Similarly, for any quantity qα (scalar, vector or tensor) defined in phase α, we define the
following averages:
V
V
φ re whe
ρ
~
φ
qρ
dVρ
dVqρ
q
q
φ
1
dVq
V
1
q
~
, dVq
V
1
q
α
α
αα
αα
Vα
α
V
αα
α
α
α
V
α
α
α
V
αα
α
aa
===
===
Eq. 2.6.1
Volume fraction of phase and subjected to the constrained:
Figure 2.6.1 Average Volume V and Three phases α, β, γ
1φ
α
α=
Eq. 2.6.2
The averaged equations now acquire the form
αααδα
δαααααααααααααα
αααααα
δuδuρτ where
τ.g
~
ρ
~
φτ.)P
~
(φ)uuρ
~
.(φ)uρ
~
(φ
t
)uρ
~
.(φ)ρ
~
(φ
t
−=
++++−=+
=+
M
Γ
Eq. 2.6.3
This tensor is sometimes called a pseudo-turbulent stress tensor since it is analogous to the usual
Reynolds stress tensor of turbulent one phase flow. Notice however, that tensor < τδα > is defined
here as a volume average instead of a time average as the usual Reynolds stress. It also contains
momentum fluxes that arise both from the turbulent fluctuations of the mesoscopic flow and from
the fluctuations of the velocity of phase due to the presence of other phases. Consequently, it does
not necessarily vanish even if the mesoscopic flow is laminar. The so called transfer integrals, Ϻα, Гα
are defined as
α phase of vector normal outwardunit
ˆ
dA
ˆ
).(ρ
V
1
dA
ˆ
).(ρ
V
1
α
αAα
Aα
ααααAα
Aα
α
=
−=−=
n
nuuuMnuuΓα
Eq. 2.6.4
2.6.1 Constitutive Relations
Eq. 2.6.4 are, in principle, exact equations for the averaged quantities. So far, they do not contain
much information about the dynamics of the particular system to be described. That information
must be provided by a set of system dependent constitutive relations which specify the material
properties of each phase, the interactions between different phases and the (pseudo) turbulent
stresses of each phase in the presence of other phases. These relations finally render the set of
equations in a closed form where solution is feasible. At this point we do not attempt to elaborate in
detail the possible strategies for attaining the constitutive relations in specific cases, but simply state
the basic principles that should be followed in inferring such relations. The unknown terms that
appear in the averaged Eq. 2.6.3 such as the transfer integrals and stress terms that still contain
macroscopic quantities, should be replaced by new terms. Typically, constitutive relations are given
in a form where these new terms include free parameters which are supposed to be determined
experimentally. In some cases constitutive laws can readily be derived from the properties of the
mixture, or from the properties of the pure phase. For example, the incompressibility of the pure
phase α implies the constitutive relation ρα = constant. Similarly, the equation of state Pα = Cρα, where
C = constant for the pure phase, implies Pα = Cρα. In most cases, however, the constitutive relations
must be either extracted from experiments, derived analytically under suitable simplifying
assumptions, or postulated.
Including a given physical mechanism in the model by imposing proper constitutive relations is not
always straightforward even if adequate experimental and theoretical information is available. In
particular, making specific assumptions concerning one of the unknown quantities may induce the
constraints on other terms. For example, the transfer integrals Гα and Mα contain the effect of
exchange of mass and momentum between the phases. According to Eq. 2.6.3, the quantity Гα gives
the rate of mass transfer per unit volume through the phase boundary Aα into phase α from the other
phases. In a reactive mixture, where phase α is changed into phase, the mass transfer term Гα might
be given in terms of the experimental rate of the chemical reaction α → γ, correlated to the volume
fractions ϕα and ϕγ, and to the temperature of the mixture T. Similarly, the quantity Mα gives the rate
of momentum transfer per unit volume into phase α through the phase boundary Aα. The second
integral on the right side of Eq. 2.6.4 contains the transfer of momentum carried by the mass
exchanged between phases. It is obvious that this part of the momentum transfer integral Mα must
be consistently correlated with the mass transfer integral Гα. Similarly, the first integral on the right
side of Eq. 2.6.4 contains the change of momentum of phase α due to stresses imposed on the phase
boundary by the other phases. Physically, this term contains forces such as buoyancy which may be
correlated to average pressures and gradients of volume fractions, and viscous drag which might be
correlated to volume fractions and average velocity differences. For instance in a liquid-particle
suspension, the average stress inside solid particles depends on the hydrodynamic forces acting on
the surface of the particles.
The choice of e.g., drag force correlation between fluid and particles should therefore influence the
choice of the stress correlation for the particulate phase. While this particular problem can be solved
exactly for some idealized cases, there seems to be no general solution available. Perhaps the most
intricate term which phase boundary Aα. The second integral on the right side of Eq. 2.6.4 contains
the transfer of momentum carried by the mass exchanged between phases. It is obvious that this part
of the momentum transfer integral Mα must be consistently correlated with the mass transfer
integral Гα. Similarly, the first integral on the right side of Eq. 2.6.4 contains the change of
momentum of phase α due to stresses imposed on the phase boundary by the other phases.
Physically, this term contains forces such as buoyancy which may be correlated to average pressures
and gradients of volume fractions, and viscous drag which might be correlated to volume fractions
and average velocity differences.
For instance in a liquid-particle suspension, the average stress inside solid particles depends on the
hydrodynamic forces acting on the surface of the particles. The choice of, e.g., drag force correlation
between fluid and particles should therefore influence the choice of the stress correlation for the
particulate phase. While this particular problem can be solved exactly for some idealized cases, there
seems to be no general solution available. Perhaps the most intricate term this is to be correlated to
the averaged quantities through constitutive relations is the tensor < τδα > given by Eq. 2.6.3. It
contains the momentum transfer inside phase α which arises from the genuine turbulence of phase
α and from the velocity fluctuations due to presence of other phases, and which are present also in
the case that the flow is laminar in the mesoscopic scale. Moreover, the truly turbulent fluctuations
of phase α may be substantially modulated by the other phases. Bearing in mind the intricacies that
are encountered in modeling turbulence in single phase flows, it is evident that inferring realistic
constitutive relations for tensor < τδα > remains as a considerable challenge. It may, however, be
attempted, e.g., for fluid-particle suspensions by generalizing the corresponding models for single
phase flows, such as turbulence energy dissipation models, large-eddy simulations or direct
numerical simulations.
2.7 Modeling Approach Defined Based on Interface Physics
Genuine models for multiphase flows have been developed mainly following two different
approaches (see Figure 2.7.1). Within the Eulerian Approach all phases are treated formally as
fluids which obey normal one phase equations of motion in the unobservable ’mesoscopic’ level (e.g.,
in the size scale of suspended particles) with appropriate boundary conditions specified at phase
boundaries. The macroscopic flow equations are derived from these mesoscopic equations using an
averaging procedure of some kind.
This averaging procedure can be carried out in several alternative ways such as time averaging,
volume averaging and ensemble averaging. Various combinations of these basic methods can also
been considered. Irrespective of the method used, the averaging procedure leads to equations of the
same generic form, namely the form of the original physical equations with a few extra terms. These
extra terms include the interactions (change of mass, momentum etc.) at phase boundaries and
terms analogous to the ordinary Reynolds stresses in the turbulent single phase flow equations. Each
averaging procedure may however provide a slightly different view in the physical interpretation of
these additional terms and, consequently, may suggest different approach for solving the closure
problem that is invariably associated with the solution of these equations. The manner, in which the
various possible interaction mechanisms are naturally divided between these additional terms, may
also depend on the averaging procedure being used. The advantage of the Eulerian method is its
generality means that in principle it can be applied to any multiphase system, irrespective of the
number and nature of the phases. A drawback of the straightforward Eulerian approach is that it
often leads to a very complicated set of flow equations and closure relations.
In some cases, however, it is possible to use a simplified formulation of the full Eulerian approach,
namely Mixture Model (or Algebraic Slip Model). The mixture model may be applicable, e.g., for a
Figure 2.7.1 Multi-Fluid in 2-Phase Flow and Transport Analysis Between Them
Interface
Approaches
Model
Definitions
Flow
Regions
Eulerian
Volume of Fluid
Model (VOF)
Direct method of predicting interface
shape between immiscible phases
Stratified
Flow
Eulerian
Eulerian Model
Model resulting from averaging of VOF
model applicable to dispersed flows
Dispersed
Flow
Eulerian
Mixture Model
Simplification of Euler model;
applicable when inertia of dispersed
phase is small
Dispersed
Flow
Lagrangian
Dispersed Phase
Model (DPM)
Lagrangian particle/bubble/droplet
tracking
Dilute Flow
Table 2.7.1 Modeling Available for Multi-Phase Flows
relatively homogeneous suspension of one or more species of dispersed phase that closely follow the
motion of the continuous carrier fluid. For such a system the mixture model includes the continuity
equation and the momentum equations for the mixture, and the continuity equations for each
dispersed phase. The slip velocities between the continuous phase and the dispersed phases are
inferred from approximate algebraic balance equations. This reduces the computational effort
considerably, especially when several dispersed phases are considered.
Another common approach is the so called Lagrangian Method which is mainly restricted to
particulate suspensions. Within that approach only the fluid phase is treated as continuous while the
motion of the discontinuous particulate phase is obtained by integrating the equation of motion of
individual particles along their trajectories. Table 2.7.1 represents the different modeling
approaches.
2.7.1 Comparison of Computational Multiphase Flows
16
Out of three Euler-Euler models are implemented, VOF is recommended if enough resolution to track
interfaces is available [BSC et al.]
17
. It should be mentioned that VOF model may present problems
(inaccuracies or convergence issues) where large velocity, temperature or viscosity differences exist
between the phases. Mixture and Eulerian models are recommended for bubbly, droplet or particle-
laden flows in which volume fraction exceed 10%. Mixture model permits different velocities for
each phase while Eulerian model solves continuity, momentum and energy for each of the phases. As
a result, Eulerian model is more accurate and requires more computational effort than Mixture
model. The complexity of the Eulerian model can make it less computationally stable than the
mixture model. Finally Lagrange (discrete model) is also implemented when phases mix is below
10%. Consequently, it
can be inferred that VOF
model should be used
when enough resolution
to capture interfaces is
available, Mixture or
Eulerian model should be used if there is not enough resolution to capture interfaces but volume
fraction exceed 10% , otherwise, Lagrangian approach should be used if the volumetric phase mix is
below 10%. (see Table 2.7.2). More involved differences between the multiphase models, outlined
by Ansys©, summarized in Table 2.7.3. The VOF model is generally used for the cases where large
deforming interfaces are of interest. Both mixture and Eulerian-Eulerian (Multiphase VOF) models
are suitable where the interphase forces are of importance. Furthermore, the Eulerian-Eulerian
model is suitable when the lift forces are of importance in the flow. The Eulerian-Eulerian model is
good fit when the flow regime is unknown and the Mixture model in many cases can be a good
replacement for the full Eulerian-Eulerian model as it is computationally cheaper
18
.
Another point of view expressed by Cees Haringa is , “When you enable "multi-fluid VOF" under
the Eulerian model options, you basically get the same capabilities as regular VOF, but with 1
difference; in regular VOF, the momentum and temperature equations are shared between the
phases, whereas in multi-fluid VOF, there are separate equations for each phase”.
16
Ansys Fluent User Guide
17
BSC, UPV, and UPM, “Deliverable 1.1. Two-phase and phase change model approach review and requirements
coverage report”, Ref. Ares (2018)3995664 – 2018).
18
Nausheen Basha , Ahmed Kovacevic and Sham Rane, (2019), “Analysis of Oil-Injected Twin-Screw Compressor
with Multiphase Flow Models”, Licensee MDPI, Basel, Switzerland.
Model
VOF
Mixture /Euler
Lagrangian
Volume Fraction
α >> 0.1
α > 0.1
α < 0.1
Table 2.7.2 Choosing Guide According to Ansys Fluent
Table 2.7.3 Parameters Considered Within Multiphase Flow Models
2.7.2 Physics of Eulerian Multiphase Models
Eulerian Multiphase Model is a result of averaging of NS equations over the volume including
arbitrary particles + continuous phase. The result is a set of conservation equations for each phase
(continuous phase + N particle “media”). Both phases coexist simultaneously: conservation equations
for each phase contain single-phase terms (pressure gradient, thermal conduction etc.). Interfacial
terms express interfacial momentum (drag), heat and mass exchange. These are nonlinearly
proportional to degree of mechanical (velocity difference between phases), thermal (temperature
difference). Hence equations are harder to converge. Within the Eulerian-Eulerian Model, certain
inter phase transfer terms used in momentum, heat, and other interphase transfer models, can be
modeled using either the Particle Model, the Mixture Model or the Free Surface Model. In
particular, the calculation of the interfacial area density, used for all inhomogeneous transfer models
for a given fluid pair, is calculated according to one of these models. The available options depend on
the morphology of each phase of the pair (for example, continuous, dispersed, etc.), and as settings
in (homogeneous options, free surface model option).
In the Eulerian Multiphase Model, the phases are treated as interpenetrating continua coexisting in
the flow domain. Equations for conservation of mass, momentum and energy are solved for each
phase. The share of the flow domain occupied by each phase is given by its volume fraction and each
phase has its own velocity, temperature and physical properties. Interactions between phases due to
differences in velocity and temperature are taken into account via the inter-phase transfer terms in
the transport equations. Eulerian multi-phase modelling provides a general framework for all types
of multi-phase flows; both dispersed (e.g. bubble, droplet, and particle flows) and stratified (e.g. free-
surface flows) flows can be modelled. Comparing the Eulerian multi-phase with the Lagrangian two-
phase method, the former has the advantage of being computationally more efficient in situations
where the phases are widely dispersed and/or when the dispersed phase volume fraction is high.
For free-surface flows, similar advantages could be found in the Eulerian model relative to the
previously developed approach. However, the free surface calculated will be less sharp in
comparison with the Volume of Fluid (VOF) method.
2.7.3 Volume of Fluid (VOF) Model
The VOF Model is designed to track the position of the interface between two or more immiscible
fluids
19
. VOF is an Eulerian fixed-grid technique which solves one set of momentum equations for all
fluids. Tracking is accomplished by solution of phase continuity equation resulting in volume
fraction as:
Eq. 2.7.1
19
C. W. Hirt and B. D. Nichols, “Volume of Fluid (VOF) Method for the Dynamics of Free Boundaries”, Journal of
Computational Physics 39, 201-225 -1981.
Assumes that each control volume contains just one phase (or the interface between phases). Solves
one set of momentum equations for all fluids. A mixture fluid momentum equation is solved using
mixture material properties. Thus the mixture fluid material properties experience jump across the
interface. Turbulence and energy equations are also solved for mixture fluid. Surface tension and
wall adhesion effects can be taken into account. Mass transfer between phases can be modeled by
using a user defined subroutine to specify a nonzero value for Sεκ. Volume of fluid model used for
immiscible fluids with clearly defined interface. Typical problems are:
➢ Jet breakup
➢ Motion of large
bubbles in a
liquid
20
➢ Motion of liquid
after a dam break
(see Figure 2.7.2)
➢ Steady or transient
tracking of any
liquid-gas
interface.
21
A simple everyday example
of 2 phase flow using VOF
scheme would be pouring milk in your coffee, as demonstrated by [Shekhar]
22
in LinkedIn. Instances
of VOF modeling are numerous and far between, such as example of water and oil mixing on a pipe
(see next sections).
Recently, [Huang and Xie]
23
came up with a generic balanced-force algorithm to solve the
incompressible multiphase flows with complex interfaces and large density ratios on the polyhedral
unstructured grids of large non-orthogonality, skewness and non-uniformity. This algorithm
combines the finite volume method based on the volume of fluid (VOF) approach, with the fractional
step.
20
Inappropriate if bubbles are small compared to a control volume (e.g., bubble columns).
21
André Bakker, “Lecture 16 - Free Surface Flows - Applied Computational Fluid Dynamics”, Fluent Inc. (2002).
22
Suman Shekhar, Indian Institute of Technology, India. https://www.linkedin.com/feed/hashtag/
23
Yichen Huang, BinXie
A generic balanced-force algorithm for finite volume method on polyhedral
unstructured grids with non-orthogonality
nal Physics, 479 (2023) 112010
Figure 2.7.2 Transient Simulation of a Dam Break (Courtesy of Bakker)
2.7.3.1 Case Study 1 - VOF Simulation for Stratified Oil-Water Two-Phase Flow in a Horizontal Pipe
Authors : Adib Zulhilmi Mohd Alias , Jaswar Koto, and Yasser Mohamed Ahmed
Title : CFD Simulation for Stratified Oil-Water Two-Phase Flow in a Horizontal Pipe
Appeared in : Science and Engineering, 2014.
Source : The 1st Conference on Ocean, Mechanical and Aerospace. Published by International Society of
Ocean, Mechanical and Aerospace Scientists and Engineers.
Oil-water two-phase flow in 0.0254m horizontal pipe is simulated using FLUENT 6.2 [Zulhilmi Mohd
Alias st al.]
24
. The stratified flow regime is modeled using Volume of Fluid (VOF) with turbulent
model RNG k-ε. Grid independent study has been conducted to decide mesh size for solution accuracy
and optimum computational cost. The simulation is performed in time-dependent simulation where
oil and water are initially separated by patching the region base on difference in density. Observation
on the effect of velocity to the pressure gradient was also simulated. Flow velocity at 0.2, 0.5, 0.8 and
1.1 m/s with same volume fraction for each phase with appropriate multiphase model and
turbulence model are presented.
2.7.3.1.1 Introduction
Immiscible liquid-liquid flow is a common occurrence encountered in a variety of industrial
processes. In oil and gas industry, oil transportation either from reservoir to processing facilities or
to onshore refinery are usually transported in multiphase flow condition since water and oil are
normally produced together. Fractions of water are usually influenced by its existence within the
stratum and also through oil recovery method which used water to enhance the remaining oil in the
reservoir. The presence of water, during the transportation of oil has a significant effect because the
flow is no longer can be treated as a single-phase flow. Oil-water has complex interfacial structure
which complicates the hydrodynamic prediction of the fluid flow. Changes in water fraction may
influence the power required to pump the fluid due to corresponding changes in pipeline pressure
drop. Either water-in-oil or oil-in-water dispersions, both can influence the pressure gradient
dramatically.
2.7.3.1.2 Literature Survey
Computational fluid dynamics (CFD) techniques have been used to simulate the stratified pipe flow.
One of the early CFD models of turbulent stratified flow in a horizontal pipe was presented by
[Shoham and Taitel [1] where a 2D simulation for liquid-gas flow was simulated by adopting zero-
equation models for the liquid region flow field while the gas region was treated as a bulk flow. Issa
[2] numerically simulated the stratified gas liquid pipe flow, using standard k-ε turbulence model
with wall functions for each phase.
[Newton and Behnia [3] obtained more satisfactory solutions for stratified pipe flow by employing a
low Reynolds number turbulent model instead of wall functions. Hui et al [4] simulated stratified oil-
water two-phase turbulent flow in a horizontal tube by applying RNG k-ε model combined with a
near-wall low-Re turbulence model to each phase and they adopt continuum surface force
approximation for the calculation of surface tension. Their simulation results was compared with
[Elseth et al [5] who simulated the turbulent stratified flow, however their numerical results are not
acceptable when compared with their measured data.
Stratified oil-water two-phase pipe flow was investigated using different type of multiphase model.
[Awal et al [6] achieved CFD simulation tool to investigate inline oil and water separation
characteristics under downhole conditions. They chose the Eulerian-Eulerian model, which is
computationally most comprehensive but more suitable for multiphase systems with the dispersed
phase exceeding 10% v/v/. Carlos F. [7] developed a 2D model for fully-developed, turbulent-
24
Adib Zulhilmi Mohd Alias , Jaswar Koto, and Yasser Mohamed Ahmed, “CFD Simulation for Stratified Oil-
Water Two-Phase Flow in a Horizontal Pipe”, The 1st Conference on Ocean, Mechanical and Aerospace, 2014.
turbulent oil-water stratified flow using finite-volume method in a bipolar coordinate system and
applying a simple mixing-length turbulence model. Hui et al [4] and Al-Yaari et al [8] simulated
stratified oil-water two-phase turbulent flow in a horizontal tube numerically using a volume of fluid
(VOF) model.
They applied RNG k-ε model with enhanced wall function combined with optimum meshes through
grid independent study to obtain clearly separated oil layer and optimum computational cost. In the
present paper multiphase model of Volume of Fluid (VOF) is used to model the stratified oil-water
flow. Optimum number of elements for simulation accuracy has been conducted through grid
independent study. Observation on the effect of velocity to the pressure gradient was also simulated
at flow velocity 0.2, 0.5, 0.8 and 1.1 m/s with same volume fraction for each phase.
2.7.3.1.3 Numerical Simulation (Geometry and Mesh)
The domain and the meshes were created using ANSYS Design Modeler. A sketch of the geometry of
the calculation domain is shown in Figure 2.7.3. The geometry consists of semicircular inlet for oil
and water with 1 meter length of the flow domain. The inlet for both phases is at the same inlet face
where oil on top and water at the bottom region. This will initially made the flow in stratified
condition. In addition, as both inlets also flew with a same velocity with direction almost parallel to
each phase makes fewer disturbances to maintain stratified flow. The diameter of the pipe for the
present work is 0.0254 m. In order to keep the volume of oil and water are flowing continuously
throughout the domain until the outlet, patch file and adapt region is used to declare the top and
bottom regions for oil and water. This will avoid insufficient volume of either phase.
A block-structured meshing approach was used to create meshes with only tri/tet cells. To obtain
fine meshing scheme, sizing was setup with curvature normal angle ll degree, 0.0001 minimum size
and 3.0 m maximum size. While to improve the flow near the wall region, two layer inflation with
growth rate 1.2 is adapted
2.7.3.1.4 Boundary
Conditions
There are three faces bounding
the calculation domain: the
inlet boundary, the wall
boundary and the outlet
boundary. Flat velocity profile
for oil and water were
introduced at the inlet of their
sections. The outlet boundary condition at the end was set up as a pressure outlet boundary. No slip
was used to model liquid velocity at the wall. The main fluid phases’ physical properties are reported
in Table 2.7.4.
Figure 2.7.3 Schematic Representation of Pipe Flow and cross-sectional Mesh
Table 2.7.4 Fluid Phases Physical Properties
2.7.3.1.5 Solution Strategy And Convergence
Pressure-based solver is chose since it was applicable for wide range of flow regimes from low speed
incompressible flow to high speed compressible flow. This solver also requires less memory
(storage) and allows flexibility in the solution procedure. Green-gauss Node-Based is elected for
higher order discretization scheme since it is more accurate for tri/tet meshes. For pressure,
PRESTO! discretization scheme was used for pressure, second order upwind discretization scheme
was used for the momentum equation, volume fraction, turbulent, kinetic and turbulent dissipation
energy. Second-order upwind is chose rather than First-order upwind because it uses larger stencils
for 2nd order accuracy and essential with tri/tet mesh even though the solution to converge may be
slower but manageable. In addition, the simulation is time dependent (transient) with 1000 time
steps, 0.01 time step size and 200 iterations at each time step size.
2.7.3.1.6 Results
In this section one presents, use of Volume of Fluid multiphase model along with RNG k-ε for
turbulent model, grid independent test and sample of pressure drop prediction using this simulation
Figure 2.7.4 Oil Volume Fraction Contours At Pipe Length (Z = 0.5 M) of Different Size Mesh
2.7.3.1.7 Grid Independent Study
A grid independent study is conducted to obtain sufficient mesh density as it was necessary to resolve
accurate flow. A grid independent solution exists when the solution does not change when the mesh
is refined. The computational grid of 46631, 79488, 104584 and 142374 elements were tested for
the mesh independent study to find out the optimum size of the mesh to be used for simulation.
Figure 2.7.4 shows an oil volume fraction contours at plane z = 0.5 m which indicates the accuracy
of the mesh to display the flow pattern. As shown in figure, system increased number of elements
shows better prediction for stratified flow pattern with smoothness of the clearly oil and mixed layer.
46631 showing bad prediction on the oil and mixed layer since insufficient amount of elements could
not give detail prediction especially on the mixed layer. Both meshes for 104584 and 142374 gave
almost similar contours of oil fraction with slight differences in the smoothness of the clearly oil and
mixed layer. Therefore, based on the oil volume fraction contours results, 142374 cells are the most
optimum number of cells required to predict the oil-water stratified flow in the tested domain and
such mesh is going to be used for simulation.
In addition, such decision has been tested by comparing the pressure profiles obtain for every meshes
tested (Chart 1-not shown). At mesh size 46631, 68204 and 79488, the pressure plot is away from
the other plots. The pressure profile starts to unchanged with mesh 92440 until 171393. Before
deciding th e best meshes size, simulation cost also is required to look at. Since increase num of
meshes will increase the amount of time for simulation, the meshes size of 142374 is the most
optimum number of elements could be chose.
2.7.3.1.8 Pressure Prediction at Different Flow Velocity
By using the simulated oil-water stratified flow, pressure prediction at different flow velocity have
been conducted. Flow velocity of 0.2, 0.5, 0.8 and 1.1 m/s with (0.5 input water volume fraction) as a
sample flow pattern has been simulated. Volume of fluid (VOF) multiphase model with RNG k-ε model
was used for simulation the tested domain containing 142374 cells (the optimum mesh size) based
on the decision mentioned earlier in this paper. At such condition, the oil-water flow pattern
simulated is seen stratified (see Figure 2.7.5) with multiple layers of phase density in the middle of
the pipe where the oil and water phases met.
2.7.3.1.9 Conclusions
The following conclusive remarks result from our analysis. As far as the fluid dynamic analysis is
concerned:
1 CFD calculations using Fluent 6.2 were performed to predict the oil-water stratified flow in
0.0254 m horizontal pipe.
2 Volume of Fluid (VOF) multiphase model with RNG k-ε two equations turbulent model was
selected among other different multiphase and turbulent models based on the convergence,
prediction off the oil-water stratified flow pattern and the smoothness of the interface.
3 Mesh independent study has been achieved to decide on the optimum mesh size to be used
in the simulation process.
4 Pressure prediction base on different flow velocity have been observed. It can be seen that as
velocity increases, the pressure gradient also increases.
Figure 2.7.5 Stratified Oil-Water Flow Simulation
5 The pressure prediction will be extended to examine the effect from different water volume
fraction.
Acknowledgements
The authors are very grateful to Universiti Teknologi Malaysia, Ocean and Aerospace Research Institute,
Indonesia for supporting this study. Authors are also grateful for useful
discussions with my family and all my friends.
2.7.3.1.10 Reference
1. O.Shoham, Y.Taitel, “Stratified turbulent-turbulent gas liquid flow in horizontal and inclined pipes”,
AIChE J. 30 (2) (1984) 377-385.
2. R.I, Issa, “Prediction of turbulent, stratified, two-phase flow in inclined pipes and channels”, Int. J.
Multiphase Flow 14 (1) (1988) 141-154.
3. C.H. Newton, M. Behnia, “Numerical calculation of turbulent stratified gas-liquid pipe flows”, Int. J.
Multiphase Flow 24 (5) (1998) 141-154.
4. Hui gao, Han-Yang Gu and Lie-Jin Guo, “Numerical study of stratified oil-water two-phase turbulent
flow in a horizontal tube”, Int. J. heat and mass transfer, (46) (2003) 749-754
5. G. Elseth, H.K. Kvandal, M.C. Melaaen, “Measurement of velocity and phase fraction in stratified oil-
water flow”, International Symposium on Multiphase Flow and Transport Phenomena, Antalya,
Turkey, pp.206-210, 2000
6. Awal, Mohammad R., Zughbi, Habib D., Razzak, Shaikh A., Al-Majed, Abdulaziz A., and Al-Yousef,
hasan Y., “Liquids phase holdup and separation characteristics as a function of well inclination and
flowrate”, SPE SA, 2005, 14-16 May.
7. Carlos F. “Modelling of oil-water flow in horizontal and near horizontal pipes”, PhD Thesis, Tulsa
University, 2006.
8. Al-Yaari, M., and Abu-Sharkh, “CFD Prediction of stratified oil-water flow in a horizontal pipe”,
Asian Transactions on Engineering Volume 01 Issue 05, November 2011.
2.7.3.2 Case Study 2 - Application of Volume Of Fluid (VOF) Method for Prediction of Wave
Generated by Flow around Cambered Hydrofoil on a Free Surface
Authors : Md. Imran Uddin1, Md. Mashud Karim2
Affiliations : 1Lecturer, Accident Research Institute (ARI), Bangladesh University of Engineering and
Technology (BUET), Dhaka-1000, Bangladesh (BUET), Dhaka- 1000, Bangladesh
2Professor, Department of Naval Architecture and Marine Engineering (NAME),
Bangladesh University of Engineering and Technology (BUET), Dhaka-1000, Bangladesh
Title of Paper : Application of Volume of Fluid (VOF) Method for Prediction of Wave Generated by Flow
around Cambered Hydrofoil
Appeared in : 10th International Conference on Marine Technology, MARTEC 2016
Source : Available online at www.sciencedirect.com
Citation : Md. Imran Uddin, and Md. Mashud Karim. "Application of Volume of Fluid (VOF) Method for
Prediction of Wave Generated by Flow around Cambered Hydrofoil" Procedia Engineering, vol. 194,
2017. DOI:10.1016/j.proeng.2017.08.120
The wave generated by flow around cambered hydrofoil NACA 4412 near free surface is predicted
numerically in this study. To solve Reynolds Averaged Navier-Stokes (RANS) equation, two-
dimensional implicit Finite Volume Method (FVM) is applied. The Realizable κ – ε turbulence model
has been implemented at different submergence depth to hydrofoil chord ratios (h/c) ranging from
1 to 5 for capturing the flow around the cambered hydrofoil in the free surface zone. The Volume Of
Fluid (VOF) method has been applied to determine the free surface effect of water at an angle of
attack of 50 by the hydrofoil. Firstly, the computed result at h/c = 1 is validated by comparing with
the experimental one. Then the wave profiles, contours of velocity magnitude, velocity vectors,
contours of static pressure near the hydrofoil surface are computed at Froude number (Fn ) =1 for
different h/c ratios.
2.7.3.2.1 Introduction
The study of performance of hydrofoil is one of the significant subjects in hydrodynamics. Hydrofoils
are used to diminish drag force and to increase lift force and speed for many marine crafts. In the
design of these marine crafts, evaluation of hydrodynamic behavior of the hydrofoil is very
important. When submergence depth of hydrofoil is small, the free surface effect should be taken into
consideration including evaluations of free surface profile, distribution of pressure, lift and drag
forces. This study is concerned with the wave generated by a 2D cambered hydrofoil moving with
constant speed placed in a steady stream close to the free surface.
The problem has been considered by many researchers
around the world. For the analysis of 2D hydrofoil Bal [1]
applied the potential based panel method. A distribution of
Rankine type sources on the ship hulls and free surfaces
was applied by [Dawson [2]. [Yeung and Bouger [3] applied
a hybrid integral equation method based on Green’s
theorem which satisfied exact body condition and free
surface condition in linearized form. Bai and Han [4]
applied the localized finite-element method based on the
classical Hamilton’s principle for the nonlinear steady
waves due to 2D hydrofoils. For the calculations of free
surface waves along with lift and drag force of hydrofoils,
vertical struts and Wigley ship hulls, Janson [5] applied
linear and nonlinear potential flow.
Kouh et al. [6] analyzed the performance of 2D hydrofoil
near free surface by distributing the source on undisturbed
Nomenclature
CL lift coefficient
CD drag coefficient
Fn Froude number
g acceleration due to gravity
h height of the free surface
Re Reynolds number
Uavg mean flow velocity
ρ density
α volume fraction
κ turbulent kinetic energy
ε turbulent dissipation rate
μt turbulent viscosity
free surface and also doublet on foil and wake surface. In that analysis, instead of Neumann-type
boundary condition, Dirichlet-type body boundary condition was used and the free surface condition
was linearized by free stream potential. [Chen and Liu [7] employed vortex lattice method for the
calculation of flow around hydrofoil by distributing the doublet on a sub-surface inside the body.
[Ghassemi and Kohansal [8] presented nonlinear free surface flow and boundary element method of
higher order on various types of surface and submerged bodies. More recently, Karim et al.[9]
employed numerical simulation of free surface water wave for the flow around the hydrofoil NACA
0015 by using the Volume Of Fluid (VOF) method.
The main focus of this analysis is laid on the wave generation by a submerged cambered
hydrofoil at different submergence depth ratios to compute the wave amplitudes, lift and drag
forces near the free surface. For simulation of the problem where both the fluids i.e. air and water
are considered as single effective fluid, the interface capturing method is applied there. At first the
method is applied to cambered hydrofoil NACA 4412 at submergence depth ratio of one for
comparing the computed results with the experimental results of [Kouh et al. [6]. Then the method
is applied for various submergence depth ratios ranging from one to five at Fn=1.00 and Re =2.79 ×
105 for obtaining the wave elevations, contour of static pressure and velocity magnitude and values
of lift and drag coefficients near the hydrofoil.
2.7.3.2.2 Theoretical Formulation
The Reynolds Averaged Navier-Stokes (RANS) equation is used to simulate the incompressible
viscous flow around the submerged hydrofoil. The RANS equation requires appropriate modelling of
Reynolds stress (−ρu´iu´j). The main equation of the flow field and mathematical expression of
turbulence model are given below:
1. In Cartesian tensor notation the RANS equation may be expressed as
Eq. 2.7.2
Boussinesq hypothesis can be applied to relate the Reynolds stresses with mean velocity gradients
as follows:
Eq. 2.7.3
This approach has the advantage of relatively low computational cost for computing turbulent
viscosity, μt .
2. The equation of realizable κ – ε turbulence model can be expressed as
Eq. 2.7.4
In these equations Gκ is the generation of turbulent kinetic energy due to the mean velocity gradients
and Gb represents the generation of turbulent kinetic energy due to buoyancy, YM is the contribution
of the fluctuating dilatation in compressible turbulence to the overall dissipation rate, C2 and C1ε are
constant terms, σκ and represents the turbulent Prandtl numbers for κ and respectively and Sκ and
Sε are user defined source terms. The turbulent viscosity μt can be computed by combining κ and ε as
given below:
Eq. 2.7.5
The turbulent kinetic energy κ and turbulent dissipation rate ε are expressed as
Eq. 2.7.6
where, Uavg represents the mean flow velocity, I is the turbulent intensity = 0.16 (Re)−(1/8) and, l
=0.007L (for details Fluent Inc. [10] can be seen). For simulation of the free surface wave generation,
Marker-And-Cell (MAC) and fractional Volume Of Fluid (VOF) are often used. The MAC method
calculates the free surface by recording movement of each of the fluid particles. So, it often needs
huge amount of computational space for storage and consumes substantial amount of time for
computation. The VOF method can be helpful to overcome this shortcoming. It is used to compute the
surface wave that is caused by the submerged hydrofoil that moves near the free surface of water.
The governing equation of the VOF method is expressed as
Eq. 2.7.7
where, F is a function having a value of unity at any point in the fluid. For a cell full of fluid a unit
value of F is used. A zero value of F is used for a cell that contains no fluid and a cell that has a value
between one and zero contains a free surface. The VOF formulation applies the concept that two or
more fluids (or phases) are not interpenetrating. For each additional phase a variable is introduced
with the volume fraction of the phase in the computational cell. In each of the control volume, the
volume fraction of all the phases sum to a value of unity. As long as the volume fraction of each of the
phases is known at each location, the fields for all variables and properties are shared by the phases
and represent volume-averaged values. Thus the variables and properties in any particular cell are
either purely representative of one of the phases, or representative of a mixture of the phases,
depending upon the values of volume fraction. In other words, if the volume fraction of qth fluid in the
cell is denoted as αq, then three conditions are possible as given below
➢ αq = 0 : the cell is empty (of the qth fluid).
➢ αq = 1: the cell is full (of the qth fluid)
➢ 0 ≤ αq ≤ 1 : the cell contains the interface between the qth fluid and one or more other fluids.
The appropriate properties and variables will be assigned to each control volume within the domain
based on the local value of αq. The tracking of the interface between the phases is done by the solution
of a continuity equation for the volume fraction of one of the phases ( see Eq. 2.8.1). For the qth
phase, this equation is of the following form:
Eq. 2.7.8
where, m˙pq is the mass transfer from phase p to phase q and m˙qp is the mass transfer from phase q
to phase p. The volume fraction equation will not be solved for the primary phase. The volume
fraction of the primary phase will be computed based on the following constraint:
Eq. 2.7.9
2.7.3.2.3 Numerical Simulation
For numerical simulation the computational domain is created and simulations are run with the two-
dimensional model of NACA 4412 hydrofoil at h/c=1. Then the computed results are compared with
the experimental results of [Kouh et al. [6] to validate the computational models for observing the
free surface effect near the hydrofoil. Finally, the simulations are carried out for submergence depth
ratios ranging from one to five to observe the pattern of free surface near the hydrofoil. A two
dimensional flow field is modelled around the hydrofoil. For construction of the computational
domain the commercial meshing software Pointwise (Version 17.0 R2) [11] is used. The geometry of
the hydrofoil is constructed by using standard NACA 4412 coordinates. The origin of the coordinate
system is placed at the leading edge of the hydrofoil and the hydrofoil is set to an angle of attack of
5. The length of the inlet and outlet boundaries is 10c each whereas that of upper and lower
boundaries is 17.5 C each where c denotes the chord
length of the hydrofoil. The hydrofoil is placed at a
distance 5c right from the inlet boundary. The distance
from trailing edge of hydrofoil to the outlet is kept to
11.5 C. The meshing of the faces is made by
quadrilateral elements throughout the computational
domain. For the computational domain a total of
841866 structured cells are used. A fine meshing is
employed near the hydrofoil and free surface. Since the
hydrofoil has blunt section at the trailing edge so a fine
meshing is also employed there for better capturing of
wave profile. At the rest of the computational domain a
coarse meshing is employed. The boundary conditions
of the computational domain are shown in Table
2.7.5. For inlet and outlet boundaries the ’pressure inlet’ and ’pressure outlet’ boundary conditions
are applied respectively. The ’symmetric’ boundary condition is used at the upper boundary surface.
For both lower boundary and hydrofoil the boundary condition of ’stationary wall’ is used in which
no slip shear condition is employed.
For solving Reynolds Averaged Navier Stokes (RANS) equation the two-dimensional implicit Finite
Volume Method (FVM) is employed. The Volume Of Fluid (VOF) method along with the Realizable κ
Table 2.7.5 Different Boundary Types of
The Domain
− ε turbulence model is implemented to capture the flow around the hydrofoil in the free surface
region at various submergence ratios (h/c). The non-equilibrium wall function is employed for near
wall treatment. The SIMPLEC algorithm is applied for coupling between pressure and velocity. The
body force weighted scheme is applied for discretization of pressure. For discretization of volume
fraction, momentum, turbulent kinetic energy and turbulent dissipation rate the second order
upwind scheme is applied. The whole region of the computational domain is patched for velocity of
1.4 m/s along x-direction. And the region from free surface to the bottom boundary is adapted to
patch under volume fraction of one since it contain water as fluid. The complete analysis of the flow
around hydrofoil is done by the renowned CFD software, FLUENT 6.3.26 [10].
2.7.3.2.4 Results and Discussion
To validate the computed numerical results with the experimental results of [Kouh et al. [6], a
hydrofoil having chord length of 20 cm, velocity 1.4 m/s, angle of attack 50, Froude number 1.00 and
Reynolds number 2.79 × 105 is modelled. The grid independency of the computed results is checked
by using four grids namely Grid 1, Grid 2, Grid 3 and Grid 4. The Grid 1 consists of 841866 cells, Grid
2 930156 cells, Grid 3 1021638 cells and Grid 4 1116147 cells. The wave profiles obtained by using
those four meshes are illustrated in Figure 2.7.6; from which it is seen that all the four grids provide
nearly the same results.
In Figure 2.7.7 (a) and Figure 2.7.7 (b), the computed values of lift and drag coefficient for four
grids are shown respectively. In this case also very slight fluctuation occurs between the results
provided by the grids. The percentage variation of lift and drag coefficients with different grids is
shown in Table 2.7.6.
It is seen that there is negligible
amount of variation between the
results provided by different
grids. So, Grid 1 is chosen for this
study to reduce CPU time, since it
has least number of cells. More
refined mesh could produce
better results but due to
limitation of computer resources
and to reduce CPU time, Grid 1 is
Table 2.7.6 Difference of Lift And Drag Coefficients Between
Different Grids
Figure 2.7.6 Grid Independency Check According To Wave Height
used in this study. The comparison between the present computational results and the experimental
results is shown in Figure 2.7.7 (a). It is seen from the figure that the computed wave elevations
demonstrates good concurrence with the experimental wave elevations. Then numerical simulation
is carried out for various submergence depth ratios of hydrofoil. In Figure 2.7.7 (b) the convergence
history of the simulation for h/c =1 after 20 s is illustrated. It is observed that after the iteration
number of 9500, i.e. at time 19s the various residual parameters stay nearly constant. The free
surface wave profiles for different submergence depth ratios h/c are compared in Figure 2.7.10.
With the increase in the ratio of h/c the maximum amplitudes of the wave crest and trough reduce.
From the figure it can also be seen that there is almost no effect due to hydrofoil on the free surface
at h/c = 5.0. Therefore, submergence depth ratios of greater than 5.0 may be taken as deep water
case. The contour of static pressure around NACA 4412 hydrofoil at various depths of water is shown
in Figure 2.7.8. As the depth increases the static pressure gradually increases from the free surface
Figure 2.7.7 Grid Independence Study of Airfoil Forces
(a) CLvs Number of Cells (b) CDvs Number of Cells
Figure 2.7.8 Comparison of Wave Elevations For NACA 4412 Hydrofoil At Various H/C Ratios
level of water (as indicated by
the blue color). The highest
pressure of the computational
domain is at the bottom
boundary (as indicated by red
color).
Figure 2.7.8 shows the
computational domain having
no color filled in it. The figure is
a close up view to hydrofoil
from which the pattern of
decrease of wave amplitude
with increase of water depth is
observed clearly. Figure 2.7.9
(a) shows the contour of
velocity magnitude around the
hydrofoil at h/c=1. It is seen
from the figure that the
fluid velocity is lesser than
the average value (1.4 m/s)
below the crest and above
the trough and greater
above the crest and below
the trough. Figure 2.7.9
(b) shows the velocity
vectors which are colored
by velocity magnitude. The
velocity of fluid is lower at
the leading edge and
trailing edge than the rest of
the surface of hydrofoil The lift and drag coefficients of the cambered hydrofoil NACA 4412 for
different submergence depth ratios ranging from one to five are shown in Table 2.7.7. It is seen
that with the increase in submergence depth, the values of lift coefficients increase and drag
coefficients of hydrofoil decrease gradually.
Table 2.7.7 Lift And Drag Coefficients For Different Submergence
Depths of Cambered Hydrofoil NACA 4412
Figure 2.7.10 Contour of Static Pressure Near NACA 4412
Hydrofoil And Free Surface At H/C = 1
Figure 2.7.9 (A) Contour of Velocity Magnitude Around The Hydrofoil At H/C=1 ; (B) Velocity Vectors
Around The Hydrofoil At H/C=1
2.7.3.2.5 Conclusions
The following conclusions can be drawn from the above study:
• The Two-dimensional implicit Finite Volume Method (FVM) shows satisfactory results for
analyzing the wave generated by flow around the cambered hydrofoil NACA 4412 near free
surface.
• The Volume Of Fluid (VOF) method with the Realizable κ−ε turbulence model satisfactorily
predicts the wave generated by flow around the cambered hydrofoil.
• The amplitude of wave generated by flow around the hydrofoil decreases with the increase
in submergence depth. At submergence depth ratio of five, the effect of hydrofoil on free
surface is almost disappeared. So, the submergence depth ratios more than five can be
considered as the deep water case.
• With the increase in submergence depth of hydrofoil, the values of lift coefficients increase
and drag coefficients decrease gradually.
Acknowledgements
The authors are grateful to Bangladesh University of Engineering and Technology for all type of
supports.
2.7.3.2.6 References
[1] Bal S., A potential based panel method for 2-D hydrofoil, J. Ocean Engineering, 26 (1999) 343-361.
[2] Dawson, C. W., A practical computer method for solving ship-wave problems, Proceedings of
Second International Conference on Numerical Ship Hydrodynamics, 1977, pp. 30-38.
[3] Yeung, R.W., Bouger, Y. C., A hybrid-integral equation method for steady two- dimensional ship
waves, Int. J. Num. Meth. Eng., 1979, Volume 14, pp. 317-336.
[4] Bai, K.J. and Han, J.H., A localized finite-element method for the nonlinear steady waves due to a
two- dimensional hydrofoil, J. Ship Res., 38 (1994) 4251.
[5] JJanson, C.E., Potential flow panel method for the calculation of free surface flows with lift, Ph. D.
thesis, Chalmers University of Technology, 1997.
[6] Kouh, J.S., Lin, T.J., Chau, S.W., Performance analysis of two-dimensional hydrofoil under free
surface. J. Natl. Taiwan Univ., 2002, pp. 86..
[7] Chen, C.K., Liu, H., 2005.A submerged vortex lattice method for calculation of the flow around
three-dimensional hydrofoil, J. Ship Mech., 2005, Volume 9, Issue 2.
[8] Ghassemi, H., Kohansal, A.R., Higher order boundary element method applied to the hydrofoil
beneath the free surface, Proceedings of the 28th International Conference on OMAE, USA, 2009.
[9] Karim, Md.M., Prasad, B., Rahman, N., Numerical simulation of free surface water wave for the
flow around NACA 0015 hydrofoil using the volume Of fluid (VOF) method, J. Ocean Engineering,
2014, Volume 78, pp. 89-94.
[10] Fluent Inc., 2006, FLUENT 6.3 User’s Guide.
[11] Pointwise, Inc., 2012, Pointwise 17.0 R2 User Manual.
2.7.3.3 Case 3 - Numerical Simulations of Submarine Self-propulsion Flows near the Free Surface
Authors : Enkai Guo1, Liushuai Cao1, Zhiben Shen2, Yun Wang2
Affiliation : 1 Computational Marine Hydrodynamics Lab (CMHL), School of Naval Architecture,
Ocean and Civil Engineering, Shanghai Jiao Tong University, Shanghai, China.
2 Wuhan Second Ship Design and Research Institute, Wuhan, China.
Title : Numerical Simulations of Submarine Self-propulsion Flows near the Free Surface
License : Published under license by IOP Publishing Ltd. The 12th International Workshop on Ship
and Marine Hydrodynamics IOP Conf. Series: Materials Science and Engineering 1288 (2023) 012055
-IOP Publishing, doi:10.1088/1757-899X/1288/1/012055
Content from this work may be used under the terms of the Creative Commons Attribution 3.0
license.
2.7.3.3.1 Abstract
Submarine needs to complete more tasks near the free-surface area in modern war. When sailing
near the free surface, the self-propelled characteristics of the submarine and its nearby flow field will
be affected by the free surface. This paper presents the research on the self-propulsion submarine
near the free surface with computational fluid dynamics (CFD) method. We take the generic Joubert
BB2 submarine and Marine 7371R propeller models as the research objects. The RANS method and
SST k-ω turbulence model are selected to solve the turbulent flows. The volume of fluid (VOF)
method is used to capture the free surface. Grid convergence study is performed based on three sets
of grids with different resolution. Numerical simulations are performed under the self-propulsion
cases with different submergence depths and velocities. The proportional integral (PI) controller
method is proposed to obtain the self-propulsion point. The results are more accurate compared with
the traditional one. It is found that with the decrease of the submergence depths, the rotating speed
of the self-propelled point and the corresponding thrust increase. The study also explores the free
surface effect on flow field characteristics, wave-making characteristics and vortex structures. The
scientific findings provide some useful results for the self-propulsion submarines near the free
surface and support the further research in the future.
2.7.3.3.2 Introduction
Modern warfare requires submarines to perform a variety of tasks in near-free-surface conditions,
such as navigating in near-free-surface formations, coordinating with air forces, launching missiles,
and entering or leaving ports for maintenance and resupply. Additionally, submarine listening,
surveillance, and special operations capabilities in shallow coastal waters are becoming increasingly
important. Modern operations require that submarines not only stick to deep-water operations, but
also have near surface combat capabilities. Research has shown that the hydrodynamic performance
and flow field characteristics of submarines change significantly when sailing near the free surface.
Different research methods have been used to investigate this phenomenon, including theoretical
analysis, model experiments, and computational fluid dynamics (CFD). Theoretical analysis method
is an important method. Some early scholars used slice theory and potential flow method to solve the
hydrodynamic performance of the near-surface submarines [1].
Gourlay and Dawson [2] adopted the Havelock-source panel method to describe the potential flow
around submarines near the free surface. It is found that the method can accurately calculate the
wave resistance, pressure drag, vertical force, and trim moment of DARPA SUBOFF and Joubert
submarines compared with the experimental data. The method also shows advantages in
computation speed, simplicity and robustness. However, the theoretical method is often limited by
conditions and experience, such as the selection of empirical formula, which is insufficient to deal
with complex flow field problems. The results of theoretical analysis often need to be verified by
experimental data.
The advantage of the model experiment method is that it can create a real physical environment,
therefore the results are highly reliable. Wang et al. [3] determined the hydrodynamic performance
and wake characteristics of the submarine propeller when it is self-propelled near the free surface
by using stereoscopic particle image velocimetry (SPIV) method. However, the model experiment
method also has some shortcomings, such as the limitation of test conditions and the difficulty of flow
field measurement. So, there are few documents and articles on the study self-propulsion of
submarine near the free surface by using the model experiment method, which lacks sufficient data
support.
With the rapid development of CFD technology, simulation software based on CFD can quickly
analyze and simulate the flow characteristics of submarines. Many researchers have investigated the
relative problems with different CFD methods. Lungu [4] used the detached eddy simulation (DES)
method to study the flow around the self-propelled SUBOFF submarine near the free surface and
mainly discussed the wave variation under different conditions. Li et al. [5] coupled the Reynolds-
Averaged Navier-Stokes (RANS) equation with k-ω turbulence model to conduct the self-propulsion
simulation and analyze the influence of the free surface on the performance of propeller. Carrica [6]
used a general purpose CFD code REX to conduct near-surface self-propulsion simulations and study
the hydrodynamics performance of submarine and propeller both in calm water and waves. Dong [7]
used RANS solver to simulate the impact of long-crested waves on the self-propulsion submarines.
Huang et al. [8] also used RANS method to analyze the wave-making characteristics of the near-
surface submarines.
This paper presents the research on the self-propulsion submarines near the free surface. The study
in this paper takes the standard Joubert BB2 submarine and Marine 7371R propeller as the research
object. The RANS equation and SST k-ω turbulence model is selected. The VOF method is used to
establish the free surface. Numerical simulations are conducted under the cases with different
submergence depths and velocities. The linear interpolation method and the PI controller method
are applied to obtain the self-propulsion points. There is no significant difference between their
results. The results are compared to explore the influence of and submergence depth on submarines
self-propulsion performance, flow field characteristics, wave-making characteristics and vortex
structures. All of the simulations are conducted based on the CFD software STAR-CCM+.
2.7.3.3.3 Methodology
2.7.3.3.4 Submarine and Propeller Geometries
The Joubert BB2 submarine model and six-bladed propeller 7371R model were used for the self-
propulsion study. They were both designed by Maritime Research Institute Netherlands (MARIN).
shows the entire self-propulsion model and the appendages on it. The BB2 model consists of main
hull, sail, sailplanes and X rudders. Table 2.7.8 shows the main parameters of the submarine and
propeller models at model scale (λ=18.348) and full scale boundary is 4.18L away from the tail tip of
submarine which is defined as pressure outlet. The top boundary is 2.09L away from the submarine’s
Table 2.7.8 The main parameters of the submarine and propeller models.
surface. The bottom boundary is 4.18L away from the submarine’s surface. The bilateral boundaries
are 4.18L away from the port or starboard. They are all defined as plane. The surfaces of body
(including hull, appendages, propeller blades and shaft) are defined as no-slip wall. As shown in
Error! Reference source not found., the free surface is established parallel to the submarine’s base
plane (z = 0 plane). The distance between the base plane and the free surface is defined as the
submergence depth H. The
static region is divided
into air domain and water
domain by the free
surface.
2.7.3.3.5 Governing
Equations
and
Turbulence
Model
Simulations in this study
were conducted by solving
Reynolds-Averaged
Navier-Stokes (RANS)
equations in STAR-CCM+ software. The flow is incompressible and turbulent. The governing
equations of RANS method can be expressed as follows:
Eq. 2.7.10
Eq. 2.7.11
where , and are the time averaged values of velocity component, force and pressure. In this
study, the SST k-ω turbulence model is selected to close the solving equations, which is proposed by
Menter [9]. It uses k-ω model to deal with the flow in the boundary layer and k-ε to deal with the
flow of free fluid. Its transport equations are given as:
Figure 2.7.11 The submarine and propeller model
Figure 2.7.12 The computational domain
Eq. 2.7.12
Eq. 2.7.13
where Γ, Γ represent the effective diffusivity; G, G represent the turbulent kinetic energy; Y , Y
represent the energy dissipation; S, S represent the source item.
2.7.3.3.6 Free Surface Model
Volume of fluid (VOF) method is a moving interface tracking method based on Euler grid, which is
proposed by Hirt and Nichols [10]. Its basic principle is to simulate the moving interface by defining
a VOF function of the ratio between the volume of the target fluid and the grid, and calculating the
function value on each cell element. VOF method is widely used in the simulation of multiphase
transition. The advantage of VOF method is that it has good mass conservation characteristics and
leads to high accuracy. The free surface separates the air domain and the water domain. The volume
fraction α is introduced to represent the ratio of a kind of fluid in the grid. The α = 0 represents the
air and α =1 represents the water. The equation of calculating the volume fraction α can be expressed
as:
Eq. 2.7.14
2.7.3.3.7 Computational Domain and Boundary Conditions
The computational domain consists of two regions. The outer region is the static region and the inner
region is the rotating region. The rotating region is a cylinder with a diameter of 1.32Dp and a height
of 0.26Dp. It completely encloses the blades and hub of the propeller. The boundary of the rotating
region is defined as interface. The boundary of the static region is a cuboid. The inlet boundary is
3.18L away from the front nose tip of submarine which is defined as velocity inlet. The outlet
2.7.3.3.8 Self-Propulsion Simulation Method
In this study, two different methods were used to obtain self-propulsion point in order to verify the
accuracy of simulation. The first one is a traditional method which was proposed by Yang et al. [11].
The key to this method is to adjust rotating speed in order to balance the thrust of propeller and total
resistance of submarine under fixed velocity. The process is as follows.
1. There is a uniform flow with fixed speed in the computational domain. We estimate an initial
rotating speed through propeller’s open water performance.
2. The numerical simulation is conducted at fixed speed and rotating speed. The thrust (T) value
and resistance (D) value are monitored and noted when they are convergent.
3. If T > D, reduce the rotating speed; If T<D, increase the rotating speed. Then we conduct the
simulation again and repeat the steps above until the thrust value is equal to the resistance
value.
1. When T = D, the corresponding rotating speed represents the self-propulsion point at that
speed. The wake fraction, thrust deduction coefficient and other self-propulsion factors can
be calculated according to the resistance curve of the hull and the open water performance
curve of the propeller.
However, in the realistic operating process, it is often difficult to directly obtain the self-propulsion
point where the thrust value is exactly equal to the resistance value. Therefore, simulations are
conducted at several rotating speeds near the self-propulsion point and the balancing point of thrust
and resistance can be acquired through linear interpolation. The other one is using a proportional-
integral (PI) controller to find the self-propulsion point. A PI controller is designed to drive the
propeller's rotating speed based on the error between the submarine’s current speed and target
speed. During the simulation, the rotating speed is not fixed but changing dynamically. The process
of every step is given in Figure 2.7.13. The general formula for the PI controller can be expressed
as follows:
Eq. 2.7.15
where () is the rotating speed at different times; 0 is the initial value of rotating speed; error is
the error at certain time which means submarine’s target speed minus current speed here. is the
gain for the proportional component of the controller; is the gain for the integral component of the
controller.
2.7.3.3.9 Mesh Generation and Validation
In this study, mesh generation is mainly based on the Trimmed Mesher in both static region and
rotating region. The Prism Layer Mesher is used in the boundary layer around the submarine and the
propeller to simulate the fluid flow in the boundary layer more accurately. The mesh is refined in the
turbulence wake region of rudders and sail. Meanwhile the mesh in far field is relatively coarser. To
verifying the mesh dependence and the accuracy of simulation, we totally established three different
grids and classify them as coarse grid, medium grid and fine grid based on their basic cell sizes. Then
all of the grids are used to simulate at deep depth (submergence depth H is big enough) in a fixed
speed of 1.19m/s. The results of rotating speed and thrust at self-propulsion point are compared with
the results from Kim et al. [12] as shown in Table 2.7.9. It can be noticed that all the values of other
cases are well below 4% which is acceptable. The results of the case with the finest grid also don’t
show much superiority compared with others. So there is no need to further increase the grid size.
Table 2.7.9 The results of mesh dependence validation.
Figure 2.7.13 The process of PI controller simulation
The medium grid is finally chosen to be
used for the following simulation which
has an approximate 5.8 million cells. The
details of the mesh in the midship section
are shown in Figure 2.7.14.
2.7.3.3.10 Results and Discussions
2.7.3.3.11 Hydrodynamic Forces
Simulations were conducted in totally 8
different cases including 2 submarine
velocities (1.201m/s and 1.6309m/s)
and 4 submergence depth (0.5m, 0.845m,
1.0m and infinite) as is given in Table
2.7.10. In every case, both of the linear
interpolation method and the PI
controller method were used to obtain
the self-propulsion point. Table 2.7.10
shows the results of rotating speed (n)
and thrust (T) at the self-propulsion
point in corresponding cases. Obviously
at the same submergence depth, higher
submarine velocity corresponds to
higher rotating speed and thrust. At the
same velocity, deeper submergence
depth corresponds to lower rotating
speed. The results of the linear
interpolation method and the PI controller method have the same trend. There is no significant
difference between them, which proves that the simulations’ accuracy.
2.7.3.3.12 Wave-Making Characteristics
Figure 2.7.15 shows the height of the free surface relative to the initial position under different
depth conditions, that is, the wave height. The same color bar scale is used at the same velocity, which
reflects the wave making characteristics at the free surface. The wave on the free surface resembles
the Kelvin wave pattern well, which consists of transverse wave system perpendicular to the
direction of motion and divergent wave system diagonal to the direction of motion.
Table 2.7.10 The results of mesh dependence validation.
Figure 2.7.14 The details of the mesh in the midship
section
In case 1 and case 5, where the submergence depth is 0.5m, clear Kelvin wave system characteristics
can be observed, especially steep divergent waves. As part of the sail and sailplanes protruding from
the water, the free surface interacts with the hull to form a wave with large amplitude. In case 2 and
6, where the submergence depth increases to 0.845m. Kelvin wave system features become weak
and divergent waves cannot be clearly observed. In case 3 and 7, where the submergence depth
increases to 1.0m. Divergent wave system features become further weaker and the Kelvin angle
decreases. In addition, due to the lower amplitude, there are some clutter wave interferences.
2.7.3.3.13 Flow Field Characteristics
Figure 2.7.16 shows the velocity nephograms at the midship section of the submarine at the velocity
of 1.6309 / at various depths. Color bar scale is represented by dimensionless velocity. When the
free surface exists, the bow flow field gradually diffuses from the front stagnation point of the
submarine to the free surface in a circle, forming a wave crest; The high-velocity flow formed above
the sail and sailplanes diffuses upward and backward to the free surface, forming a wave trough with
large amplitude; The flow behind the sail diffuses to the rear of the submarine and merges with the
flow behind the stern rudders and the flow formed by the propeller rotation, which diffuse upward
to the free surface, forming a wave crest with large amplitude. They correspond to the wave-making
characteristics in section 2.7.3.3.7. Compared the cases (b), (c), (d) with the case (a), it is found that
the flow field below the submarine is similar, while the flow field above it changes greatly. Due to
Bernoulli's principle, the flow velocity increases in the area below the wave trough, forming a high-
speed area. The flow velocity decreases in the area below the wave crest respectively. In addition,
the existence of free surface aggravates the disturbance of the flow field near the propeller, increasing
the wake velocity of the propeller and making the two wake lines generated by the propeller shift
downward.
Figure 2.7.15 The waves on the free surface in different cases
When the submergence depth is shallow, the flow near the sail interacts with the transverse waves
on the free surface, generating divergent waves and other wave systems. When the submergence
depth is deep, while the distance from the free surface is far, the hull can hardly affect the waveform.
Therefore, the transverse waves are the main waveform.
2.7.3.3.14 Vortex Structures
After the analysis of flow field, Q-criterion is used to analyze the vortex structure around the
submarine and propeller. Q-criterion is widely used for discriminating and visualizing vortex tubes.
The basic expression of Q is as follows:
Eq. 2.7.16
Figure 2.7.17 shows the vortex structures visualized by Q-iso-surface under three different
submergence conditions. The Q values of all the conditions are the same. The pressure field function
is used for coloring. In Figure 2.7.17 where the sail and sailplanes protruding from the free surface,
it can be seen that the vortex structure formed behind the sail merges with the free surface, and then
tends to approach the upper surface of the hull. The tip vortex behind the rudders is affected by the
free surface, and the vortex tube becomes longer and thicker. The vorticity on the free surface is high.
In Figure 2.7.17 (b) the tip vortex tube behind the sail tends to approach the free surface. In
Figure 2.7.17 (c) the vortex structure is influenced little by the free surface.
2.7.3.3.15 Conclusions
This study conducted the self-propulsion numerical simulations of Joubert BB2 submarine and
Marine 7371R propeller through both linear interpolation method and PI controller method based
on a commercial software STAR-CCM+. The main findings are described below:
1. The self-propulsion results calculated by the PI-controller method is similar to the results
calculated by the traditional method. With the decrease of the submergence depth, the
rotating speed and corresponding thrust at the self-propulsion points will increase.
Figure 2.7.16 The velocity nephograms at the midship section in different cases
2. The wave-making characteristics on the free surface are similar to Kevin waves. With the
increase of submergence depth, divergent wave features become weaker and only transverse
waves can be observed. Under the same velocity, the case with deeper submergence depth
has the smaller amplitude, while at the same submergence depth, the case with higher
velocity has greater amplitude and longer wavelength. A wave crest appears at the bow, a
wave trough with large amplitude appears at the middle of the hull and a wave crest with
large amplitude appears behind the propeller.
3. The existence of the free surface changes the flow field between the free surface and the
upper surface of the hull. The flow near the sail spread upward to the free surface. The
interaction between the flow field and the free surface aggravates the inhomogeneity of the
wake velocity behind the rudders and the propeller.
4. When the sail protrudes from the free surface, a high vorticity field will be formed on the free
surface around it. The vortex structure formed behind the sail merges with the free surface,
Figure 2.7.17 The vortex structures in different cases
and then tends to approach the upper surface of the hull. When the sail is below the free
surface, the tip vortex behind the sail extends longer and tends to diffuse to the free surface.
This paper presents some basic research results of submarine self-propulsion in straight near the
free surface. In the future, complex maneuverability tests such as steady turning tests can be
investigated as further research.
Acknowledgements
This work was supported by the National Natural Science Foundation of China (52001210, 52131102),
and the National Key Research and Development Program of China (2019YFB1704200), to which the
authors are most grateful. The authors specially thank to Prof. Decheng Wan for his kind suggestions
and supervision.
2.7.3.3.16 References
[1] Feng X, Jiang Q, Miao Q and Kuang X 2002 Journal of Ship Mechanics 02 1-14
[2] Gourlay T and Dawson E 2015 J. Mar. Sci. Appl. 14 215-224
[3] Wang L, Martin J E, Felli M and Carrica P M 2020 Ocean. Eng. 206 107304
[4] Lungu A 2022 Ocean. Eng. 244 110358
[5] Li P, Wang C, Han Y, Kuai Y and Wang S 2021 Chinese Journal of Theoretical and Applied
Mechanics 53(9) 2501-2514
[6] Carrica P M, Kim Y and Martin J E 2019 Ocean. Eng. 183 87-105
[7] Dong K, Wang X, Zhang D, Liu L and Feng D 2022 J. Mar. Sci. Eng. 10(1) 90
[8] Huang F, Meng Q, Cao L and Wan D 2022 Ocean. Eng. 250 111062
[9] Menter F R 1994 AIAA. J. 32(8) 1598-1605
[10] Hirt C W and Nichols B D 1981 J. Comput. Phys. 39(1) 201-225
[11] Yang Q, Wang G, Zhang Z, Feng D and Wang X 2013 Chinese Journal of Ship Research 8(2) 22-27
[12] Kim H, Ranmuthugala D, Leong Z Q and Chin C 2018 Ocean. Eng. 150 102-112
2.8 Eulerian Multiphase Model
While it is rather straightforward to derive the equations of the conservation of mass, momentum
and energy for an arbitrary mixture, no general counterpart of the Navier-Stokes equation for
multiphase flows have been found. Using a proper averaging procedure it is however quite possible
to derive a set of Equations of Multi-Phase Flow which in principle correctly describes the dynamics
of any multiphase system and is subject only to very general assumptions
25
. A direct consequence of
the complexity and diversity of these flows is that the discipline of multiphase fluid dynamics is and
may long remain a prominently experimental branch of fluid mechanics. Preliminary small scale
model testing followed by a trial and error stage with the full scale system is still the only conceivable
solution for many practical engineering problems involving multiphase flows. Inferring the necessary
constitutive relations from measured data and verifying the final results are of vital importance also
within those approaches for which theoretical modeling and subsequent numerical solution is
considered feasible. The six-equations, one pressure model is currently implemented, supplemented
with the High Reynolds number k-ε model for turbulence. A set of distinct mass, momentum and
energy conservation equations is solved for each phase, and the phases are coupled via momentum
and heat transfer terms. The pressure is assumed to be the same in each phase. Sub-models are
provided to describe the interphase exchange terms and close the equations. In the following, we first
present the fundamental equations for generic phase k (where k could be either the continuous or
dispersed phase), before going on to present the models and sub-models which are implemented to
obtain closure. The fundamental equations for the Eulerian two-phase model (i.e., Multiphase VOF)
are:
Eq. 2.8.1
25
Multiphase flow Dynamics, Theory and Numeric.
Eq. 2.8.2
The inter-phase momentum transfer represents the sum of all the forces the phases exert on one
another and satisfies Mc = - Md. The internal forces represent forces within a phase. In the current
form, they are limited to particle-particle interaction forces in the dispersed phase. The derivation
for energy equation and interphase momentum transfer can be applied through CD-adapco®
methodology manual.
A simple example would be modeling of the gravity current where mixing of saltwater and fresh
water. The simulation used 190K cells with a time step 0.002 using PISO algorithms. Figure 2.8.1
shows selected time frame of 10s
26
. Certain statement can be made for simplification of the equation
with regard to the case investigated. For example in gas-particle two-phase flows, when the
concentration of the dispersed phase is low, certain assumptions may be made which simplify
considerably the equations to solve. The gas and particle flows are then linked only via the
interaction terms. One may therefore uncouple the full system of equations into two subsystems: one
for the gas phase, whose homogeneous part reduces to the Euler equations; and a second system for
the particle motion, whose homogeneous part is a degenerate hyperbolic system. The equations
governing the gas phase flow may be solved using a high-resolution scheme, while the equations
describing the motion of the dispersed phase are treated by a donor-cell method using the solution
of a particular Riemann problem. Coupling is then achieved via the right-hand-side terms
27
.
2.8.1 Case Study 3 - Comparison of Eulerian and VOF Models
Authors : Esteban Guerrero, Felipe Muñoz and Nicolás Ratkovich
Title : Comparison Between Eulerian And VOF Models For Two-Phase Flow Assessment In Vertical Pipes
Appeared in : CT&F - Ciencia, Tecnología y Futuro, 7(1), 73 – 84, 2017
Source : Journal of oil, gas and alternative energy sources
Citation : Guerrero, E., Muñoz, F., & Ratkovich, N. (2017). Comparison between eulerian and vof models
for two-phase flow assessment in vertical pipes. Ciencia Tecnologia y Futuro, 7, 73-84.
The appropriate characterization of the two-phase flow has been recently considered as a topic of
interest at industrial level [Guerrero et al. ]
28
. The (CFD) is one of the techniques used for this
26
André Bakker, “Lecture 16 - Free Surface Flows - Applied Computational Fluid Dynamics”, Fluent Inc. (2002).
27
R. Saurel, A. Forestier, D. Veyret And J. C. Loraud, “A Finite Volume Scheme For Two-Phase Compressible
Flows”, International Journal For Numerical Methods In Fluids, Vol. 18, 803-819 (1994).
28
Guerrero, Esteban. Muñoz, Felipe. Ratkovich, Nicolas. (2017). Comparison between Eulerian and VOF models
for two-phase flow assessment in vertical pipes. CT&F - Ciencia, Tecnología y Futuro, 7(1), 73 – 84.
Figure 2.8.1 Mixing of Brine(Salt Water) with Fresh Water
analysis. Commonly, the Volume Of Fluid (VOF) model and the Eulerian model are used to model
the two-phase flow. The mathematical formulations of these models cause differences in their
convergence, computational time and accuracy. This article describes the differences between these
two models for applications in the two-phase upward-flow. In order to accomplish this objective, the
CFD models were validated with experimental results. This study modeled six experiments with an
orthogonal grid. As a result, the Eulerian model shows mean square errors (13.86%) lower than the
VOF model (19.04%) for low void fraction flows (< 0.25). Furthermore, it was demonstrated that
Eulerian model performance is independent from grid, spending less computational time than the
VOF model. Finally, it was determined that only the VOF model predicts the pattern flow.
2.8.1.1 Introduction & Literature Survey
The multiphase flow, specifically the gas-liquid two phase flow, is an operating condition found in
different types of industries. It appears in systems of energy generation, mass transportation, heat
transfer, equipment for separation and reaction processes, and equipment for environmental control
[Ishii & Hibiki, 2011]. The nuclear and petroleum industries mainly work with the gas-liquid two-
phase flow in their processes. The former, works with this phenomenon in the boiling water or
pressurized water nuclear reactors used for the generation of electrical power. The latter, confronts
the multiphase flow during oil and gas production in vertical, horizontal and inclined pipes.
Furthermore, the two-phase flow appears when well production is enhanced by steam, water or gas
injection [Zhang, Wang, Sarica & Brill, 2003]. As a consequence, the correctly operation of these
processes is fixed to the variables that describe the gas-liquid two-phase flow.
The variation in the volume fractions of the two-phase flow varies from a discontinuous production
to a shutdown of the process (Abdulkadir, 2011). For that reason, characterization of the gas-liquid
two-phase flow is essential to avoid operating problems.
Different techniques are used to determine the gas-liquid two-phase flow. Experimental methods
measure important parameters like local void fraction, bubble size and phase velocities. However,
every instrument has advantages and disadvantages in their cost, intrusiveness and resolution (Da
Silva, 2008).
There is no a cheap non-intrusive multiphase measuring instrument giving the best resolution
(Sharaf et al., 2011). Other predictive methods are the empirical and semi-empirical correlations.
[Woldesemayat and Ghajar (2008)] listed and compared 68 void fraction correlations. Nevertheless,
all these correlations were formulated for specific flow patterns, inclinations and operating
conditions. As a consequence, the two-phase flow models present incorrect predictions when they
are extrapolated. Finally, Computational Fluid Dynamic (CFD) is a useful technique to predict the
two-phase flow behavior under any condition.
The CFD (model) is capable of simulating the two-phase flow by using different physical models.
[Wachem & Almstedt (2003)] conducted a review of the mathematical formulation for CFD models
to predict the behavior of the fluid-fluid flow and solid-fluid flow. For the liquid-gas two-phase flow,
researches mainly used the Eulerian model (Krishna, Urseanu, van Baten & Ellenberger, 1999; Ahmai
& Al-Makky, 2014; Shang, 2015) or the Volume of Fluid (VOF) model which is an Eulerian approach
(Anglart & Podowski, 2001; Fang, David, Rogacs & Goodson, 2010; Abdulkadir, 2011). Additionally,
vertical flows have been analyzed using both CFD models (Abdulkadir, 2011; Shang, 2015).
Nevertheless, these researches did not stablish a selection criterion for both models.
This study demonstrates the differences between the Eulerian model and the VOF model for the two-
phase flow assessment in vertical pipes. Models comparison will analyze accuracy, distinguishable
phases and computational performance. Finally, it proposes an innovative criteria for the selection
of the multiphase flow model on CFD simulations.
2.8.1.2 Theoretical Frame
The analyses of the CFD results take into account the hydrodynamic of the two-phase flow. The
previous behavior is called the flow patterns. This section explains the possible flow patterns that
are acquired in a vertical pipe configuration at different phase velocities. Furthermore, the analysis
is easier if Eulerian and VOF models differences are understood, as shown in the mathematical
formulation for each model.
2.8.1.2.1 Flow Patterns
The phase configurations in vertical pipes are: bubbly flow, slug flow, churn flow, annular flow and
mist flow. Previously these are listed from low velocity to high velocity. Moreover, an increase in the
gas flow is one of the ways that transitions between patterns occur. By increasing gas velocity in a
bubbly flow, small bubbles coalesce to form the Taylor bubbles in slug flow. Churn flow is an instable
slug flow resulting from raising the gas velocity. Annular flow appears when gas flow increases,
creating an interface stress larger than the effects of gravity. As a consequence, liquid phase is thrown
out of the center of the pipe [Thome, 2004].
The flow pattern appearances are shown in Figure 2.8.2 (a) mist flow has the same configuration
as a bubbly flow except that their phases are inverted [Abdulkadir, 2011]. Transport mechanisms are
different in pipes with diameters longer than 50 mm. Consequently, different flow regimes appear
[Sharaf & Luna-Ortiz, 2014]. Hence, the pipe diameters modeled in this study are about 50 mm.
Furthermore, a flow pattern map for upward flow in a 50 mm diameter tube is used to predict flow
patterns [Hewitt, Delhaye & Zuber, 1986]. Figure 2.8.3 shows the map mentioned before.
Figure 2.8.2 Flow patterns in vertical pipes. a) Bubbly & mist flow. b) Slug flow. c) Churn flow. d)
Annular flow. Source: (Bratland, 2010).
2.8.1.2.2 Mathematical Models
The gas-liquid two-phase flow involves transport of momentum, mass and heat. Nevertheless, heat
transfer is omitted, setting the assumption that temperature is constant and uniform in the whole
pipe. Hence, Eulerian and VOF models only consider mass and momentum transfers. The
mathematical formulation for both physic models are detailed in this section.
2.8.1.2.3 Eulerian Model
This method analyzes each phase using one equation for each transport phenomenon. Eq. 2.8.3
show the conservation of mass and momentum for phase i (Siemens, 2014).
Eq. 2.8.3
Additionally, the Eq. 2.8.4 must be achieved. For the previous equations α is the void fraction, u is
the superficial velocity, g is the gravity, P is the pressure, τ is the molecular stress, τt is the turbulent
stress, ρ is the density and Mi represents the momentum transfer in the interface. Furthermore,
Eulerian model requires specifying the bubble´s gas size. Therefore, the discontinuous phase solution
is an agglomerate of these bubbles [Siemens, 2014].
Figure 2.8.3 Experimental conditions plotted on Hewitt et al. (1986) flow pattern map
Eq. 2.8.4
2.8.1.2.4 VOF Model
As a difference, this method analyzes all phases using a unique equation for each transport
phenomenon. Eq. 2.8.5 show the conservation of mass and momentum respectively (Abdulkadir,
2011) :
Eq. 2.8.5
Density and viscosity are calculated as a function of the volume fraction, as shown in the Eq. 2.8.6,
Eq. 2.8.6
The VOF model adds an additional equation solving the interfaces. It uses a continuity equation as a
function of the volume fractions as shown in the Eq. 2.8.7. Consequently, this method does not
require specifying the bubble gas size [Abdulkadir, 2011]:
Eq. 2.8.7
Differences between both models enable simulations with different accuracy, distinguishable phases
and computational performance. Therefore, a methodology is established to study this problem.
2.8.1.2.5 Turbulence Model
The gas-liquid two-phase flow has a turbulent dynamic which has to be taking account in the CFD
models. In this research, the k-ε turbulence model was used to close the consecutive equations for
both models. Eq. 2.8.8 show the PDE equations describing this model [Sadrehaghighi, I.]
29
:
Eq. 2.8.8
The new two variables correspond to the turbulent kinetic energy (k) and the dissipation rate (ε).
The constants values of σε, σk, C1 and C2 are 1.2, 1.0, 1.44 and 1.9, respectively. Finally, the turbulence
effect on the viscosity (turbulent viscosity, μt ) has to be involved in the conservative equations using
29
Sadrehaghighi, I., “Turbulence Modeling – A review”, Patch 1.87.1.
the effective viscosity (μeff) as shown in the Eq. 2.8.9.
Eq. 2.8.9
2.8.1.2.6 Methodology
This section describes the modeling study procedure. First, the test matrix and facilities geometries
are presented. Second, it explains the mesh generation and selection criterion. Finally, the time-step
is selected by the Courant-Friedrich-Lévy condition (CFL criterion).
2.8.1.2.7 Test Matrix
The CFD models performance in the two-phase flow assessment were validated by experimental
results. Data was obtained by different authors: [Sun et al. (2004), Krepper, Lucas & Prasser (2005)
and Westende (2008)]. Experiments were replicated using the CFD software STAR-CCM+ v9.02 from
Siemens. Operating conditions and facilities geometries are described in Table 2.8.1, where ui is the
superficial velocity of phase i, z is the pipe height and z/D describes the measurement tool location
in the pipe. Each studied case was developed at atmospheric pressure.
Figure 2.8.3 shows the experimental conditions plotted on [Hewitt et al. (1986)] flow pattern map.
The study cases location on Figure
2.8.3 predicted that the experimental
data is the bubbly flow and the annular
flow. Therefore, this project studied the
two-phase flow with low and high void
fractions. The CFD prediction is used as
the variable average, as the solution
obtains a steady signal.
2.8.1.3 Mesh Generation
The CFD solution method requires a
grid to solve the partial differential
equations of both models. Mesh
dimensions and arrangement may
create a variety of grids for the same
geometry. However, the solution
convergence, accuracy and velocity
depend upon the mesh quality.
Figure 2.8.4 Orthogonal (Butterfly) Mesh
Table 2.8.1 Geometries and Operating Conditions
[Hernandez, Abdulkadir & Azzopardi(2010)] determined that the best mesh distribution for pipes is
the orthogonal grid (also known as butterfly shape gird). Figure 2.8.4 illustrates the grid
distribution mentioned before. The grid presented in Figure 2.8.4 was associated with three
boundary conditions. The inlet and outlet face were modeled with a velocity inlet and outlet pressure
conditions, respectively. The surrounding face used a wall boundary condition. In addition, the mesh
distribution was tested using a grid independence test to remove any mesh dependency in the system
solution.
Two selection criteria were established in the grid independence test: resulting in accuracy and
simulation time. The experiment case D was simulated with four grids that contained 43400, 228780,
312800 and 415140 mesh cells. As Eulerian and VOF models have a different mathematical
formulation, previous tests were carried for each model to have the correct grid distribution for both
models.
2.8.1.4 Stability Criterion
Unsteady simulation was used to model the two phase flow dynamics. Consequently, the model
stability depends strongly upon the time-step established. Convergence problems are present when
the time-step is larger than velocity magnitude. The previous situation provokes the flow going
through a large quantity of cells without solving intermediate points. As a consequence the CFD
software brings up values to the intermediate points without solving the next interactions, in most
of cases creating a diverge system (Abdulkadir, 2011). Due to the previous problem, the time-step is
selected by the CFL criterion which uses the Courant number (C). Where C is the Courant number (≈
0.25), Δt is the time-step and Δx is the mesh cell size in direction of the maximum fluid velocity
component. The velocity uG is calculated by the Drift-Flux model (Ujang et al., 2008) described in Eq.
2.8.10.
Eq. 2.8.10
Where g is gravity, Res
is the Reynolds
number for the liquid
phase and D is the
pipe diameter. Based
on the previous
equations and the
experiments
description, a correct
time-step is calculated
to achieve a stable
simulation.
2.8.1.5 Results and
Analysis
This section describes
the results in two
parts. The first section
exposes the mesh
independence tests
results and describes the grid selected. The second part describes the two CFD models performance.
2.8.1.5.1 Geometry Meshing
Figure 2.8.5 Mesh Independence Test – Experimental And CFD Results
The simulation of the case D experiment was used to carry out the mesh independence test. [Krepper
et al. (2005)] measured the void fraction using a sensor placed at z/D=60 with a flow inlet of ug =0.34
m/s and ul =1.00 m/s. The average void fraction was 0.2618 with a standard deviation of 10%. Results
obtained by the VOF model and the Eulerian model are shown in Figure 2.8.5.
The VOF model in Figure 2.8.5 establishes that increasing the mesh cells number in the grid will
decrease the error between the simulation and the experimental results. When considering the first
selection criterion that
standard deviation is 10
% for the experimental
result, only the grid with
415140 mesh cells could
model the system
correctly. On the other
hand, the Eulerian model
results demonstrate that
resulted accuracy is not
modified by the number
of mesh cells.
Furthermore, these
results show that
simulations with
Eulerian model obtain an
error equal to the
standard deviation of the
experimental results.
The second selection
criterion for the grid is
the simulation time. This
parameter was analyzed
using a one-node of the processor of an Intel® core-i5 computer with 6 GB of memory ram. The
study´s results are shown in Figure 2.8.6.. It is evident that both models require more computer
time if the number of mesh cells increase.
Considering the previous results, the grid selected for the Eulerian model is the mesh with 43400
cells, as it reduces the simulation time without any effect in the accuracy of the results. On the
contrary, the grid selected for the VOF model is the mesh with 415140 cells guaranteeing the
accuracy of good results despite higher simulation time.
The simulation time spent by the Eulerian model and the VOF model is compared in Figure 2.8.6.
The simulation studied requires 62 000 inner interactions to complete the physical time established
by the problem. This test proved that the Eulerian model always requires more simulation time than
the VOF model. The reason for the previous result is that Eulerian model has more equations to solve
than the VOF model. Furthermore, the Eulerian model is capable to predict the variable values in 40
000 inner interactions. However, this new magnitude of interactions also requires more simulation
time than the VOF model.
2.8.1.5.2 Case Studies
Figure 2.8.6 Mesh Independence Test – Simulation Time
The two-phase flow experiments described in Table 2.8.1 were simulated using the Eulerian model
and the VOF model. Table 2.8.2 shows the results for cases A, B, C, and D in which the variable
analyzed is the void fraction. The cases E and F analyzed the total gas velocity and their results are
shown in Table 2.8.2. Additionally, these tables show the experiment results obtained by the
authors and the standard deviation of their experimentation. The simulation results demonstrate
that the Eulerian model and the VOF model can describe correctly the two-phase flow with low void
fractions. This fact is corroborated by the CFD results of cases A, B, C and D which are inside of the
experimented standard deviations. On the contrary, both models showed errors higher than the
standard deviation when simulating flows with higher void fractions.
Error! Reference source not found. shows the void fractions prediction of Eulerian and VOF models
for cases A, B, C and D. The case C result for the VOF model shows an error higher than 30%.
Considering void fraction magnitude, the previous error is strongly significant. Therefore, the two-
phase flow dynamics affects the accuracy of the VOF model. The best model selection criterion is the
relative error which is calculated by the Eq. 2.8.11. By modeling the low void fraction flow, the
Eulerian model shows an error (13.86 %) smaller than the VOF model (19.04 %). Additionally, both
models obtain the same error (≈ 23 %) in the prediction of high void fraction flow.
Eq. 2.8.11
The physical models differ in their mathematical formulation as it was explained in the theoretical
background. This difference causes a distinct solution appearance for both models in spite of the
similar variable values that they obtained in the system´s solution. The VOF model details better the
bubbles in the two-phase flow than the Eulerian model, as shown in Figure 2.8.8. As an explanation,
the VOF model solves the interface by the continuity of the equation as a function of the volume
fraction, Eq. 2.8.8, differentiating phase variables as none of the other equations distinguish phases.
On the contrary, the Eulerian model does not solve the interface between liquid and gas phases. As a
consequence, each cell has an average value for each variable. Hence, the Eulerian model solutions
Table 2.8.2 Results of Cases A, B, C And D Using Eulerian Model And VOF Model
have a uniform color for the void fraction
parameter. Moreover, Figure 2.8.8 shows
that the VOF model is the correct physical
model predicting the flow pattern.
The simulation results have a correct
physical meaning considering that the case
studies are organized in an ascendant
manner according to the void fraction. The
previous fact is corroborated in Figure
2.8.8. Additionally, as it was predicted in
Figure 2.8.3, Eq. 2.8.8 shows that cases A,
B, C, and D have a bubbly flow as the flow
pattern, and cases E and F an annular
pattern. However, the VOF model shows
problems when modelling the liquid film
between the wall and gas flows as caused by
the mesh distribution. It is required to
develop a more fineness mesh near the pipe
wall to obtain this phenomenon.
2.8.1.6 Conclusions
CFD is a method capable to predict the dynamics of the gas-liquid two-phase flow. This project
conducted a comparison between two CFD models in an upward flow. The methods studied are the
Eulerian and VOF models. The first part evaluated the grid-model relations. The results
demonstrated that the Eulerian model performance to predict the void fraction is irrelevant to the
number of mesh cells in the grid. Moreover, the results exposed that Eulerian model requires more
Figure 2.8.7 VOF Model And Eulerian Model
Predictions For Cases A, B, C And D
Figure 2.8.8 Void Fraction For The Cases Studies By VOF Model And Eulerian Model (1.74 M Of Pipe)
simulation time than the VOF model using the same grid. Nonetheless, the Eulerian model would
spent less time if a grid with a low number of mesh cells is used, due to the mesh independency. The
second part assessed the model prediction of the two-phase flow properties. In the bubbly flow, the
Eulerian model is more accurate than VOF model by a difference of 5% in the void fraction prediction.
On the other hand, both models showed problems when simulating the annular flow. Models
accuracy may be increased by coupling new the CFD models. Opposite to the Eulerian model, the VOF
model is capable of distinguishing the discontinuous and continuous phases in the solution
appearance.
Acknowledgements
We would like to express our sincere gratitude to Siemens for all questions solved that supported the
related research.
2.8.1.7 References
Abdulkadir, M. (2011). Experimental and computational fluid dynamics (CFD) studies of gas-liquid
flow in bends. PhD Thesis. University of Nottingham, Nottingham, England.
Ahmai, S. & Al-Makky A. (2014). Simulation of two phase flow in elbow with problem solving.
International Journal of Modern Physics C.
Anglart, H. & Podowski, M. (2001). Mechanistic multidimensional modeling of slug flow- 4th
International Conference on Multiphase Flow.
Bratland, O. (2010). Pipe flow 2. Multi-phase flow assurance.
Chonburi, Tailandia: Dr. Ove Bratland Flow Assurance Consulting. Siemens. (2014). Documentation
for STAR-CCM+. Siemens.
Da Silva, M. (2008). Impedance sensors for fast multiphase flow measurement and imaging. PhD
Thesis. Technischen Universität Dresden.
Fang, C., David, M., Rogacs, A. & Goodson, K. (2010). Volume of fluid simulation of the boiling two-
phase flow in a vapo rventing microchannel. Frontiers in Heat and Mass Transfer.
Hernandez, V., Abdulkadir, M. & Azzopardi, B.J. (2010). Grid generation issues in the CFD modeling
of the two-phase flow in a pipe. Journal of Computational Multiphase Flows, 3(1), 13-26.
Hewitt, G.F., Delhaye, J.M. & Zuber, N. (1986). Multiphase science and technology (Volume 2).
Springer-Verlag, Germany: Berlin. CT&F - Ciencia, Tecnología y Futuro - Vol. 7 Num. 1 Dec. 2017
Ishii, M. & Hibiki, T. (2011). Thermo-fluid dynamics of two phase flow (2nd Ed.). West Lafayette, U.S.A.:
Springer.
Krepper, E., Lucas, D. & Prasser, H. (2005). On the modeling of bubbly flow in vertical pipes. Nuclear
engineering and design, 235, 597-611.
Krishna, R., Urseanu, M., van Baten, J. & Ellenberger, J. (1999). Influence of scale on the
hydrodynamics of bubble columns operating in the churn-turbulent regime: experiments vs. Eulerian
simulations. Chemical Engineering Science. 54, 4903-4911.
Ratkovich, N., Majumder, S.K. and Bentzen, T.R. (2013). Empirical correlations and CFD siulations of
vertical two phase gas-liquid (Newtonian and non-Newtonian) slug flow compared against
experimental data of void fraction. Chemical Engineering Research and Design. 91, 988-998.
Shang, Z. (2015). A novel drag force coefficient model for gas-water two-phase flows under different
flow patterns. Nuclear and Engineering and Design. 288, 208-219
Sharaf, S., Da Silva, M., Hampel, U., Zippe, C., Beyer, M. & Azzopardi, BJ. (2011). Comparison between
wire mesh sensor and gamma densitometry void measurements in two phase flows. Meas. Sci.
Technol. 22(10).
Sharaf, S. & Luna-Ortiz, E. (2014). Comparison between the two-phase models and wire mesh sensor
measurements in medium and large diameter pipes. 14th AIChE Spring Meeting. New Orleans, U.S.A.
Sun, X., Paranjape, S., Kim, S., Ozar, B. & Ishii, M. (2004). Liquid velocity in upward and downward
air-water flows. Annals of Nuclear Energy, 31, 357-373.
Thome, J.R. (2004). Engineering Data book III. Lausanne Switzerland: Wolverine Tube, Inc.
Tkaczyk, P. (2011). CFD simulation of annular flows through bends. PhD Thesis. University of
Nottingham, Nottingham, England.
Ujang, P.M., Pan, L., Manfield, P.D., Lawrence, C.J. & Hewitt, G.F. (2008). Prediction of the translational
velocity of liquid slugs in gas-liquid slug flow using computational fluid dynamics. Multiphase Science
and Technology, 20(1), 25-79.
Van Der Meulen, G.P. (2012). Churn-annular gas-liquid flows in large diameter vertical pipes. PhD
Thesis. University of Nottingham, Nottingham, England.
Wachem, B.G.M. & Almstedt, A.E. (2003). Methods or multiphase computational fluid dynamics.
Chemical Engineering Journal. 96, 81-98.
Westende, J.M.C. (2008). Droplets in annular-dispersed gas-liquid pipe-flows. PhD Thesis. Delft
University of technology, Netherlands.
Woldesemayat, M. & Ghajar, A. (2007). Comparison of void fraction correlations for different flow
patterns in horizontal and upward inclined pipes. International Journal of Multiphase Flow.
Zhang, H.Q., Wang, Q., Sarica, C. & Brill, J. (2003). Unified model for the gas-liquid pipe flow via slug
dynamics-Part 1: Model development. Journal of Energy Resources Technology, 125, 266-273.
2.9 Multiphase Flow Instability Mechanisms
The objective here is to review the main kinds of instabilities occurring in two-phase flows. It
complements previous reviews, putting all two-phase flow instabilities in the same context and
updating the information including coherently the data accumulated in recent years. In the first
section, a description of the main mechanisms involved in the occurrence of two-phase flow
instabilities is made. In order to get a clear picture of the phenomena taking place in two-phase flow
systems it is necessary to introduce some common terms used in this field. The first distinction
should be made between microscopic and macroscopic instabilities. The term microscopic
instabilities is used for the phenomena occurring locally at the liquid–gas interface; for example, the
Helmholtz and Taylor instabilities, bubble collapse, etc. The treatment of this kind of instabilities is
out of the scope of this work. On the other hand, the macroscopic instabilities involve the entire two-
phase flow system. In this review, the main focus is kept on macroscopic phenomena. The most
popular classification, introduced in [Bouré]
30
, divides two-phase flow instabilities in static and
dynamic. In the first case, the threshold of the unstable behavior can be predicted from the steady-
state conservation laws. On the other hand, to describe the behavior of dynamic instabilities it is
necessary to take into account different dynamic effects, such as the propagation time, the inertia,
compressibility, etc. In addition, the term compound instability is normally used when several of the
basic mechanisms, described later, interact with each other
31
.
2.10 3 - Phase Flow
It is possible to have more than one dispersed phase in a continuous phase. For example, certain
regimes of water-oil-gas flow in an oil pipeline may involve both oil droplets and gas bubbles
immersed in a continuous water phase.
2.11 Poly-Dispersed Flow
The above dispersed flow examples assume a single mean particle diameter for the dispersed phases.
Poly-dispersed flows involve dispersed phases of different mean diameters.
2.12 Homogeneous & Inhomogeneous Multiphase Flow
Inhomogeneous multiphase flow refers to the case where separate velocity fields and other relevant
30
J. Bouré, A. Bergles, L. Tong, Review of two-phase flow instabilities, Nucl. Eng. Des. 25 (1973) 165–192.
31
Leonardo Carlos Ruspini, Christian Pablo Marcel, Alejandro Clausse, “Two-phase flow instabilities: A review”,
International Journal of Heat and Mass Transfer 71 (2014) 521–548.
fields exist for each fluid. The pressure field is shared by all fluids. The fluids interact via interphase
transfer terms. The Particle and Mixture Models are both inhomogeneous multiphase models.
Homogeneous multiphase flow is a limiting case of Eulerian-Eulerian multiphase flow where all
fluids share the same velocity fields, as well as other relevant fields such as temperature, turbulence,
etc. The pressure field is also shared by all fluids.
2.13 Multi-Component Multiphase Flow
It is possible to combine the notions of multicomponent and multiphase flows. In this case, more than
one fluid is present, and each such fluid may be a mixture of chemical species mixed at molecular
length scales. An example is air bubbles in water in which ozone gas is dissolved in both the gaseous
and liquid phases. In this case, mass transfer of common species may occur by diffusion across the
phase interface.
2.14 Free Surface Flow
Free Surface flow refers to a multiphase situation where the fluids (commonly water and air) are
separated by a distinct resolvable interface.
2.15 Surface Tension
Surface tension is a force that exists at a free surface interface which acts to minimize the surface
area of the interface. It gives rise to effects such as a pressure discontinuity at the interface and
capillary effects at adhesive walls. To determine significance, first evaluate the Reynolds number.
Then
➢ For Re << 1, evaluate the Capillary number, Ca = μU/σ
➢ For Re >> 1, evaluate the Weber number, We = σ/ρLU2
Surface tension important when We >> 1 or Ca << 1. Surface tension modeled with an additional
source term in momentum equation
32
.
2.16 Mixture Model
Mixture Model is a simplified Eulerian approach for modeling n-phase flows. The simplification is
based on the assumption that the Stokes number is small (particle and primary fluid velocity is nearly
equal in both magnitude and direction). Solves the mixture momentum equation (for mass-averaged
mixture velocity) and prescribes relative velocities to describe the dispersed phases. Interphase
exchange terms depend on relative (slip) velocities which are algebraically determined based on the
assumption that St << 1. This means that phase separation cannot be modeled using the mixture
model. Turbulence and energy equations are also solved for the mixture if required. It solves a
volume fraction transport equation for each secondary phase.
33
2.17 Dispersed Phase Model (DPM)
Trajectories of particles/droplets/bubbles are computed in a Lagrangian frame. Particles can
exchange heat, mass, and momentum with the continuous gas phase. Each trajectory represents a
group of particles of the same initial properties. Particle-particle interactions are neglected.
Turbulent dispersion can be modeled using either stochastic tracking or a “particle cloud” model.
Numerous sub-modeling capabilities are available: Heating/cooling of the discrete phase,
vaporization and boiling of liquid droplets, volatile evolution and char combustion for combusting
particles, Droplet breakup and coalescence using spray models, erosion. For particulate (or particle-
32
André Bakker, “Lecture 16 - Free Surface Flows - Applied Computational Fluid Dynamics”, Fluent Inc. (2002).
33
Associate Professor Britt M. Halvorsen (Dr. Ing) Amaranath S. Kumara,” Computational Fluid Dynamics (CFD)
and Multiphase Flow Modelling”, Telemark University College, PO. Box 203, N-3901, Norway.
like) flow, it is possible to construct methods based on an idea that following each particle of the flow
as they advect in the continuous phase
34
. Here, the particles would represent one phase. This
approach is referred to as the Lagrangian–Eulerian Method, where the continuous phase is
calculated in an Eulerian reference frame. Among these there are three different strategies for
coupling between the phases
35
. In one-way coupling, the only influence is on the particle by the
surrounding fluid. Two-way coupling, the fluid is also influenced by the particle, and in four-way
coupling, particles are also influenced by each other (see Figure 2.2.1).
A different way of modeling dispersed flows is to treat both phases as a continuum. This is generally
referred to as the Eulerian–Eulerian approach or the two-fluid model, as discussed in
36
. In this case
local instantaneous equations of mass, momentum and energy balance for both phases are derived
along with instantaneous jump conditions for interaction between phases. These equations must
then be averaged in a suitable way. A volume concentration or volume fraction function is defined.
Using this approach introduces more unknowns than equations. Hence, it is necessary to use closure
laws. There are two common ways of obtaining these closure laws. The first is obtained by empirical
assumptions. The second type is obtained from Kinetic Theory of Dense Gases. Kinetic theory
describing rough matters or gritty flow has also been used to model dispersed two-phase flow.
Kinetic theory originates from statistic al description of ideal and semi-ideal gases, see
37
. Using this
theory it is possible to describe the behavior of molecules or particles with well-defined properties
and well-defined interactions.
2.18 Porous Bed Model
The porous-bed model predicts flow in channels and cavities much smaller than the mesh. The model
requires that the volume fraction of the continuous phase is given a priori and that the pressure drop
is given by an algebraic model.
2.19 Some Thought in Multiphase CFD for Industrial Processes
CFD is a rapidly evolving discipline oriented on developing computational tools for solving problems
related to transport processes: fluid mechanics, heat and mass transfer, reactive flow, and multiphase
flow, [Eskin and Derksen]30. In narrow terms CFD is the numerical solution of the mass, momentum,
and energy conservation equations with properly defined boundary conditions. Those equations may
be supplemented with (Newtonian or non-Newtonian) constitutive equations and equations of state
for compressible fluids. In broader terms CFD also involves modelling (parameterization) of
phenomena at length and time scales that are too small to be fully resolved computationally; the three
most prominent examples being turbulence, multiple phases flows, and reactive flows. In strongly
turbulent flows, the spectrum of length and time scales is simply too wide to be completely resolved
in a single computation. Models for small-scale turbulence are used to alleviate the computational
burden and make simulations of large-scale industrial turbulent flows possible. Multiphase flows
usually take the form of a continuous phase that carries one or more dispersed phases. The solid
particles, or droplets, or gas bubbles that constitute the dispersed phases are often too small to be
fully resolved; their impact on the macroscopic flow patterns needs to be modelled. A similar multi-
scale issue relates to chemically reacting flow where mixing at the micro (molecular)-scale defines
the rate of chemical reactions.
34
Reynir Leví Guðmundsson, “A numerical study of the two-fluid models for dispersed two-phase flow”, Doctoral
Thesis Stockholm, Sweden 2005.
35
C. Crowe, M. Sommerfeld, and Y. Tsuji. Multiphase Flows with Droplets and Particles. CRC Press, 1998.
36
T.B. Anderson and R. Jackson. A fluid mechanical description of fluidized beds. Industrial & Engineering
Chemistry Fundamental, 6(4):527–539, 1967.
37
S. Chapman and T.G. Cowling. “The Mathematical Theory of Non-Uniform Gases”, Cambridge Univ. Press, 3rd
edition, 1970.
The most important issue in predictive modelling of chemical industrial processes is how to deal with
their multiphase character. Process equipment (chemical reactors, burners, mixers, crystallizers,
hydro and pneumatic conveying pipe lines, fluidized beds, flotation cells) usually operates with
multiple phases, modelling of which is much more complicated than that of a single phase flow. In
dependence on the phases composing the flow system, the geometry of the flow domain and the
process conditions (flow rates, agitation speeds), an abundance of flow regimes and flow phenomena
can be distinguished. Resolving and predicting these in a numerical simulation is a clear and grand
challenge. Key in virtually any simulation effort is to distinguish between the relevant and irrelevant
physics and model what is relevant. Though, general mathematical descriptions of multiphase
processes are known, it is practically impossible to solve all the conservation equations numerically
without simplifications. There are the two major groups of approaches, which are currently used in
engineering and science:
➢ Methods based on a simplified model representation of some processes involved in a certain
multiphase system.
➢ Methods of direct numerical simulation.
The simplified model representation focuses on the macroscale processes and global flow patterns,
and uses simplifying assumptions and models to represent micro-scale effects. Direct simulations
aim at fully resolving the micro-scale including the behavior (motion, deformation, breakup,
coalescence, aggregation) of individual dispersed phase particles (solids, droplets, bubbles). Given
the high resolution at the micro-scale, direct simulations are only able to simulate small volumes and
thus need simplifying assumptions regarding the macro-scale, such as homogeneous turbulent
conditions, or simple shear flow.
The first group of methods is usually employed when a computational domain is large and/or a
number of different phenomena revealing themselves on different scales are involved. For example,
a force interaction of dispersed and continuous phases is modelled through a drag force that is
calculated based on empirical correlations. Heat and mass transfer in such a case are also described
by empirical equations. The situation becomes even more complicated when concentration of a
dispersed phase is high. Then dispersed phase components interact with each other. Those
interactions lead to generation of additional stresses in a flow, causing a change in flow pattern. If
particles are solid then kinetic theory of granular media can be employed for modelling dispersed
phase dynamics. Models where both continuous and dispersed phases are represented as two
interacting interpenetrating continua are classified as two-fluid models and often used in
engineering practice. Such models are incorporated into commercial CFD codes (e.g., Fluent and CFX)
and widely used for computing of large-scale technological devices (e.g., fluidized bed chemical
reactors, hydraulic or pneumatic conveying pipelines, etc.).
Alternatively, the equations of motion of the dispersed phase are solved in Lagrangian coordinates.
In this case motion of each particle is tracked. Collisions of a tracked particle with others are
accounted for assuming that it moves through a cloud formed by other particles. It is assumed that
particle–particle collisions are binary and mutual orientations of colliding particles are random. Post-
collision particle velocities are calculated based on momentum conservation for particle pair. This
approach is more accurate than the two-fluid model, but limited to relatively low particle
concentration and computationally expensive. If the second phase is not dispersed down to small size
particles or droplets the two-fluid approach cannot be used. If both phases are immiscible fluids then
dynamics of each fluid is modelled by solving the corresponding conservation equations. The models
for each fluid flow are coupled through no-slip conditions and equality of stress on the fluid/fluid
boundary. That boundary is tracked by one of the known techniques (e.g., volume of fluid method).
The option of computing immiscible fluid flows is provided by modern commercial CFD codes.
Examples of successful application of such an approach are modelling a bubbly flow in a capillary
channel, a liquid film flow on a surface, etc.
Direct Numerical Simulation (DNS) is a direction that is rapidly developing during the last 20 years.
DNS methods suppose solving the conservation equations for all phases composing the system
directly, without introducing simplifying assumptions. For example, in a case of a fluid–solids flow a
dispersed phase is treated as a moving boundary of a complicated changing configuration. There are
a number of different DNS methods. A DNS method is often considered as a technique for solving
problems on the meso-scale that is assumed to be a minimum scale representing an important
property of a flow system. An example of such a property is an apparent viscosity of a slurry or an
emulsion. The meso-scale in this case is a characteristic size of a computational domain that is
sufficient to calculate the apparent viscosity based on accurate modelling of dynamics of interacting
carrying and dispersed phases. A DNS method should not require a model of turbulence, that is, such
a method should allow resolving Navier–Stokes equation from a micro-scale (significantly smaller
than the inner turbulence scale) to a relatively large-scale (e.g., a few percent of a tube radius for a
pipe flow). Some known DNS methods are based on direct solution of the conservation equations for
all components of a given flow system.
Unfortunately, these equations are strongly non-linear and characterized by poor convergence and
numerical stability. The other group of DNS methods is based on ideas borrowed from statistical
mechanics. A fluid is represented as a system of particles, characterized by a probability density in a
6-dimensional space (3 coordinates in the geometrical space and 3 coordinates in the velocity space).
Dynamics of such a system is described by a known Boltzmann equation. It was proven that the
Boltzmann equation can be reduced to the Navier–Stokes equation, therefore the Boltzmann
equation can be used for modelling fluid flows. Examples of methods based on such an approach are:
the Lattice Boltzmann Method (LBM), its predecessor Lattice Gas Automata (LGA), and Dissipative
Particle Dynamics (DPD) approach. LBM and LGA methods employ a fixed grid. The velocity in each
node is discretized to a number of fixed directions. The simplified kinetic equation formulated for
such a grid allows obtaining an approximate solution of the Boltzmann equation and the Navier–
Stokes equation, respectively.
The Lattice–Boltzmann technique can be applied to modelling flows in a domain with very complex
boundary conditions. The LBM equations are free of drawbacks associated with strong nonlinearity
of Navier–Stokes equation. LBM has been successfully used for modelling multiphase flows,
especially on a micro-scale. The DPD is an off-lattice mesoscopic simulation method which involves
a set of particles randomly moving in continuous space. Each particle moves under the action of three
pairwise-additive forces: a conservative force, the dissipative force, and the random force. The DPD
technique has an advantage over other methods when it is necessary to relate the macroscopic non-
Newtonian flow properties of a fluid to its microscopic structure. Though DNS methods are
prospective for accurate modelling of flows on a mesoscopic level their applicability are often limited
to small computational domains. Modern technological equipment is often characterized by
enormous dimensions. DNS methods may serve as an excellent tool for deriving correlations or
models used as sub-models for macro-scale CFD codes.
In an ideal world, micro, meso, and macro-scale simulations are tightly connected to provide a multi-
scale approach for truly predictive modelling of large-scale industrial processes. The challenges in
multi-scale modelling are the formulation of generic coarse and fine graining techniques to
meaningfully connect simulations at vastly different length and time scales. The topic of our article
series on CFD of multiphase flow covers given the above considerations a broad spectrum of methods
and applications. The articles presented can be considered as examples of developments and
applications of CFD techniques. Their common theme is solution of engineering problems arising in
process industries. We hope that the series will be interesting for scientists from industry and
academia as well as for practicing engineers involved in simulations of multiphase systems.
3 Multicomponent Flow
3.1 Preliminary
Mass transfer deals with situations in which there is more than one component present in a system;
for instance, situations involving chemical reactions, dissolution, or mixing phenomena
38
. A simple
example of such a Multi-Component
system is a binary (two component)
solution consisting of a solute in an
excess of chemically different solvent. In
a multicomponent system, the velocity
of different components is in general
different. For example, in Figure 3.1.1
pure gas A is present on the left and pure
gas B on the right. When the wall
separating the two gases is removed and
the gases begin to mix, A will flow from
left to right and B from right to left clearly the velocities of A and B will be different. The velocity of
particles (molecules) of component A (relative to the laboratory frame of reference) will be denoted
vA. Then, in this frame of reference, the molar flux NA of species A (units: moles of A/(area time) ) is
Eq. 3.1.1
where cA is the molar concentration of A
(moles of A/volume). This could be used to
calculate how many moles of A flow
through an area Ac per unit time (see
Figure 3.1.2) where the flux is assumed to
be normal to the area Ac. Then the amount
of A carried across the area Ac per unit time
is Amount of A carried through Ac per unit
time = NA AC = cA vA Ac (moles/time). Since
the volume swept out by the flow of A per
unit time equals vA AC (Figure 3.1.2), the
above expression is seen to equal this rate
of volumetric "sweeping" times cA, the
amount of A per volume.
More generally, for arbitrary direction of NA
and a differential area element dB, the rate of A transport through dB would be (see Figure 3.1.2),
flux of A through dB = - cAvA . n dB (moles/time) n is the outward unit normal vector to dB. One can
understand this by realizing that - vA . n dB is the volumetric flowrate of A species (volume/time)
passing across dB from "outside" to "inside", where "outside" is pointed at by the unit normal vector
n. Multiplying the volumetric flowrate -vA . n dB by the number of moles of A per volume, cA, equals
the moles of A passing through dB per unit time. cA is related to the total molar concentration c (c
is moles of particles, irrespective of particle type, per volume) where xA is the mole fraction of A.
Summing over the mole fractions of all species must produce unity (n equals the total number of
different species present in solution). Similarly, we can also define a mass flux of A, nA (units: mass
of A/(area time) ), nA = ρA vA. Here, vA is still the velocity of species A. ρA is the mass concentration of
38
Lecture Notes from CBE 6333, Levicky.
Figure 3.1.1 Binary System of Gases
Figure 3.1.2 Volumetric Flux
A (mass of A per volume of solution).
ρωρω
Eq. 3.1.2
As previously stated, in general each chemical species "i" in a multicomponent mixture has a different
velocity vi. However, it will nevertheless prove convenient to define an average velocity of the bulk
fluid, a velocity that represents an average over all the vi's. In general, three types of average
velocities are employed: mass average velocity v (v is what is usually dealt with in Fluid Mechanics),
molar average velocity V, and volume average velocity vo. We will only deal with the first two
average velocities
ρ
Eq. 3.1.3
Why bother with two different average velocities? The mass average velocity is what is needed in
equations such as the Navier Stokes equations, which deal with momentum, a property that depends
on how much mass is in motion. Thus, the amount of momentum per unit volume of a flowing
multicomponent mixture is ρv ( ρv = mv/Volume, where m is the total mass traveling with velocity v;
m/Volume = ρ); thus momentum must be calculated using the mass average velocity v. Similarly, the
Equation of Continuity expresses conservation of mass, and is similarly written in terms of v. The
physical laws expressed by these equations (conservation of momentum, conservation of mass) do
not depend on the moles of particles involved, but they do depend on the mass of the particles.
On the other hand, when dealing with mass transfer, we will see that it is common to write some of
the basic equations in terms of V as well as v. The reason for using V, in addition to v, is convenience.
For instance, if in a particular problem there is no bulk flow of particles from one location to another
so that, during the mass transfer process the number of particles at each point in space stays the
same, then V = 0. Setting V to zero simplifies the mathematics. Figure 3.1.1 at the beginning
provides an example. Imagine that, in their separated state as drawn, A and B are both ideal gases at
the same pressure p and temperature T. Then, from the ideal gas equation, the molar concentration
of A and B is the same, cA = cB = c = p/RT (R = gas constant). The equality of cA and cB to the total
concentration c is appropriate because the gases are pure; thus in each compartment the
concentration of the gas (A or B) must also equal the total concentration c. After the separating wall
is removed, particles of A and B will mix until a uniform composition is achieved throughout the
vessel. In the final state, assuming the gases remain ideal when mixed, the value of p and T will remain
the same as in the unmixed state and therefore the total concentration c also remains the same, c =
p/RT (p is now the total pressure, a sum of the partial pressures of A and B). Thus, in the final mixed
state, the number of particles per volume c (here a sum of particles of A and B types) is the same as
the number of particles per volume in the initial unmixed state. Thus mixing produced no net transfer
of particles from one side of the vessel to the other, it only mixed the different particle types together.
Under these conditions, when there is not net transfer of particles from one part of a system to
another, V = 0.
In contrast, for the same mixing process, in general v will not be zero. For example, imagine that mass
of A particles is twice as large as that of B particles. Then in the initial unmixed state the left hand
side of the vessel (filled with A) contains more mass, and the density (mass/volume) of the gas A is
higher than that of B even though its concentration (particles/volume) is the same. Once A and B mix,
however, the density everywhere will become uniform. For this uniformity to be achieved mass must
have been transferred from the A side to the B side; therefore, in contrast to the molar average
velocity V, the mass average velocity v was not zero during the mixing process.
3.2 Integral and Differential Balances on
Chemical Species
We will refer to the species under consideration as
species A. Following a derivation that parallels that
employed for the other conservation laws
(divergence theorem), the first step in the derivation
of a conservation law on the amount of species A is to
perform a balance for a closed control volume V'. V' is
enclosed by a closed surface B (Figure 3.1.1). The
amount of species A inside V' can change either due
to convection through the boundary B, or by
generation/consumption of A due to a chemical
reaction. In words, the conservation for species A can
stated as:
Eq. 3.2.1
3.2.1 Molar Basis
An integral molar balance on species A, performed over the control volume V', is written as
Eq. 3.2.2
where n is the outward unit normal vector to surface B, not to be confused with the mass flux ni = ρi
vi of species i. On the left side, cA is concentration of A in moles per volume; thus cAdV' is the number
of moles of A in a differential volume dV'. Integrating (i.e. summing) this term over the entire control
volume V' yields the total number of moles of A in V'; the time derivative of this integral is the rate of
change of moles of A inside V' (units: moles/time). Thus, the left hand term is just the rate of
accumulation of A in V', expressed in
molar units. The accumulation term
equals the rate at which A is
convected into V' (1st term on right)
plus the rate at which A is generated
inside V' by a homogeneous chemical
reaction (2nd term on right). The 2nd
term on the right in Eq. 3.2.2
represents production of A by
homogeneous reactions. A
"homogeneous" reaction is one that
occurs throughout the interior of V'.
In contrast, a heterogeneous
chemical reaction would be one that
occurs only at an interface; for
instance, between a solid and a
Figure 3.2.2 Volume Swept
Figure 3.1.1 Divergence Theorem Applied
to Chemical Species (Same Source)
liquid phase; and is not distributed throughout the entire volume. The molar reaction rate RA has
units of moles/(volume time) and represents the rate at which moles of A are produced or consumed
by all homogeneous reactions. RAdV' is the number of moles of A produced inside a volume element
dV' per unit time (units: moles/time). Summing this production over the entire control volume leads
to the total molar rate of production of A, inside V', due to homogeneous chemical reactions.
Eq. 3.2.2, by assumption, did not include any generation of A due to heterogeneous reactions. Clearly,
if in V' there was a large interface at which a heterogeneous reaction leads to production of A, one
would have to add that term to Eq. 3.2.2. The term would typically have the form of a rate of
production of A per area (moles / (area time)) times the total area of the reacting surface. However,
it may also be that a heterogeneous reaction is actually more conveniently modeled as homogeneous.
Because the reaction occurs only at the interface between a particle and the liquid, it is
heterogeneous. However, since the particles are dispersed throughout V', one could think of the
reaction rate on a per volume basis (i.e. moles produced per volume of solution per time) as opposed
to a per area basis (moles produced per surface area of particles per time).
1. As done previously for the other balances, one can use the Divergence Theorem to convert
the surface integral of the convection term (1st term on right) into a volume integral,
2. Move the d/dt derivative inside the accumulation integral since the integration limits are
time independent (the limits do not depend on time because a fixed control volume is
considered, whose shape and location do not change; this assumption can be relaxed at the
expense of a somewhat more complicated mathematical expression),
3. Combine all terms under a common volume integral to obtain,
Eq. 3.2.3
The only way to ensure that Eq. 3.2.3 evaluates to zero for an arbitrary control volume V' is to
require that
Eq. 3.2.4
The above equation is the differential molar balance on species A. It states that the rate of
accumulation of moles of A at a point in space (left hand side) is equals the rate at which moles of A
are convected into that point (1st term on right), plus the rate at which moles of A are produced at
that point by chemical reactions (2nd term on right). These physical interpretations can be verified
by tracing the origin of the terms back to the corresponding terms in the integral balance, equation.
3.2.2 Mass Basis
Similarly, For mass balance on species A,
Eq. 3.2.5
The differential equation of continuity (total mass balance) derived in fluid mechanics for single
component systems. It also applies to multicomponent systems in which chemical reactions happen.
The prove this is straightforward.
Eq. 3.2.6
This equation states the law of mass conservation in multicomponent systems, even if chemical
reactions are present. The total accumulation of mass at a point (left hand side) can only occur
by convection of mass to that point (right hand side). For multicomponent systems whose
density ρ is constant (i.e. ρ does not vary from point to point irrespective of variations that may
be present in temperature, pressure, or composition).
3.3 Diffusion Fluxes
The diffusion flux of species A is that portion of its total flux that is not attributed to bulk flow (as
represented by the mass or molar average velocities). More precisely, jA, the mass diffusive flux of A,
is defined as
)-(-N
motionbulk todueA offlux molar -A offlux Molar total=
)-(--n
motion bulk todueA offlux mass -A offlux Mass total=
AAAA
A
AAAAAAA
A
VvV
J
vvvvv
j
cc ==
===
Eq. 3.3.1
Thermodynamics also states that, for a system with n components, n + 1 intensive variables are
sufficient to fully specify the equilibrium state. Since binary fluid mixtures are being considered, for
which n = 2, three intensive variables are needed. It will be convenient to choose temperature T,
pressure p, and μT (the chemical potential per mass of species i by μi). In the absence of equilibrium,
one or more of these variables will vary with location in a way that non-equilibrium gradients in ΔT,
Δp, and ΔμT exist. To move toward equilibrium, the system will transfer heat and masses of the
different species around so as to eliminate these gradients. For instance, heat flux will occur from hot
too cold to equalize the temperature, and mass fluxes of individual chemical species will occur so as
to equalize each species' total (μi + yi) potentials. Non-equilibrium pressure gradients can be
normalized by bulk flow of material from high to low pressure regions. One possible way the system
can eliminate non-equilibrium gradients in ΔT, Δp, and ΔμT is by diffusion of the various chemical
species; it is then logical to assume that the diffusive fluxes will be functions of these gradients, with
steeper gradients producing greater fluxes. Let's consider the diffusive mass flux jA, assumed to be a
function of the gradients such that jA = jA(ΔT, Δp, ΔμT). When the gradients ΔT, Δp, and ΔμT are not too
large, one could perform a Taylor series expansion of jA (around equilibrium) in the gradients and
truncate it after the first order terms. Such an expansion would lead to the following mathematical
relation for jA:
Eq. 3.3.2
The proportionality factors Ci are functions of T, p, and ΔT, but not of the non-equilibrium gradients
in these quantities (this is because, recalling Taylor Series expansions, these factors are to be
evaluated at equilibrium, the "point" around which the expansion is being formed. However, at
equilibrium, the non-equilibrium gradients are zero). Eq. 3.3.2 must be constrained to obey
requirements imposed by thermodynamics. In particular, using the second law of thermodynamics,
it can be shown that C3 must equal zero
39
. Therefore, Eq. 3.3.2 simplifies to
Eq. 3.3.3
A species chemical potential, at some point in the mixture, can be viewed as a function of the pressure,
temperature, and composition at that point. For a binary mixture, this means that μA = μA(T, p, ωA)
and μB = μB(T, p, ωA)
40
.
Eq. 3.3.4
If the diffusion coefficient DAB and chemical potentials are known (i.e. from experimental
measurement), C1 can be evaluated. Error! Reference source not found. becomes
Eq. 3.3.5
The product DAB kT is called the thermal diffusion coefficient, kT the thermal diffusion ratio, and
DAB kP may be called the baro-diffusion coefficient. Eq. 3.3.5 shows that diffusive flux of mass of
species A, in a binary solution of A and B, can arise from four different contributions.
3.4 Fick's Law
Having briefly outlined the four causes of mass diffusion spatial variations in composition, external
potential, temperature, and pressure it is useful to highlight the most common scenario in which only
ordinary diffusion is of importance. The discussion will be specialized to binary solutions that obey
Fick's Law. The restriction to binary solutions is not as limiting as it may seem. Indeed, even when
more than two components are present, as long as the solutions are sufficiently dilute the diffusion
of solute species can be modeled as for a binary system. This is because when one of the species (the
solvent) is present in vast excess, with all the rest (the solutes) in trace amounts, the diffusion of each
solute species can be treated as if it was in pure solvent alone. Under these dilute conditions a solute
particle will not "see" any of the other solute particles, and so its diffusion will not be affected by their
presence but only by the solvent. Such a situation is effectively a two component problem, the solute
of interest plus the solvent. Fick's Law can be written in several common forms such as Mass
39
Landau & Lifshitz, Fluid Mechanics, Pergamon Press, pp 187 and 222, 1959.
40
An implicit assumption is being made that thermodynamic relations such as μA = μA(T, p, ωA), which are
strictly applicable to systems at equilibrium, apply even though equilibrium does not exist throughout the
system. Qualitatively, this assumption can be expected to hold over sufficiently short length scales over which
only insignificant variations in temperature, pressure, and composition occur, so that the values of these
quantities are well defined. Since thermodynamic quantities are only needed at a “point” (i.e. over very short
lengths), from a practical perspective this consideration is not limiting. Also, note that ωB is not an independent
thermodynamic variable since, for a binary mixture, ωB = 1 - ωA.
diffusion flux and reference bulk average velocity v, or Molar diffusion flux; reference bulk
average velocity V:
xD c
MM
M
)-(c
ωD ρ )(ρ
AAB
BA
AAAA
AABAAA
−===
−=−=
jVvJ
vvj
Eq. 3.4.1
3.4.1 Species' Balances for Systems Obeying Fick's Law
The differential molar and mass balances on a species, are general in the sense that they are
independent of the number of components present or any models of diffusion. For example, they do
not require ordinary diffusion to obey Fick's Law. These equations are only based on the statement
that the rate at which the amount of A can change at a point in space equals the rate at which A is
convected into that point plus the rate at which it is generated by chemical reactions. However, in
their present form, these equations can be inconvenient because they contain the species' velocity
vA, which must be known in order to accomplish the usual goal of solving for the mass or molar
concentrations. One way to model vA is to consider it as consisting of the two contributions previously
encountered:
1. one due to bulk flow of the fluid mixture (convection)
2. one due to the diffusion of species A (mass diffusion)
Separation of the total flux of A into diffusive and bulk convection contributions is motivated by
convenience. The mass average velocity v is easy to measure, and can be obtained by direct
calculation from the differential equations of fluid mechanics (e.g. Navier Stokes equations for
Newtonian fluids with ρ and μ constant). Typically, the diffusive fluxes are modeled well by Fick's
Law for solutions in which only ordinary diffusion is present and which are either binary or, as
discussed earlier, dilute. Equations can be specialized to fluids that follow Fick's Law as
R.c-x.cD Rc. -.
t
c
:balanceMolar
r.ρρ.-ωD.
t
ρ
: balance Mass
AAAABAA
A
AAAAAB
A
+=+=
+−=
vJ
vv
A
Eq. 3.4.2
Further information can be obtained in handout “Multicomponent Systems”, CBE 6333, [Levicky].
3.5 Case Study - Assessment of an Open-Source Pressure-Based Real Fluid Model
for Trans-critical Jet Flows
Authors : Faniry N.Z. Rahantamialisoa1, Adrian Pandal2, Ningegowda B. M.1, Jacopo Zembi1, Nasrin
Sahranavardfard1, Hrvoje Jasak3, Hong G. Im4, Michele Battistoni1
Affiliation : 1Department of Engineering, Università degli di Studi Perugia, Perugia, Italy
2Departement of Energy, Universidad de Oviedo, Gijon, Spain
3Department of Physics, University of Cambridge, Cambridge, UK
4Clean Combustion Research Center, King Abdullah University of Science and
Technology, Saudi Arabia
Original Publication : ICLASS 2021, DOI: https://doi.org/10.2218/iclass.2021.6040
Conference : 15th Triennial International Conference on Liquid Atomization and Spray Systems,
Edinburgh, UK, 29 Aug. - 2 Sept. 2021
Format : Extracted for Contents
3.5.1 Abstract
Complexity behind physical phenomena of supercritical and trans-critical jet flows, still leaves an
ambiguous understanding of such widespread technology, with applications ranging from diesel and
liquid rocket engines to gas turbines. In this present numerical study, a new open-source CFD model
construction is presented and validated using a liquid-rocket benchmark comprised of liquid-oxygen
(LOX) and gaseous-hydrogen (H2) streams. Mixing process of liquid oxygen hydrogen streams under
liquid rocket engine (LRE) relevant conditions is scrutinized using the pressure-based solution
framework implemented in the versatile computation platform Open-FOAM. The model accounts for
real fluid thermodynamics and transport properties, making use of the cubic Peng-Robinson
equation of state (PR-EOS) and the Chung transport model. The solver capability to capture the
mixing layer between the two separated streams is discussed as well as its capability to predict with
adequate accuracy the thermophysical quantities. Following the thorough validation, a comparison
of the contribution of the accurate laminar transport properties vs. the large eddy simulation (LES)
sub grid scale (SGS) turbulent values is conducted in order to assess the relative importance of the
turbulent viscosity. By means of an assessment of the pressure-based numerical framework with
available data in the literature, this work contributes to a better understanding of well resolved
simulations. In addition, it enables the further development of a real fluid pressure-based multi-
species solver as an open-source code.
3.5.2 Introduction
Modern high-performance propulsion and transportation devices from rocket engines to diesel
engines involve injections occurring at high pressure. For liquid-fueled rocket engines, this translates
to propellants injected at a super- or trans-critical state, i.e., at pressures above the critical pressure
of the fluid and temperatures close to or below the critical temperature. In this context, such
situations come with changes in the physical characteristics and behavior compared to classical sub-
critical injection and fluid properties are highly influenced by changes in temperature. Fluid behavior
deviates from the ideal gas as the assumption of negligible molecule volume does not hold anymore
and also there is a diminution of the surface tension [1]. Besides, as the fluid undergoes the trans
critical path, it crosses the pseudo-boiling line along which some thermodynamic properties (heat
capacity, thermal expansion coefficient, isothermal compressibility) are at their maxima. Hence,
detailed understanding of these complex operating conditions is crucial.
Many theoretical and experimental studies have been conducted over the years regarding high
pressures flows: from Mayer and Tamura [2] that conducted experimental visualizations of
supercritical injection and mixing processes of Liquid Oxygen (LOX) and Gaseous Hydrogen (H2) to
Habiballah et al. [3] and their investigations on the differences of flame structure in sub- and super-
critical regimes with Mascotte benchmark test case. Experiments of a cold supercritical nitrogen jet
that is injected into an ambient temperature nitrogen environment were also conducted by Mayer et
al. [4]. Further experiments regarding inert binary injection and mixing processes were presented by
Oschwald et al. [5].
Both studies underline that the prevailing physical phenomena change when the operating pressure
exceeds the critical point. Even though, those works have allowed to make remarkable progress in
order to gain deeper insight into such complex phenomena, still limited information can be captured
through experiments. This has motivated the growing efforts towards modeling studies of trans-
critical and super-critical flows. Several works have been carried out to mimic Mayer et al.
experiments: like in [6] or in [7] where the role of SGS model were investigated for a jet of cryogenic
nitrogen or in [8] which among their results provides an analysis of the heat transport phenomena
within a three dimensional Direct Numerical Simulation (DNS).
Reitz and co-workers focused on a thermodynamic analysis of the mixtures states [9]. The group of
J. Bellan [10, 11] has extensively studied shear layers in a supercritical environment using both (DNS)
and Large Eddy Simulation (LES). Similar works have also been reported in [12, 13].
On the other hand, numerical studies are also subjected to challenges. The difficulties arise mainly
from real-gas effects that strongly influence these processes, leading to non-linearities of the
thermodynamic system and thereby non-physical oscillations of the pressure which can severely
impact the accuracy. It has been therefore the main focus of many researchers to develop numerical
strategies in order to achieve both stability and accuracy [7, 14–18].
This present study follows previous works carried out in [19] to simulate multicomponent mixture
species spray mixing processes with real-fluid thermophysical properties on both cryogenic and non-
cryogenic fuel injections. However, here the thermophysical models have been modified to
incorporate more convenient mixing rules. It is then one of the main objective of this work to make
further validations of the pressure-based framework with available data in the literature.
In fact, Ruiz et al. [20] provides a comprehensive data set with a benchmark test case at high-
Reynolds-number supercritical flow with large density gradients. The case consists of a two
dimensional DNS of LOX-H2 streams mixing layer separated by an injector lip and is taken up by Ma
et al. in [16] among other test cases to validate the robustness of the proposed entropy stable hybrid
scheme or by Lacaze et al. [17] that reproduce the same configuration to address an extensive
comparison of three numerical approaches based on different formulations of the transported
properties. Furthermore, LES results are also presented in the present numerical study to
characterize the influence of the filtering approach on the mixing prediction and to assess the relative
importance of the turbulent viscosity vs. the real-fluid laminar one.
3.5.3 Case Setup
As aforementioned, the benchmark case proposed in [20] is reproduced in the present work and it is
represented in Figure 3.5.1 with the boundary conditions. Under LRE relevant conditions with a
pressure set at 100 bar, this case is representative of cryogenic coaxial rocket combustor and has
been widely studied [18, 21–24]. An injector lip with a height of h = 0.5 mm separates the two
streams of high speed GH2 in the surroundings and dense LOX in the center. The computational
domain consists of a two
dimensional domain of
15h x 10h where the area
of interest is limited
axially to 10h from the
splitter face and the
remaining region of 5h is
a sponge layer used to
deal with pressure
oscillations eventually
due to the outlet. A grid
convergence study is
shown in [20].
Even though, the mesh
with 250 grid points
along the splitter is
chosen in the reference
work [20], this present
study follows [16, 17] by
adopting a coarser mesh
with a uniform grid
Figure 3.5.1 Schematic of the case geometry and boundary conditions
spacing of ∆x/h = ∆y/h = 100. It has been demonstrated to not having noticeable differences with
respect to the finer meshes presented in [20]. Similarly to [16], this resolution is applied for the
region up to 10h in the x-direction and 1.5h on both sides of the lip center in the y-direction while
the remaining part of the domain is stretched using a factor of 1.02 in the transverse direction. In
addition, the inlet velocities profiles in both streams follow a 1/7 power law. It is noteworthy to
mention that the Reynolds numbers are respectively ReO2 = 50,000 and ReH2 = 200,000 based on the
splitter height and the injections velocities; while the density ratio is on the order of 80. An adiabatic
no-slip wall is applied at the injector lip whereas the top and the bottom are treated as adiabatic slip
walls and a Dirichlet pressure boundary is imposed at the outlet. DNS and LES cases are then
considered in the present study.
3.5.4 Model Description & Governing Equations
The governing equations of a fully conservative homogeneous, multicomponent and compressible
non reacting two phase flow which are the mass, momentum, energy and species conservation
equations, are respectively summarized below:
Eq. 3.5.1
Eq. 3.5.2
Eq. 3.5.3
Eq. 3.5.4
where ρ is the density, U is the velocity vector, p is the pressure, Yi refers to the mass fraction of
species i, Ji is the species diffusion flux of species i, τ is the viscous stress tensor, and q is the heat flux.
The energy equation is expressed in terms of total enthalpy with hT = h+1/2U2. The viscous stresses
are deduced as for the classical compressible Newtonian fluid model. Contributions of the species
diffusion with different enthalpies are neglected when evaluating the heat fluxes using the Fourier’s
law. Mass diffusion fluxes are modeled using Fick’s law.
Note : Sections regarding Thermophysical models, Transport Properties, Turbulence Model and
Implementation, are omitted here. Users are encourage to consult the source (Rahantamialisoa et al.
2021) for those.
3.5.5 Results and Discussion
To assess the simulations results, comparison with those from the conservative approach proposed
in [20] are presented. To recall, Ruiz et al. [20] propose two solvers which are based on conservative
and non-conservative approach. As reported in [20], the steady state is normally reached after 1.25
m/s, the equivalent of 10 flow-through times (10 FTT). Figure 3.5.2 shows the instantaneous flow
fields of axial velocity, transverse velocity, pressure and density. The present numerical solution is
able to capture the three large vortical structures in the velocity fields, expected within x/h = 10, as
well as the steep density gradient. Kelvin-Helmholtz mechanisms generate the initial eddies in the
hydrogen downstream, at the top corner of the lip. These structures with the interfacial instabilities
lead to the larger vortical elements in the oxygen stream. The “comb-like” or “finger-like” structures
that have been described in many experimental studies of trans critical flows under LRE relevant
conditions [2,5,27], are also observed in the density field (see Figure 3.5.2 c).
The contour plots of the temperature field and hydrogen mass fraction along with the corresponding
Figure 3.5.2 Instantaneous fields of axial and transverse velocities, density and pressure for the DNS
case (from top to bottom and from left to right), at 1.25 ms.
Figure 3.5.3 Instantaneous fields of hydrogen mass fractions, temperature and scatter plot of
temperature versus mass-fraction of hydrogen, at 1.25 ms
scatter plot with respect to the hydrogen mass fraction are shown in Figure 3.5.3. Results are in a
good agreement with the simulations presented in [17] for both the energy based (EB) and the
enthalpy based (HB) approaches. Figure 3.5.3 c, in addition to the CFD scatter data, also includes
phase boundaries from off-line vapor-liquid-equilibrium (VLE) calculations and the adiabatic frozen
temperature profile, as references. The comparison clearly shows that, indeed, the oxygen goes
through a trans critical thermodynamic process. Additionally, to make further assessments,
comparison of statistics collected over time for axial velocity, transverse velocity, pressure, density,
temperature, and oxygen mass fraction for both DNS and LES are presented in Figure 3.5.4. These
Mean and root-mean-square statistics (RMS) are obtained after 15 FTT and are taken at various axial
Figure 3.5.4 Transverse cuts of Mean (Top) and RMS (Bottom) axial, transverse velocity, pressure,
density, temperature and oxygen mass fraction
locations, namely at x/h = 1, 3, 5 and 7. Overall, there are good agreements with the general trends
of the reference works [17, 20] like the asymmetry observed in the rms profiles that broaden towards
the hydrogen stream from x/h = 3 to x/h = 7. The mean axial velocity profiles shown in Figure 3.5.5
a are almost identical for the two solvers. However, for the mean transverse velocity profiles, some
discrepancies are noted for both DNS and LES cases compared to the results in [20] at x/h = 1 and 3,
where the transverse velocity is negative due to the recirculation in the wake of the splitter.
Nevertheless, the proposed solver is able to capture the upward velocity on the right side at x/h = 5
as well as the increase of the rms velocity on the oxygen side and its decrease starting at the lip which
indicate the growth of the mixing-layer thickness (Figure 3.5.5 b).
Figure 3.5.6 shows the various contributions to viscosity. Molecular levels, either in DNS or LES,
are clearly very similar (Figure 3.5.6 a- b). In Figure 3.5.6 c high values of modeled turbulent
viscosity in LES are mostly observed in the recirculation zone. This confirms that the mixing
formation is mainly triggered by the development of initial large-scale Kelvin-Helmholtz instabilities.
The impact of the SGS viscosity is mainly located at the interface between the two fluids, while
elsewhere the laminar viscosity obtained through the real-fluid Chung’s correlation plays a major
role also in the LES.
Figure 3.5.5 Influence of SGS modeling on the Reynolds stresses
3.5.6 Conclusions
The ultimate goal of this work was to contribute to a better understanding of high-Reynolds number
supercritical flow with large density gradients. An assessment of the proposed numerical framework
capability to handle such simulation conditions with multi-species and real fluid thermodynamics as
well as quantitative analysis of the impact of the LES approach have been conducted. Overall, there
is a good agreement of the results with the available data in the literature. Besides, no severe pressure
or velocity oscillations were recorded. The filtering approach does not play an important role on the
mean flows; nevertheless differences are visible in the rms profiles, hence second order moments.
This study enables the further development of a real fluid pressure-based multi-species solver as an
open-source code.
Acknowledgements
Authors gratefully acknowledge the support from KAUST, under the CRG grant OSR-2017- CRG6-
3409.03, and the usage of Shaheen HPC facilities.
3.5.7 References
[1] Reid, R. C., Prausnitz, J. M., and Poling, B. E., 1987. “The properties of gases and liquids”.
[2] Mayer, W., and Tamura, H., 1996. “Propellant injection in a liquid oxygen/gaseous hydrogen
rocket engine”. Journal of Propulsion and Power, 12(6), pp. 1137–1147.
[3] Habiballah, M., Orain, M., Grisch, F., Vingert, L., and Gicquel, P., 2006. “Experimental studies of
high-pressure cryogenic flames on the mascotte facility”. Combustion Science and Technology,
178(1-3), pp. 101–128.
[4] Mayer, W., Telaar, J., Branam, R., Schneider, G., and Hussong, J., 2003. “Raman measurements of
cryogenic injection at supercritical pressure”. Heat and Mass Transfer, 39(8), pp. 709–719.
[5] Oschwald, M., Smith, J., Branam, R., Hussong, J., Schik, A., Chehroudi, B., and Talley, D., 2006.
“Injection of fluids into supercritical environments”. Combustion science and technology, 178(1-3),
pp. 49–100.
Figure 3.5.6 Instantaneous fields of molecular (DNS and LES), turbulent and effective viscosity (from
left to right and from top to bottom)
[6] Müller, H., Niedermeier, C. A., Matheis, J., Pfitzner, M., and Hickel, S., 2016. “Large-eddy simulation
of nitrogen injection at trans-and supercritical conditions”. Physics of fluids, 28(1), p. 015102.
[7] Schmitt, T., Selle, L., Ruiz, A., and Cuenot, B., 2010. “Large-eddy simulation of supercritical-
pressure round jets”. AIAA journal, 48(9), pp. 2133–2144.
[8] Ries, F., Obando, P., Shevchuck, I., Janicka, J., and Sadiki, A., 2017. “Numerical analysis of turbulent
flow dynamics and heat transport in a round jet at supercritical conditions”. International Journal of
Heat and Fluid Flow, 66, pp. 172–184.
[9] Qiu, L., and Reitz, R. D., 2015. “An investigation of thermodynamic states during high pressure fuel
injection using equilibrium thermodynamics”. International Journal of Multiphase Flow.
[10] Bellan, J., 2000. “Supercritical (and subcritical) fluid behavior and modeling: drops, streams,
shear and mixing layers, jets and sprays”. Progress in energy and combustion science, 26(4-6).
[11] Masi, E., Bellan, J., Harstad, K. G., and Okong’o, N. A., 2013. “Multi-species turbulent mixing under
supercritical-pressure conditions: modelling, direct numerical simulation and analysis revealing
species spinodal decomposition”. Journal of Fluid Mechanics, 721, pp. 578–626.
[12] Foster, J., and Miller, R. S., 2012. “A priori analysis of subgrid mass diffusion vectors in high
pressure turbulent hydrogen/oxygen reacting shear layer flames”. Physics of Fluids, 24(7).
[13] Matsuyama, S., Shinjo, J., Mizobuchi, Y., and Ogawa, S., 2006. “A numerical investigation on shear
coaxial lox/gh2 jet flame at supercritical pressure”. In 44th AIAA Aerospace Sciences Meeting and
Exhibit, p. 761.
[14] Terashima, H., and Koshi, M., 2012. “Approach for simulating gas–liquid-like flows under
supercritical pressures using a high-order central differencing scheme”. Journal of Computational
Physics, 231(20), pp. 6907–6923.
[15] Jarczyk, M.-M., and Pfitzner, M., 2012. “Large eddy simulation of supercritical nitrogen jets”. In
50th AIAA Aerospace Sciences Meeting including the New Horizons Forum and Aerospace
Exposition, p. 1270.
[16] Ma, P. C., Lv, Y., and Ihme, M., 2017. “An entropy-stable hybrid scheme for simulations of Trans
critical real-fluid flows”. Journal of Computational Physics, 340, pp. 330–357.
[17] Lacaze, G., Schmitt, T., Ruiz, A., and Oefelein, J. C., 2019. “Comparison of energy-, pressure-and
enthalpy-based approaches for modeling supercritical flows”. Computers & Fluids, 181, pp. 35–56.
[18] Oefelein, J. C., and Yang, V., 1998. “Modeling high-pressure mixing and combustion processes in
liquid rocket engines”. Journal of Propulsion and Power, 14(5), pp. 843–857.
[19] Ningegowda, B. M., Rahantamialisoa, F. N. Z., Pandal, A., Jasak, H., Im, H. G., and Battistoni, M.,
2020. “Numerical modeling of trans critical and supercritical fuel injections using a multi-component
two-phase flow model”. Energies, 13(21), p. 5676.
[20] Ruiz, A. M., Lacaze, G., Oefelein, J. C., Mari, R., Cuenot, B., Selle, L., and Poinsot, T., 2016. “Numerical
benchmark for high-Reynolds-number supercritical flows with large density gradients”. AIAA
Journal, 54(5), pp. 1445–1460.
[21] Oefelein, J. C., 2005. “Thermophysical characteristics of shear-coaxial lox–h2 flames at
supercritical pressure”. Proceedings of the Combustion Institute, 30(2), pp. 2929–2937.
[22] Oefelein, J. C., 2006. “Large eddy simulation of turbulent combustion processes in propulsion
and power systems”. Progress in Aerospace Sciences, 42(1), pp. 2–37.
[23] Zong, N., and Yang, V., 2006. “Cryogenic fluid jets and mixing layers in trans critical and
supercritical environments”. Combustion science and technology, 178(1-3), pp. 193–227.
[24] Zong, N., Meng, H., Hsieh, S.-Y., and Yang, V., 2004. “A numerical study of cryogenic fluid injection
and mixing under supercritical conditions”. Physics of fluids, 16(12), pp. 4248– 4261.
[25] Chung, T. H., Ajlan, M., Lee, L. L., and Starling, K. E., 1988. “Generalized multiparameter
correlation for nonpolar and polar fluid transport properties”. Industrial & engineering chemistry
research, 27(4), pp. 671–679.
[26] Ningegowda, B. M., Rahantamialisoa, F., Zembi, J., Pandal, A., Im, H. G., and Battistoni, M., 2020.
Large eddy simulations of supercritical and trans critical jet flows using real fluid thermophysical
properties. Tech. rep., 2020-01-1153 SAE Technical Paper.
[27]Chehroudi, B., 2012. “Recent experimental efforts on high-pressure supercritical injection for
liquid rockets and their implications”. International Journal of Aerospace Engineering, 2012.
4 Multiscale Modeling
Multiscale modeling refers to a style of modeling in which multiple models at different scales are used
simultaneously to describe a system. The different models usually focus on different scales of
resolution. They sometimes originate from physical laws of different nature, for example, one from
continuum mechanics and one from molecular dynamics. In this case, one speaks of multi-physics
modeling even though the terminology might not be fully accurate. The need for multiscale modeling
comes usually from the fact that the available macroscale models are not accurate enough, and the
microscale models are not efficient enough and/or offer too much information. By combining both
viewpoints, one hopes to arrive at a reasonable compromise between accuracy and efficiency. The
subject of multiscale modeling consists of three closely related components: multiscale analysis,
multiscale models and multiscale algorithms. Multiscale analysis tools allow us to understand the
relation between models at different scales of resolutions. Multiscale models allow us to formulate
models that couple together models at different scales. Multiscale algorithms allow us to use
multiscale ideas to design computational algorithms
41
.
4.1 Traditional Approaches to Modeling
Traditional approaches to modeling focus on one scale. Macroscale models require constitutive
relations which are almost always obtained empirically, by guessing. Making the right guess often
requires and represents far-reaching physical insight, as we see from the work of Newton and
Landau, for example. It also means that for complex systems, the guessing game can be quite hard
and less productive, as we have learned from our experience with modeling complex fluids. The other
extreme is to work with a microscale model, such as the first principle of quantum mechanics. As was
declared by Dirac back in 1929, the right physical principle for most of what we are interested in is
already provided by the principles of quantum mechanics, there is no need to look further. There are
no empirical parameters in the quantum many-body problem. We simply have to input the atomic
numbers of all the participating atoms, then we have a complete model which is sufficient for
chemistry, much of physics, material science, biology, etc. Dirac also recognized the daunting
mathematical difficulties with such an approach after all, we are dealing with a quantum many-body
problem. With each additional particle, the dimensionality of the problem is increased by three. For
this reason, direct applications of the first principle are limited to rather simple systems without
much happening at the macroscale. Take for example, the incompressible fluids. The fundamental
laws are simply that of the conservation of mass and momentum, which, after introducing the notion
of stress, can be expressed as follows:
Eq. 4.1.1
where u is the velocity field, ρ is the density of the fluid which is assumed to be constant and τ is the
stress tensor. To close this system of equations, we need an expression for the stress tensor in terms
of the velocity field. Here is where the guessing game begins. The standard approach is to ask: What
is the simplest expression that is consistent with
• symmetry (Galilean, translational/rotational invariance);
• laws of physics, particularly the second law of thermodynamics;
• experimental data.
41
Weinan E and Jianfeng Lu, Scholarpedia, “Multiscale modeling”, 2011.
In this case, Galilean invariance implies that τ does not depend on u . The next simplest thing is to say
that τ is a function (in fact, linear function) of u . This gives us
Eq. 4.1.2
where p is the pressure, μ is the kinematic viscosity coefficient, which in this context is the only
parameter that carries the information specific to the microscopic constituents of the system, I is the
identity tensor. Second law of thermodynamics requires that μ ≥ 0 . Substituting the above expression
for τ into the momentum equation,
we obtain the celebrated Navier-
Stokes equation. Even though the
reasoning that went into the
derivation of the Navier-Stokes
equation is exceedingly simple, the
model itself has proven to be
extremely successful in describing
virtually all phenomena that we
encounter for simple fluids, i.e. fluids
that are made up of molecules with a
simple molecular structure. Partly
for this reason, the same approach
has been followed in modeling
complex fluids, such as polymeric
fluids. Unfortunately the success
there is quite limited. The first
problem is that simplicity is largely lost. In order to model the complex rheological properties of
polymer fluids, one is forced to make more complicated constitutive assumptions with more and
more parameters. The second difficulty is that accuracy is not guaranteed. For polymer fluids we are
often interested in understanding how the conformation of the polymer interacts with the flow. This
kind of information is missing in the kind of empirical approach described above. A more rigorous
approach is to derive the constitutive relation from microscopic models, such as atomistic models,
by taking the hydrodynamic limit. This is an example of the multiscale analysis approach. For simple
fluids, this will result in the same Navier-Stokes equation we derived earlier, now with a formula for
μ in terms of the output from the microscopic model. But for complex fluids, this would result in
rather different kinds of models. This is one of the starting points of multiscale modeling (see Figure
4.1.1).
4.2 Multiscale Modeling
In the multiscale approach, one uses a variety of models at different levels of resolution and
complexity to study one system. The different models are linked together either analytically or
numerically. For example, one may study the mechanical behavior of solids using both the atomistic
and continuum models at the same time, with the constitutive relations needed in the continuum
model computed from the atomistic model. The hope is that by using such a multi-scale (and multi-
physics) approach, one might be able to strike a balance between accuracy (which favors using more
detailed and microscopic models) and feasibility (which favors using less detailed, more macroscopic
models)
42
.
42
It should be noted that this diagram is slightly misleading: Quantum mechanics is valid not just at the
microscale, it also applies at the macroscale; only that much simpler models are already quite sufficient at the
macroscale.
Figure 4.1.1 Illustration of the multi-physics hierarchy
4.2.1 Sequential Multiscale Modeling
In sequential multiscale modeling, one has a macroscale model in which some details of the
constitutive relations are precomputed using microscale models. For example, if the macroscale
model is the gas dynamics equation, then an equation of state is needed. This equation of state can
be precomputed using kinetic theory. When performing molecular dynamics simulation using
empirical potentials, one assumes a functional form of the empirical potential, the parameters in the
potential are precomputed using quantum mechanics. Sequential multiscale modeling is mostly
limited to the case when only a few parameters are passed between the macro and microscale
models. For this reason, it is also called parameter passing. This does not have to be the case
though: It has been demonstrated that constitutive relations which are functions of up to 6 variables
can be effectively precomputed if sparse representations are used.
4.2.2 Concurrent Multiscale Modeling
In concurrent multiscale modeling, the quantities needed in the macroscale model are computed on-
the-fly from the microscale models as the computation proceeds. In this setup, the macro- and micro-
scale models are used concurrently. Take again the example of molecular dynamics. If one wants to
compute the inter-atomic forces from the first principle instead of modeling them empirically, then
it is much more efficient to do this on-the-fly. Precomputing the inter-atomic forces as functions of
the positions of all the atoms in the system is not practical since there are too many independent
variables. On the other hand, in a typical simulation, one only probes an extremely small portion of
the potential energy surface. Concurrent coupling allows one to evaluate these forces at the locations
where they are needed.
4.2.3 Two Types of Multiscale Problems
The first type are problems where some interesting events, such as chemical reactions, singularities
or defects, are happening locally. In this situation, we need to use a microscale model to resolve the
local behavior of these events, and we can use macroscale models elsewhere. The second type are
problems for which some constitutive information is missing in the macroscale model, and coupling
with the microscale model is required in order to supply this missing information. We refer to the
first type as type A problems and the second type as type B problems.
4.2.4 Modeling Approach defined based on Length Scale
Alternatively, another modeling approach is developed which is based length scale on fluid and
particle systems
43
. It was originally presented by Anderson and Jackson
44
. The idea was that
modeling complexity increases as more effects associated with time and length scales are included
in the simulation. Depending on the length scales, various combinations of modeling scales can be
suggested. These are classified as Micro, Meso, and Macro scale models. In a Micro scale model,
trajectories of individual particles are calculated through the equation of particle motion and the fluid
length scale is the same as the particle size or even smaller. At the same time, instantaneous flow
field around individual particles is calculated. In the Meso-Scale Model, both solid and fluid phases
are considered as inter penetrating bands. The conservation equations are solved over a mesh of
cells. The size of the cells is small enough to capture main features of the flow, like bubble motions
and clusters, and large enough (essentially larger than the size of individual particles) to allow
averaging of properties (porosity, interactions, etc.) over the cells. In the Macro Scale Model, the fluid
length scale is in the order of the flow field. This means that motions of the fluid and the assemblage
of particles are treated in one dimension based on overall quantities
45
. It is also possible to develop
43
Coupled CFD-DEM Modeling: Formulation, Implementation and Application to Multiphase Flows, First Edition.
Hamid Reza Norouzi, Reza Zarghami, Rahmat Sotudeh-Gharebagh and Navid Mostoufi. John Wiley & Sons, Ltd.
44
Anderson, T.B. and Jackson, R. (1967),”Fluid mechanical description of fluidized beds. Equations of motion”,
Industrial and Engineering Chemistry Fundamentals, 6(4), 527–539.
45
Tsuji, Y. (2007) Multi‐scale modeling of dense phase gas–particle flow. Chemical Engineering Science.
some intermediate models in which the length scales of fluid and solid phases are different. For
example, the length scale of solid phase can be kept at the Micro Scale while changing the length scale
of fluid phase to meso or macro. Under these conditions, the affective interactions in the larger scale
can be calculated by averaging the information in the smaller scale.
In general, in multi‐scale modeling, the smaller scale model takes into account various interactions
(i.e., fluid–particle, and particle–particle) in detail. These interaction details can be used with some
assumptions and averaging to develop closure laws for calculating the effective interactions (e.g.,
drag force) in the larger scale model
46
. This allows capture of the essential information needed on
the larger scale. Alternatively, calculation of effective interactions can be performed through the local
experimental data, if available. Combination of fluid/particle motion with different modeling scales
can be calculated by averaging the information in the smaller scale can provide different modeling
approaches, as sketched in
Figure 4.2.1 with detailed below.
4.2.4.1 Micro Approach (Fluid–Micro, Particle-Micro)
In this approach, the fluid flow around particles is estimated by the Navier–Stokes equation. Since
the forces acting on particles are calculated by integrating stresses on the surface of the particle, the
empirical correlation for drag and lift forces are not required. This approach is used in cases where
particle inertial force is relatively small (e.g., liquid–particle flow) or the fluid lubricating effect on
particles is rather significant (e.g., dense‐phase liquid–particle flow). A typical example of such an
approach, is the direct numerical simulation–discrete element method (DNS‐DEM).
4.2.4.2 Meso Approach (Fluid–Meso, Particle-Meso)
This is referred to as the two‐fluid model (TFM), in addition to the real fluid, the assemblage of
particles is also considered to be the second continuum phase. The flow field is divided into a number
of small cells to capture motions of both phases, provided that the cell size is larger than the particle
size. The two continuous phases are modeled by applying laws of momentum and mass
conservations in each fluid cell, leading to averaged Navier–Stokes and continuity equations.
Capability of the TFM in capturing the solid phase motion greatly depends on the closure laws used
for this phase. These closure laws always involve some simplifications or are obtained by semi‐
empirical correlations. While this approach is preferred in commercial packages for its
computational simplicity, its effectiveness depends on the constitutive equations and is not easily
applicable to all flow conditions. The TFM has been successfully utilized to obtain the flow behavior
of various non‐reacting and reacting multiphase flows in laboratory, pilot, and industrial scales.
4.2.4.3 Macro Approach (Fluid–Macro, Particle-Macro)
This approach provides a one‐dimensional (1D) description of gas‐particle flows. The main output of
such a model is the pressure drop, which is considered as the sum of pressure drops due to flow of
fluid and particles. Usually, a formula for the single phase flow, such as Darcy–Weisbach equation, is
used for the fluid pressure drop and that of particles is balanced with the fluid drag formula from the
momentum balance. This approach would also allow the calculation of averaged flow properties by
empirical correlations that are essential in design and analysis of industrial processes. A typical
example of such approach, is the two‐phase model (TPM) in fluidization. In this model, conservation
equations are written for bubbles and emulsion, both having the length scale of the system in a
fluidized bed.
4.2.4.4 MacroMicro Approach (Fluid–Macro, Particle-Micro)
In this approach, shown in
46
Van der Hoef, M., Ye, M., van Sint Annaland, M., Andrews, A., Sundaresan, S., and Kuipers, J. ,”Multiscale
modeling of gas‐fluidized beds”, Advances in Chemical Engineering, 31, 65–149, 2006.
Figure 4.2.1 by 1D‐DEM, the fluid forces acting on particles are calculated from empirical
correlations (e.g., drag and lift) while translational and rotational motions of particles are described
based on Newton’s and Euler’s second laws. At very low concentration of particles, effect of particles
on the fluid motion can be neglected. However, at higher concentrations, closure laws should be
modified to account for the closeness of surrounding particles. Generally, in this approach the flow
field, which is considered to change in one dimension, is not divided into cells and additional pressure
drop is taken into account to reflect the effect of particles on the fluid motion.
4.2.4.5 MesoMicro Approach (Fluid–Meso, Particle-Micro)
In this method, referred to as CFDDEM and shown in
Figure 4.2.1, the flow field is divided into cells with a size larger than the particle size but still less
than the flow field. Effect of motion of particles on the flow of fluid is considered by the volume
fraction of each phase and momentum exchange through the drag force.
For example, an animation by [Oleh Baran], the Product Manager at Siemens Digital Industries
Software, demos the results of modeling of sand-water slurry flow through the horizontal elbow pipe,
where features of Sim-center STAR-CCM+. In this example, DEM non-spherical particles are
interacting with Eulerian multiphase, which uses the Volume of Fluid (VOF) method for resolving
the interface between water and air. As slurry front advances through the pipe with originally
coarser mesh, the number of cells increases because Adaptive Mesh Refinement (AMR) automatically
refines the mesh near the VOF surface. The convergence and robustness of this model with 2-way
DEM-CFD coupling is maintained with the help of the source smoothing model using an upgraded cell
clustering algorithm. Finally, the Archard wear model is used to estimate erosion of the pipe due to
Figure 4.2.1 Modeling Scales in Fluid-Particle Systems
CFD - DEM
1-D DEM
Length Scale
the impacts of sand particles. The morphing velocity of the boundary is a function of the erosion
model output. The postprocessing includes monitoring mesh morphed displacement (or erosion
depth) across the surface of the pipe.
4.2.5 Block-Spectral Method of Solution
The traditional treatment of this kind of problems would be to use empirically based models to count
for the effects of the small scale features and to solve an up-scaled problem on a coarse mesh
47
. The
generality of the solutions following this kind of approaches are of course limited by the very
empirical nature of these fine-scale models. Here we are interested in developing a new multi-scale
methodology, called ‘Block-Spectral Method’. The main intended attribute of the new approach is
that the same numerical discretization scheme and integration method are used for both the coarse
(macro) and fine (micro) scales, so that the numerical resolution is consistently and completely
dictated by the mesh scales. A blocking of the fine resolution domain is introduced to facilitate the
two basic but competing requirements:
• high resolution for fine scale flow features;
• avoidance of having to have fine meshes for a large domain
The block spectral approach can be simply illustrated by comparing a direct solution and a block
spectral solution. The method has been shown to lead to a significant gain in solving micro-scale
problems (up to 102 reduction of degrees of freedom). An important perspective is that the
methodology would enable to resolve the kind of the micro-scale problems currently intractable [L.
He]
48
-
49
.
47
“Osney Thermo-Fluids Laboratory “, University of Oxford.
48
He L, “Block-spectral Mapping for Multi-scale Solution”, Journal of Computational Physics, Vol.250, 2013.
49
He L, “Block-spectral Approach to Film-cooling Modelling”, Journal of Turbomachinery, Vol.134, 2012.
5 Case Studies for Composite Fluid
5.1 Case Study 1 - Liquid-Particle Suspension
Consider a binary system of solid particles suspended in a Newtonian liquid. We denote the
continuous fluid phase by subscript c and the dispersed particle phase by subscript d. We assume
that both phases are incompressible, that the suspension is non-reactive, i.e., there is no mass transfer
between the two phases, and that surface tension between solid and liquid is negligible. Both the
densities ρc and ρd are thus constants, and
0
0ΓΓ
dc
dc
=+
==
MM
Eq. 5.1.1
The mutual momentum equation can now be written as
n
ˆ
n
ˆ
n
ˆ
and AAA and M M M cddcdc −====−=
Eq. 5.1.2
5.2 Case Study 2 - Two Fluid Flow
Starting from a literature search, customizing the model adding specific constitutive equations and
boundary conditions. The results in terms of both concentration distribution and pressure gradient
were compared to experimental data available in literature
50
-
51
-
52
, over a wide range of operating
conditions: average solids concentration between 10% and 40% by volume; uniform particle size
between 90 and 520 μm; slurry velocities between 1 m/s and 5.5 m/s; and pipe diameters between
50 and 150 mm. The Two-Fluid model was obtained by adding the following two features to the
original model, necessary to correctly reproduce the flow:
5.2.1 Mixture Viscosity
A correlation for the viscosity of the mixture, used to define the particle Reynolds number, is
implemented. Among the different expressions available in literature, use is made of that of Mooney,
which best fits the experimental data
/αα1
ηα
expνρμ
pmp
p
c1,cm
−
=
Eq. 5.2.1
in which μ is the intrinsic viscosity, taken equal to 2.5 as suggested for spherical particles; αm is the
maximum packing concentration, taken as 0.7; ρc is the density of the carrier fluid phase; ν1,c and is
the laminar kinematic viscosity of the carrier fluid phase.
5.2.2 Drag force
The drag force law is related to the particle Reynolds number according to the Standard Drag Law
correlation, but the particle Reynolds number is defined with respect to the viscosity of the mixture
instead of that of the carrier fluid phase; therefore, where and are the particle diameter and the slip
50
Pipeline Flow Using ANSYS-CFX. Ind. Eng. Chem. Res. 48(17), 8159-8171.
51
Roco, M.C., Shook, C.A., ”Modeling of Slurry Flow: The Effect of Particle Size”, Canadian J. Chem. Eng. 1983.
52
Gillies, R.G., Shook, C.A., Xu, J., ”Modelling Heterogeneous Slurry Flow at High Velocities”, Canadian J. Chem.
Eng. 82(5), 1060-1065-2004.
velocity vector respectively. This modification is necessary to describe the phenomenon whenever
in some cells the solid volume fraction approaches the maximum packing one. At the pipe wall, no
slip conditions are imposed to the carrier fluid phase, and a logarithmic law wall function is applied
in the near wall-region. The proper wall boundary conditions for the solid phase are still a matter of
discussion in literature. Two alternatives have been considered. At first, a zero-flux condition is
applied to the particles. Afterwards, to account for particle-particle and particle-wall interactions, a
Bagnold-type shear stress is imposed. In particular, the following term, derived from the model of
[Shook and Bartosik]
53
, is introduced in the momentum equation of the particle phase:
vρ
τ
1
α
α
dρ
Re
8.3018
τ
2
c1,c
cw,
1.5
1/3
p
pm
2
pp
2.317
B
−
=
−
Eq. 5.2.2
Which Re = dpUs/ν1, c is the bulk Reynolds
number, defined with respect to the pipe
diameter dp and the slurry bulk-mean
velocity Us; ρp is the density of the
particles; τ w, c is the wall shear stress of
the liquid phase. Figure 5.2.1
demonstrates the geometry of the problem;
the computational domain covers only half
of the pipe section due to a substantial
symmetry of the phenomenon. A fully-
developed turbulent flow profile is applied
at the inlet. No slip is assumed between the
phases. The inlet volume fraction of the
solids is taken as uniform. At the outlet, the
normal gradients of all variables and the
value of the pressure are set to zero. The
length of the computational domain, equal to 100 pipe diameters, is sufficient to ensure the reaching
of fully-developed flow conditions. When imposing a zero-flux condition at the wall to the particle
phase, the predictions of the Two- Fluid model show good agreement to the experimental evidence
in terms of solid volume fraction distribution. As an example, Figure 5.2.2 reports the results for the
flow conditions considered by [Gillies]
54
i.e., and mean solid volume fraction from 12% to 41%. The
contour plots of Figure 5.2.1 highlight
the gradual accumulation of the
particles as the mean solid volume
fraction increases, phenomenon that
can be correctly reproduced applying
the above mentioned modifications to
the original model. The solid volume
fraction profiles along the vertical
diameter (AB in Figure 5.2.2) appear
in quantitative agreement to the
experimental data.
53
Shook, C.A., Bartosik, A.S.,”Particle-wall stresses in vertical slurry flows”, Power Tech. 81(2), 117-124, 1994.
54
Gillies, R.G., Shook, C.A., Xu, J., ”Modelling Heterogeneous Slurry Flow at High Velocities”, Canadian J. Chem.
Eng., 2004.
Figure 5.2.1 Contour plots for particle volume
fraction
Figure 5.2.2 Sketch of the problem
5.3 Case Study 3 - Unsteady MHD Two Phase Flow of Fluid-Particle Suspension
Between Two Concentric Cylinders
The problem of two-phase unsteady Magneto-Hydro-dynamic (MHD) flow between two concentric
cylinders of infinite length has been analyzed by [Jha & Aperea]
55
when the outer cylinder is
impulsively started. The system of partial differential equations describing the flow problem is
formulated taking the viscosity of the particle phase into consideration. Unified closed form
expressions are obtained for the velocities and the skin frictions for both cases of the applied
magnetic field being fixed to either the fluid or the moving outer cylinder.
5.3.1 Literature Survey and Background
The study of fluid/particle mixture is important in petroleum transport, powder technology,
fluidization transport of solid particles by a liquid and liquid slurries in chemical and nuclear
processing and metalized liquid fuel slurries for rocketry. Its relevance is also seen in the field of
mining, agriculture and food technologies. The flow of an electrically conducting fluid through a
channel or a circular pipe in the presence of a transverse magnetic field is encountered in a variety
of applications such as magneto-hydrodynamic (MHD) generators, pumps, accelerators, and flow
meters. The annular geometry is widely employed in the gas cooled nuclear reactors in which the
cylindrical fissionable fuel elements are placed axially in vertical coolants channel within the graphite
moderators and the cooling gas is flowing along the channel parallel to the fuel elements and also in
drilling operation of oil and gas well. [Makinde]
56
studied the steady, axisymmetric, MHD flow of a
viscous, Newtonian, incompressible, electrically conducting fluid through an isotropic, homogenous
porous medium located in the annular zone between two concentric rotating cylinders in the
presence of a radial magnetic field. The unsteady hydro magnetic Generalized Couette flow and heat
transfer characteristics of a reactive variable viscosity incompressible electrically conducting third
grade fluid in a channel with asymmetric convective cooling at the walls in the presence of uniform
transverse magnetic field was also investigated. The high possibility of particle entrainment in these
flows made the formulation of the equation of motion for a two-phase fluid/particle system a
necessity in order to understand the role of particles on the flow. [Saffman]
57
observed the effect of
dust particles on the laminar flow of an incompressible fluid with mass concentration of dust
particles. The equations he obtained neglected the interaction between the individual dust particles
and also assumed that in the continuum hypothesis, the cloud of dust particles form a pseudo-fluid.
Using Saffman’s model, [Nag et al.]
58
studied the Coquette flow of a dusty gas between two parallel
infinite plates for both the impulsive and the accelerated start of one of the plates. [Singh and Dube]
59
studied the laminar flow of an unsteady, incompressible viscous fluid with uniform distribution of
dust particles through a circular pipe under the influence of pressure gradient.
All of these studies excluded the particle-phase viscous effects. However, [Rahmatulin]
60
developed
a model which examines the unstable movement of the interface between the fluid and the particles
and thereby included the particle-phase viscosity term in his model. In this model, each phase of the
suspension has a local velocity and material properties, also, the phases are assumed to interact
mutually in a continuous manner and the phases are homogeneous and evenly distributed per unit
55
Basant K. Jha and Clement A. Aperea, “Unsteady MHD two-phase Coquette flow of fluid-particle suspension in
an annulus”, Published by the AIP Publishing LLC, 2011.
56
O. D. Makinde, O. A. B´eg, and H. S. Takhar, “Magneto-hydrodynamic viscous flow in a porous medium cylindrical
annulus with an applied radial magnetic field,” Int. J. Appl. Math. and Mech. 5, 68–81 (2009).
57
P. G. Saffman, “On the stability of laminar flow of a dusty gas,” J. Fluid Mech. 13, 120–128 (1962).
58
S. K. Nag, R. N. Jana, and N. Datta, “Couettte flow of a dusty gas,” Acta Mech 33, 179–187 (1979).
59
J. Singh and S. N. Dube, “Unsteady flow of a dusty fluid through a circular pipe,” Indian J. Pure Appl. M, (1973).
60
H. A. Rahmatulin, “Osnovi gidrodinamiki vzaimopronikayu¸sih dvijeniy,” Prikladnaya Matematika i Makanika
20, 56–65, (1956).
volume of the mixture. The following partial differential equations describes the unstable movements
of the two-phase incompressible fluids for a plane channel geometry according to Rahmatulin.
Eq. 5.3.1
where K , f are described by
61
and subscript 1 and 2 denote each streams. The problem is solved using
a combination of the Laplace transform technique, D’ Alemberts and the Riemann-Sum
approximation methods. The solution obtained is validated by comparisons with the closed form
solutions obtained for the steady states which has been derived separately. The governing equations
are also solved using the implicit finite difference method to verify the present proposed method.
The variation of the velocity and the skin friction with the dimensionless parameters occurring in the
problem are illustrated graphically and discussed for both phases. The flow of an electrically
conducting fluid through a channel or a circular pipe in the presence of a transverse magnetic field is
encountered in a variety of applications such as Magneto-Hydro-Dynamic (MHD) generators,
pumps, accelerators, and flow meters. The annular geometry is widely employed in the gas cooled
nuclear reactors in which the cylindrical fissionable fuel elements are placed axially in vertical
coolants channel within the graphite moderators and the cooling gas is flowing along the channel
parallel to the fuel elements
62
, as well as in drilling operation of oil and gas well.
5.3.2 Mathematical Formulation
Consider the motion of an unsteady, laminar, viscous fluid/particle suspension between two
concentric cylinders of infinite length. The fluid phase is assumed to be electrically conducting, while
the particles are assumed to be electrically non-conducting. The z-axis is assumed to be on the axis
of the cylinders in the horizontal direction and r´ is on the radial direction. The fluid-particle
suspension exists in the region a ≤ r´ ≤ b between the two cylinders in the presence of magnetic field
acting perpendicular to the flow direction, where a and b are the radii of the inner and the outer
cylinders respectively. Initially, the fluid, the particles and the two cylinders were at rest. However,
when t > 0, the outer cylinder begins to move in its own plane with a velocity Ut´n, where U is a
constant and the inner cylinder remains at rest. Since the cylinders are of infinite length and the flow
is time dependent fully developed one-dimensional flow, all physical variables are functions of r´ and
t´. The magnetic Reynolds number is assumed to be small so that the induced magnetic field and the
Hall effects of MHD are negligible. No applied, polarization voltage exists (Ē = 0) i.e. no energy is being
added or subtracted from the system
63
. It is further assumed that the fluid and the particles are
interacting as a continuum. Figure 5.3.1 for the schematic diagram of the problem. Under the
assumptions made in the present problem and a cylindrical geometry, the equation of motion for the
problem is
61
Basant K. Jha and Clement A. Aperea, “Unsteady MHD two-phase Couette flow of fluid-particle suspension in an
annulus”, Published by the AIP Publishing LLC, 2011.
62
S. K. Singh, B. K. Jha, and A. K. Singh, “Natural convection in vertical concentric annuli under a radial magnetic
field,” Heat and Mass Transfer 32, 399–401 (1997).
63
G. Sutton and A. Sherman, Engineering Magneto-hydrodynamics (McGraw-Hill New York, 1965).
)uu(K
r
u
r
1
r
u
f
ρ
μ
t
u
u
ρ
σB
)uu(K
r
u
r
1
r
u
f
ρ
μ
t
u
21
2
2
2
2
2
2
22
1
1
2
0
12
1
2
1
2
1
1
11
−
+
+
=
−
−
+
+
=
Eq. 5.3.2
Where f1 and f2 are substance quantity of mixture in unit volume (f1 + f2 = 1), K´ is dimensionless
interaction coefficient, and subscripts 1 and 2 represents the fluid and the particle respectively. This
equation is valid when the magnetic field is fixed relative to the fluid. If the magnetic field is also
moving with the same velocity as the moving outer cylinder, we must account for the relative motion.
Thus,
=
=
−
−
+
+
=
cylinder moving torealtive fixed is B 1
fluid torealtive fixed is B 0
G e wher
)tUG-u(
ρ
σB
)uu(K
r
u
r
1
r
u
f
t
u
0
0
n
1
1
2
0
12
1
2
1
2
11
1
Eq. 5.3.3
Considering the impulsive motion of the outer cylinder which corresponds to n = 0 and substituting
the dimensionless quantities provided in
64
, the following dimensionless equations result,
64
Basant K. Jha and Clement A. Aperea, “Unsteady MHD two-phase Couette flow of fluid-particle suspension in an
annulus”, Published by the AIP Publishing LLC, 2011.
Figure 5.3.1 Schematic diagram of the problem
0 tand r 1uu
0 tand 1r 0uu
0 tand λr1 0uu :subject to
ν
ν
R and
f
f
R where)uK(u
r
u
r
1
r
u
RR
t
u
G)-(uM)uK(u
r
u
r
1
r
u
t
u
21
21
21
1
2
ν
1
2
f21
1
2
1
2
νf
2
1
2
12
1
2
1
2
1
===
===
==
==−+
+
=
−−+
+
=
Eq. 5.3.4
5.3.3 Analytical Approach
Taking the Laplace transform, we have the following ordinary differential equations. We choose the
D’Alembert’s method to obtain the solutions for these equation by multiplying and adding it. Details
of transformation are given in
65
and omitted here for simplicity
0s anddt t)e(r,uu ,dt t)e(r,uu where
0u
RR
K
u
RR
K)(s
dr
ud
r
1
dr
ud
s
GM
uKuK)M(s
dr
ud
r
1
dr
ud
st
0 0
22
st
11
1
νf
2
νf
1
22
2
2
21
2
1
21
2
==
=+
+
−+
−=+++−+
−
−
Eq. 5.3.5
1))(
t
ikπ
ε(r,u Realε)(r,u
2
1
t
e
t)(r,u
1))(
t
ikπ
ε(r,u Realε)(r,u
2
1
t
e
t)(r,u
N
1k
k
22
εt
2
N
1k
k
11
εt
1
−++=
−++=
=
=
Eq. 5.3.6
where Real refers to the real part of’, i2 = −1 is the imaginary number, N is the number of terms used
in the Riemann-sum approximation and ε is the real part of the Bromwich contour that issued in
inverting Laplace transforms. The Riemann-Sum approximation for the Laplace inversion involves
a single summation for the numerical process. Its accuracy depends on the value of ε and the
truncation error dictated by N. The quantity εt = 4.7 is found to be more appropriate, since other
tested values of εt seem to need longer computational time.
5.3.4 Comparison with Numerical
The momentum equations for fluid and dust particles with under the initial and boundary conditions
are solved numerically using implicit finite difference method
66
, and the results presented in Table
65
See previous.
66
Obtained using the Riemann-sum approximation method and that obtained using finite difference method
for both the fluid and the particle phases when t = 0.2, G = 1, K = 50, Rf = 0.25 and M = 2.
5.3.1. The procedure involves the replacement of the partial differential into the finite difference
equations at the grid point. The time derivative is replaced by the backward difference formula, while
the spatial derivatives are replaced by central difference formula. The above equations are solved by
Thomas algorithm by manipulating into a system of linear algebraic equations in the tridiagonal form.
At each time step, the process of numerical integration for every dependent variable starts from the
first neighboring grid point of the outer surface of the inner cylinder at r = 1 and proceeds towards
the inner surface of the outer cylinder at r = λ. The process of computation is advanced until a steady
state is approached by satisfying the following convergence criterion:
10
AM
AA
6
max
ji,1ji,
−
+
Eq. 5.3.7
Here Ai, j stands for the velocity field of the fluid and dust particle, M* is the number of interior grid
points and |A|max is the maximum absolute value of Ai, j. In the numerical computation special
attention is needed to specify Δt to get steady state solution as rapid as possible, yet small enough to
avoid instabilities.
In conclusion, we have employed the combination of the Laplace transform technique, D’Alembert’s
and Riemann-sum approximation methods to obtain the solutions of unsteady MHD two-phase flow
of fluid-particle suspension in the annular gap of two concentric cylinders. We have considered the
effect of various dimensionless parameters occurring in the problem such as the Hartmann number
M, the viscosity ratio Rν and the ratio of the substance quantity of mixture Rf on the flow field. The
skin frictions at the opposite cylinders are seen to be of opposite sign; at the outer surface of the inner
cylinder it is positive and negative at the inner surface of the outer cylinder. The result obtained
demonstrates the reliability of the Riemann-Sum approximation method as comparisons made with
those obtained using the implicit finite difference method shows consistency between them.
Table 5.3.1 Comparison of Numerical Velocity (Riemann Sum vs. Finite Difference)
5.4 Case Study 4 - Simulation of Compressible 3-Phase Flows in an Oil Reservoir
Oil extraction represents an important investment and the control of a rational exploitation of a field
means mastering various scientific techniques including the understanding of the dynamics of fluids
in place. A theoretical investigation of the dynamic behavior of an oil reservoir during its exploitation
is presented by [Ahmadi, et. al.]
67
. More exactly, the mining process consists in introducing a miscible
gas into the oil phase of the field by means of four injection wells which are placed on four corners of
the reservoir while the production well is situated in the middle of this one. So, a mathematical model
of multiphase multi-component flows in porous media was presented and the cell-centered finite
volume method was used as discretization scheme of the considered model equations. It ensues from
the analysis of the contour representation of respective saturations of oil, gas and water phases that
the conservation law of pore volume is well respected. Besides, the more one moves away from the
injection wells towards the production well; the lower is the pressure value. However, an increase of
this model variable value was noticed during production period. Furthermore, a significant
accumulated flow of oil was observed at the level of the production well, whereas the aqueous and
gaseous phases are there present in weak accumulated flow. The considered model so allows the
prediction of the dynamic behavior of the studied reservoir and highlights the achievement of the
exploitation process aim
68
.
5.4.1 Mathematical Modeling
The “black-oil” model is considered as constituted by three fluid phases (oil, gas, and water) in each
of them can be present the following three components: a lighter component (gas) which can be at
the same time in the oil phase and in the gas phase, a heavier component which can only be in the oil
phase, and a component water which can only be in the water phase
69
. The capillary pressures are
assumed to be negligible
70
-
71
. Accordingly, all the present phases in the reservoir have the same
pressure. Moreover, the studied medium is considered as isotropic so that the components of the
permeability tensor have the same values in all directions.
As there is a mass transfer between the oil and gas phases, mass conservation is not satisfied for these
two phases. However, the total mass of each component is conserved. Besides, as the water phase is
completely separated from the other phases and the component water is only present in the water
phase, the mass conservation is well respected for this phase. Hence, the equations of the black-oil
model can be formulated as follows. Mass conservation related to the component water can be
written as
q)u(ρ
t
)ρ (
www
w=+
Eq. 5.4.1
67
Malik El’Houyoun Ahmadi, Hery Tiana Rakotondramiarana, Rakotonindrainy, “Modeling and Simulation of
Compressible Three-Phase Flows in an Oil Reservoir: Case Study of Tsimiroro Madagascar”, American Journal of
Fluid Dynamics 2014, 4(4): 181-193.
68
Malik El’Houyoun Ahmadi, Hery Tiana Rakotondramiarana, Rakotonindrainy, “Modeling and Simulation of
Compressible Three-Phase Flows in an Oil Reservoir: Case Study of Tsimiroro Madagascar”, American Journal of
Fluid Dynamics 2014, 4(4): 181-193.
69
Z. Chen, G. Huen, Y. Ma, “Computational Methods for multiphase flows in porous media”, SIAM Ed., Philadelphia
PA, USA, 2006.
70
Krogstad, S., Lie, K.A., Nilsen, H.M., Natvig, J.R.., Skaflestad, B., and Aarnes J.E., “A Multiscale Mixed Finite-
Element Solver for Three-Phase Black-Oil Flow”., Proc., Society of Petroleum Engineers (SPE) Reservoir
Simulation Symposium, The Woodlands, Texas, USA, 2009.
71
Hoteit, H., and Firoozabadi A., 2006, “Compositional modeling of discrete fracture media without transfer
functions by the discontinuous Galerkin and mixed methods,” SPE journal, 11(03), 341-352.
whereas for the heavier component, one can write:
q)(ρ
t
)Sρ (
oo0o
o0o =+
u
Eq. 5.4.2
and the lighter component is governed by:
q)uρu(ρ
t
)SρSρ (
gggoGo
ggoGo =++
+
Eq. 5.4.3
where ρGo and ρOo are the densities of the lighter and the heavier components in the oil phase
respectively. Equation implies that, the lighter component (gas) can be at the same time in the oil and
the gas phases. The velocity of each phase (α = w, o, g) is governed by the generalized Darcy’s law and
can be calculated by the following relationship:
g)ρp(
μ
k
u αα
α
rα
α−= K
Eq. 5.4.4
in which, K denotes the tensor of the absolute porousness’s of the porous media, whereas g denotes
the gravity acceleration vector. The system of mentioned equations is completed by the following
closing relationships. Conservation of pore volume (the sum of the saturations in a pore is equal to
unity):
1SS S wgo =++
Eq. 5.4.5
Constraints on the tube pressures
(oil-water) pcow and (gas-oil) pcgo:
0ppp
0ppp
ogcgo
wocow
=−=
=−=
Eq. 5.4.6
5.4.2 Temporal and Spatial
Discretization Methods
An implicit Euler scheme is used
for the time discretization while a
cell-centered finite volume
scheme was used for spatial
discretization. Indeed, the
developed model is constituted by
conservation equations. Since the finite volume schemes are conservative, they are better suited for
solving the considered system of equations. All the borders of the reservoir are considered
impervious. No flow either goes out or enters anywhere but places where wells are positioned. As
depicted in Figure 5.4.1, four injection wells are placed in the four corners of the reservoir while a
production well is placed in its center. A condition of pressure in each cell containing a well with
perforation is imposed. While the injection of gas in the reservoir and in each cell containing an
Figure 5.4.1 Sketch of the reservoir with the four injection
wells at the corners and the production well in the center
injection wells being the simulation object, gas saturation is considered equal to one. Further
information can be obtained from [Malik, al.]
72
. The Newton-Raphson method was used for the
linearization of the above nonlinear system of discretized equations. Afterward, the obtained linear
system can be solved by classical methods of resolution of linear systems. In the present work,
iterative Generalized Minimum Residual (GMRES) Method was used for this purpose.
5.4.3 Results and Discussion
Results simulating a three-phase oil-water-gas three components model whose lighter component
may be simultaneously in the oil phase as well as in the gas phase. They show the evolution of the
pressure, saturation and cumulative flow rate generated during the oil extraction. A spatial decay of
pressure is observed while a temporal pressure increase occurs. The pressure imposed on the
injection wells is higher than the pressure within the reservoir; the aforementioned spatial pressure
decay that is observed following the fluid displacement front towards the center may be due to a
pressure drop in the gas flow through the porous medium
73
. Moreover, the energy transferred by
the gas to fluids that are in place (oil and water) justifies the temporal pressure increase. However,
the pressure is still quite enough to push the oil to the production well and ease its drawing out.
Indeed, the purpose of the gas injection in the reservoir is not only to increase the pressure, but also
to make the oil less viscous to facilitate mobility for its extraction. As can be seen from Figure 5.4.2
which show the variations of cumulative flow in the production well, a good amount of oil is
produced. Such result conforms to the goal sought by the extraction process. The miscibility of the
oil in the gas, combined with the fact that the oil is much lighter than the existing water, promotes
such production. There is also a very low quantity of produced water which is lower compared to
that of the produced gas, which itself is significantly less than that of produced oil. It can be justified
by the fact that not only there may be an expansion of the gas during production, but the gas is also
much lighter than water.
72
Malik El’Houyoun Ahamadi, Hery Tiana Rakotondramiarana, Rakotonindrainy, “Modeling and Simulation of
Compressible Three-Phase Flows in an Oil Reservoir: Case Study of Tsimiroro Madagascar”, American Journal of
Fluid Dynamics 2014, 4(4): 181-193.
73
See previous.
Figure 5.4.2 Cumulative flow in the production well for a production day
5.5 Case Study 5 - Effects of Mass Transfer & Mixture of Non-Ideality on
Multiphase Flow
Authors : [Irani, Mohammad; Bozorgmehry Boozarjomehry, Ramin; Pishvaie, Sayed Mahmoud Reza
and Tavasoli, Ahmad]
74
In the chemical and petrochemical industries, Multi-Component phases commonly undergo
composition changes due to various phenomena resulting in the transfer of species from one phase
to another, or conversion of species through chemical reactions. On the other hand, the thermo-
physical properties of a multi-component system are strongly dependent on its compositions. This is
due to the fact that the properties of a multi-component mixture are not necessarily equal to the
weighted average of the corresponding properties of its constituting pure components. This results
in a severe interaction between hydrodynamic and thermodynamic behavior of a multi-component
system. This interaction seems to have more effects on the hydrodynamic behavior of multi-
component multiphase systems. Here we concern with the effects of the non-ideal behavior of phases
on their hydrodynamic behaviors, have been studied based on a CFD framework in which the
properties of each phase are rigorously modeled as a function of temperature, pressure and
concentration of phase constituting components. The CFD framework is developed based on
Eulerian - Eulerian model. The proposed framework can be used in modeling and simulation of
multiphase flow of non-ideal mixtures.
5.5.1 Mathematical Model
The variation of liquid holdup with time and position is obtained by solving the continuity equations
for the liquid and gas phases. The continuity equation for the flowing liquid and gas is written in
terms of the accumulation and convection terms balanced by the total mass transferred to and from
the other phases (written in terms of interphase fluxes for gas-liquid equations, discussed later).
Since gas and liquid phases do not interpenetrate into each other in the reactor, the VOF approach is
used. In this approach, the motion of all phases is modeled by formulating local, instantaneous
conservation equations for mass and momentum
75
. The variation of velocity with time and position
is calculated by solving the momentum balance equation. The momentum equations can be written
in terms of accumulation and convection terms on the left-hand side, and the gravity, pressure
gradient and viscous stresses terms on the right-hand side, as the pressure and velocity are assumed
to be equal in both phases. The properties appearing in the transport equations are determined by
their averaging based on phase volume-fraction. The continuity and momentum equations for a
phase, ‘q’, in a multiphase flow problem is as follows:
Eq. 5.5.1
74
Irani, Mohammad; Bozorgmehry Boozarjomehry, Ramin; Pishvaie, Sayed Mahmoud Reza and Tavasoli,
Ahmad, “Investigating the Effects of Mass Transfer and Mixture Non-Ideality on Multiphase Flow Hydrodynamics
Using CFD Methods”, Iran. J. Chem. Chem. Eng., Vol. 29, No. 1, 2010.
75
Hirt C. W., Nichols, B.D., Volume of Fluid (VOF) Method for the Dynamics of Free Boundaries, J. Comp. Phys.,
39, p. 201 (1981).
The variation of velocity with time and position is calculated by solving the momentum balance
equation. The momentum equations can be written in terms of accumulation and convection terms
on the left-hand side, and the gravity, pressure gradient and viscous stresses terms on the right-hand
side, as the pressure and velocity are assumed to be equal in both phases. The properties appearing
in the transport equations are determined by their averaging based on phase volume-fraction.
5.5.1.1 Bulk Species Transport
The dynamic variation in the liquid and gas phase species concentrations are obtained by solving the
unsteady state species mass balance equations, consisting of accumulation, convection, and
interphase transport for the gas and liquid phases written as
Nα)CαD-vC.(α)C(α
t
Nα)CαD-vC.(α)C(α
t
gl
ilillilillili
gl
igiggigiggigg
=+
=+
Eq. 5.5.2
5.5.1.2 Interphase Mass Transfer
Observations have indicated that the rates of mass transfers are closely related to the diffusion at the
interface that is related to the concentration gradients at the interface, too. In real problems,
however, we have usually no direct way to measure the concentration gradients at the interface. One
of the approaches that can be used to estimate the concentration gradient is the approximation of
various elements of concentration gradient in each phase using Finite Difference approach. In fact
mass transfer coefficient based on Film theory is originally obtained through this approach.
According to this approach various elements of concentration gradients of phase 'q' can be obtained
as follows:
Δx
CC
x
C
j
iqiq
j
iq
−
Eq. 5.5.3
Where Ciq is the concentration of i-th component in phase q right at the interface and C*iq is the
concentration of this component when phase q is at equilibrium with the other phase in the mixture.
This is based on the fact that in a multiphase system, they are assumed to be at equilibrium right at
their interface. For a mixture containing vapor and liquid the equilibrium concentration of various
components can be obtained through isothermal flash calculations which are presented at all
chemical engineering thermodynamic text books
76
-
77
. Details of flash calculation algorithm and
equations were given in
78
. The concentration of various species in vapor and liquid phases are
obtained based on Eq. 5.5.3, respectively. Having obtained equilibrium concentrations, one can
obtain the flux of species transfer (q Ni) and the rate of inter-phase mass transfer (Spq) through Eq.
5.5.4, respectively, in which Mi is molecular weight for i-th species. Calculated flux or component i (
q Ni) in one phase is a source or sink for the same component in the other phase because there is no
accumulation at the interface.
76
Smith J.M, Van Ness H.C., “Introduction to Chemical Engineering Thermodynamics”, 6th Edition, McGraw-Hill.
77
Walas S.M, “Phase Equilibria in Chemical Engineering”, Butterworth, Storeham, USA (1985).
78
See 44.
MNS , -NN ,
Δz
CC
DN n
1i i
q
ipq
q
i
p
i
j
iqiq
i
q
i
=
==
−
=
Eq. 5.5.4
5.5.2 Simulation Procedure
The transport equations (Eq. 5.5.1 and Eq. 5.5.2) were discretized by control volume formulation.
UPWIND scheme was used for discretization
79
. A segregated implicit solver method with implicit
linearization was used to solve discretized momentum equations. These equations have been
obtained through the application of the first-order upwind scheme and for the pressure velocity
coupling, the SIMPLE scheme has been used. For the pressure equation, the pressure staggering
option (PRESTO) scheme was used. The program first reads the structured data from pre-processing
section (in which the mesh representing the equipment has been built), before it goes into two nested
iteration loops. Inner loop iterations are performed within each time step using the equations
corresponding to the discretized version of the proposed model, while the outer loop goes through
simulation times until it gets to the final time or steady state whichever happens sooner. At each time
step, before going into the inner loop the fluid properties in each cell are calculated.
In the inner loop, all the discretized equations are solved in three steps. In the first step, the physical
properties such as density is updated based on the current solution. If the calculation has just begun,
the fluid properties will be updated based on the initialized solution. In the second step, the flash
calculation is performed in order to obtain the equilibrium concentrations based on which the source
terms of the species concentrations and continuity equations are obtained. In the third step,
equations of continuity and momentum are solved and after obtaining the velocity and pressure
fields, equations corresponding to species concentration are solved in order to obtain the profiles of
the concentration of various species. In this step, with the help of Eulerian-Eulerian approach (VOF
approach), the trajectory of interface between two phases (liquid and gas) is determined. At the end
of this step, convergence checking based on the norm of errors is done. Due to the nonlinearity and
interactions of various equations, the convergence is usually achieved after several iterations at each
time step.
In order to get stable and meaningful results the time step must be very small (in the order of 10−4 s).
However, as time goes on, and various states of the system (e.g., velocities and species concentration)
obtain their corresponding smooth profile throughout the system, the time step can be gradually
increased. This is due to the fact that dependence of various physical properties (e.g., density, specific
heat…) on species concentration increases the amount of interaction and coupling of equations. It
should also be noted that, in this mechanism the time step could not get values beyond 10-3s. In
general, the time-stepping strategy depends on the number of iterations by time step needed to
ensure very low residuals values (less than 10−7 for concentration and 10-5 for momentum and
continuity).
5.5.3 Results and Discussion
The initial condition of the simulation at which the liquid height measured from bottom was 7cm. At
the same time, the concentration of octane in gas phase and propane in liquid phase were set to zero.
It was also assumed that there is no movement in the system and hence the velocity was set to zero
for the whole domain. As time goes on, species are transferred between phases, this leads to a time
varying concentration profiles in both phases and a general velocity field for the whole fluid (see
Figure 5.5.1). Octane was transferred from liquid phase to gas phase and concentration of octane
in liquid was decreased whereas concentration of octane in gas was increased. On the other hand,
79
Patankar S.V., “Numerical Heat Transfer and Fluid Flow”, Taylor and Francis, (1980).
Propane dissolved in liquid phase which leads to its concentration decrease in gas phase, can be seen
right at the interface. The propane concentration has its least value for gas phase and the largest
value for the liquid phase . As a result of mass transfer in the interface, velocity in this region is higher
than others. Density of gas phase was increased near the interface because concentration of octane
was increased. In contrast, density of liquid phase was decreased near interface because
concentration of propane was increased; (for further information please see
80
).
5.5.4 Concluding Remarks
In the present work, a CFD framework has been proposed to simulate the multiphase mass transfer
problems in chemical processes. For this purpose, a numerical method based on a macroscopic model
and the finite volume method was applied. The proposed CFD framework is able to solve multiphase
mass transfer problems with high interaction of thermodynamic and hydrodynamic behavior of the
system. The proposed framework makes it possible to take into account the interacting effects of
mixture non-ideality, mass transfer and hydrodynamics on multiphase system in a more realistic
way. None of the analysis and studies that have been done on the hydrodynamic of multiphase
systems has covered these effects till now, the major reason why these issues have not been covered
till now was the fact that none of the available commercial CFD applications has a readymade frame
work for such an analysis.
5.6 Case Study 6 - Numerical Study of Turbulent Two-Phase Coquette Flow
5.6.1 Motivation and Literature Survey
The motivation behind this work is the need to understand bubble generation mechanisms due to
interactions between free surface and turbulent boundary layers as commonly seen near ship walls
80
Irani, Mohammad; Bozorgmehry Boozarjomehry, Ramin*+; Pishvaie, Sayed Mahmoud Reza and Tavasoli,
Ahmad, “Investigating the Effects of Mass Transfer and Mixture Non-Ideality on Multiphase Flow Hydrodynamics
Using CFD Methods”, Iran. J. Chem. Chem. Eng., Vol. 29, No. 1, 2010.
Figure 5.5.1 Contour of gas volume fraction at different time levels
t = 0.0 t = 3650
as investigated by [Ovsyannikov, et al.]
81
. As a recognized problem, we consider a turbulent plane
coquette flow with vertical parallel sidewalls and an air-water interface established by gravity in the
vertical direction. Two-phase coquette flow has been described in the literature in different flow
setups. Most studies were limited to cases of low Reynolds number and the evolution of a single
bubble/droplet. Deformation and breakup of a single droplet in a plane coquette flow at low Reynolds
number has been studied experimentally, theoretically, and numerically. In another example of the
two-phase coquette flow is the two-layers of immiscible fluids which are set between moving
horizontal walls. Due to viscosity difference between fluids, there is a jump in the tangential velocity
gradient across the interface which induces instabilities at the fluid interface [Coward]
82
, [Charru &
Hinch]
83
.
At high Reynolds number, there are only a few studies of two-phase Couette flow. [Iwasaki]
84
studied
the dynamics of a single immiscible drop in turbulent gas ow between two moving walls. [Fulgosi]
85
and [Liu]
86
performed direct numerical simulation (DNS) of interface evolution in Couette flow
between two moving horizontal walls. One interesting case of a two-phase Couette flow in a turbulent
regime is when the initial interface is set to be orthogonal to the moving vertical walls. In such a
setup, the interaction between the fluid interface and the turbulent boundary layer is a key
phenomenon. At sufficiently high Reynolds, Weber and Froude numbers, shear-induced interfacial
waves can break, which leads to the formation of air cavities. These air cavities will be further
fragmented by turbulence to smaller bubbles. These complexities make two-phase Couette flow at
high Reynolds number a challenging problem for both experiments and numerical analysis.
Capturing the small-scale ow and interface features requires high-resolution experimental
techniques and very expensive DNS calculations. Only two numerical studies Kim
87
-
88
have been
performed for investigation of air entrainment and bubble generation in two-phase Couette flow.
The current work is a continuation of our recent studies (Kim), where we performed numerical
simulations of the interface breakup in two-phase Couette flow at Reynolds number of approximately
13000 and Weber number of approximately 42000 (surface tension coefficient was much smaller
than the realistic value for an air-water system). The effect of Froude number on the interface
breakup and bubble generation was studied in Kim et al. (2012). The second paper of Kim et al.
(2013) was mostly devoted to the development and assessment of a mass conservative interface-
capturing method based on a geometric volume-of-fluid (VOF) approach, and one simulation of the
two-phase Couette flow was performed for a Reynolds number of 12000 and a Weber number of 200.
However, there have been no studies with one-to-one matched experiments and numerical
simulations.
81
A.Y. Ovsyannikov, D. Kimy, A. Mani AND P. Moin, “Numerical study of turbulent two-phase Couette flow”, Center
for Turbulence Research Annual Research Briefs 2014.
82
Coward, A. V., Renardy, Y. Y., Renardy, M. & Richards, J. R., “Temporal evolution of periodic disturbances in two-
layer Couette flow”, J. Computational Physics, 132 (2), pp. 346-361, 1997.
83
Charru, F. & Hinch, J. E., “Phase diagram of interfacial instabilities in a two-layer Couette flow and mechanism
of the long-wave instability”, J. Fluid Mech. 414, pp. 195-223, 2000.
84
Iwasaki, T., Nishimura, K., Tanaka, M. & Hagiwara, Y. ,”Direct numerical simulation of turbulent Couette flow
with immiscible droplets”, Int. J. Heat Fluid Flow 22, pp. 332-342, 2001.
85
Fulgosi, M., Lakehal, D., Banerjee, S. & De Angelis, V. ,”Direct numerical simulation of turbulence in a sheared
air-water ow with a deformable interface”, J. Fluid Mech. 482, pp. 319-345, 2003.
86
Liu, S., Kermani, A., Shen, L. & Yue, D. K. P.,” Investigation of coupled air-water turbulent boundary layers using
direct numerical simulations”. Phys. Fluids 21 (6), pp. 62-108, 2009.
87
Kim, D., Mani, A. & Moin, P., “Numerical simulation of wave breaking in turbulent two-phase Couette flow”,
Annual Research Briefs, Center for Turbulence Research, Stanford University, pp. 171-178-2012.
88
Kim, D., Mani, A. & Moin, P., “Numerical simulation of bubble formation by breaking waves in turbulent two-
phase Couette flow”, Annual Research Briefs, pp. 37-46, 2013.
5.6.2 Objectives
The primary objective of this work is to perform a numerical simulation of a two-phase Couette flow
with flow parameters very close to those of the laboratory experiment conducted by collaborators.
The bubble formation rate, bubble size distribution, and the effect of interface on the modulation of
turbulence are the main characteristics of this flow type, and our investigations are focused on
understanding these characteristics.
5.6.3 Problem Statement
We perform a simulation of a two-phase system with realistic air/water density and viscosity ratios.
The density of liquid is ρliq = 1000 kg/m3 and the density of gas is ρgas = 1.2 kg/m3. However, to reduce
values. Thus the viscosity of the
gaseous phase is μgas = 7.2 x105 Pa-s and
the viscosity of the liquid phase is μliq =
4x103 Pa - s. The surface tension
coefficient σ and gravity acceleration g
take realistic values of 0.07N/m and
9.81m/s2, respectively. Figure 5.6.1
depicts the schematic of the flow
configuration and domain size. The
computational domain is a rectangular
box with sizes 2_h, 2h and 6h in the
stream wise (x), wall-normal (y) and
span wise (z) directions, respectively.
Here h = 2 cm is the half-distance
between walls. Initially, the interface is
located at a plane z = 4h, hence a height
of liquid layer Hliq is 4h and a height of
gas layer Hgas is 2h. The sidewalls are
moving in the opposite directions with
speed of Uw = 1.6m/s. Based on the
chosen parameters, the following main
dimensionless parameters are:
h
H
Ar ,
gh
U
Fr ,
σ
hUρ
We,
μ
hUρ
Re liq
w
2
wliq
liq
wliq ====
Eq. 5.6.1
which are Reynolds, Weber, Froude numbers, and aspect ratio (ratio of water depth to h),
respectively. All non-dimensional groups are determined using properties of the liquid phase. In the
current study, Re = 8000, We = 730, Fr = 3.6 and Ar = 4.
5.6.4 Governing Equations and Numerical Method
The governing equations describing the motion of two immiscible, incompressible New
tonian fluids are the conservation of mass and momentum. The first equation is given in terms of the
volume fraction function as
Figure 5.6.1 Schematic illustration of the flow
geometry
ρ.p-).(ρ
t
ρ
0).(ψ
t
ψ
st
Fgτuu
u
u
+++=+
=+
Eq. 5.6.2
where u is the velocity, p is the pressure, ρ is the density, τ = μ( u + uT ) is the shear stress tensor,
μ is the dynamic viscosity, g is the acceleration due to gravity and Fst = σκδ∑n is the surface tension
force. Here, σ is the surface tension coefficient, δ∑ is the Dirac delta function, κ is the interface
curvature, and n is the interface normal vector. The volume fraction function is equal to 1 in the gas
phase and 0 in the liquid phase. The interface is then represented by the volume fraction values, 0 <
ψ < 1. In the case of a two-phase ow with immiscible fluids, the density and dynamic viscosity are the
stepwise functions and can be written in terms of ψ as:
ρρψρψ
μμψμψ
Eq. 5.6.3
For discretization of Eqs. (2.2), we use numerical schemes as described in [Kim et al. 2013]. In brief,
we use the finite-volume pressure-correction method, where the inter-face dynamics is captured by
the volume-of-fluid method. Geometric flux reconstruction is based on a piecewise line interface
calculation (PLIC) algorithm. The VOF method conserves the mass of each phase within machine
precision, and this is essential for simulation of two-phase flows at high Reynolds and Weber
numbers. The surface tension force is computed using the continuum surface force model [Brackbill
et al. 1992] coupled with the balanced force method [Francois et al. 2006]. For an accurate calculation
of interface normal vector and curvature, a level set function is used which is reconstructed from the
field at every time step using a fast marching method [Sethian 1999].
5.6.5 Initial and Boundary Conditions
The flow is assumed to be statistically homogeneous in the stream wise x direction where periodic
boundary conditions are used. On the side counter-moving walls (y = _h), we use no-slip boundary
conditions. On the top and bottom walls (z = 0 and z = 6h), we use slip boundary conditions. On all
solid wall boundaries, no-flux conditions are used for the volume fraction function. As the initial
condition, we use a laminar velocity profile perturbed by 10% noise. The initial value for
corresponds to the at shape of the interface.
5.6.6 Grid Resolution and Time Step Requirement
In order to accurately capture the interface dynamics, we need to resolve the typical interface scale
(rcr) and turbulent scales (η and δν).
5.6.6.1 Turbulent Length Scale
The Kolmogorov length scale is given by ≈110 μm and ε is the mean energy dissipation rate per unit
mass is ≈ 0.5m2 s-3; (for detail discussion see 54).
5.6.6.2 Interface Length Scale
In addition to turbulent length scales, we need to resolve an interfacial length scale (bubble radius)
in two-phase simulations. There are two major mechanisms of bubble formation: turbulent
fragmentation [Kolmogorov 1949; Hinze 1955] and instability of the air _lm due to liquid-liquid
impact [Esmailizadeh & Mesler 1986; Pumphrey & Elmore 1990]. In our simulations we resolve only
the bubbles due to the first mechanism. This length scale can be estimated using the Kolmogorov-
Hinze theory. We apply this theory to estimate the breakage of bubbles in a turbulent liquid flow. If
the bubble diameter is larger than the Kolmogorov length scale, then the critical bubble radius
(referred to as the Hinze scale). In our case, the Hinze scale is much larger than the Kolmogorov
length scale and the critical bubble radius. For critical Weber number 4.7 (according to Deane &
Stokes 2002), the critical bubble radius is rcr ≈3mm >> η. Therefore, we choose conventional DNS
resolution as in single-phase flows. We use a Cartesian grid with uniform mesh spacing in x and z
directions, and stretched mesh in the y direction according to
)(tanh
1N
1)2(j
1γ(h tanh
y y
j
−
−
+−
=
Eq. 5.6.4
where the stretching parameter ϒ is 2.9. Based on the viscous length scale in the liquid phase the
grid resolution is Δx+ =13, Δy+min= 0.2, Δy+max =13 and Δz+ =7. Such discretization results in at least 4
grid points per Hinze scale (8 points per bubble diameter) and 18 grid points per viscous sublayer.
Finally, the time step is given from the stability constraint due to surface tension as it is more
restrictive than the stability conditions due to convection and gravity terms (the viscous terms are
treated implicitly):
s10Δy
4ππ
ρρ
Δt 6-3/2
min
gasliq
+
=
Eq. 5.6.5
5.6.7 Results
Figure 5.6.3 (a-d) show instantaneous snapshots of the interface (given by iso surface ψ = 0.5). On
the free surface, shear-induced oblique wave structures are observed (Figure 5.6.3(a)), then the
interfacial waves grow in amplitude (Figure 5.6.3(b)), leading to breakup of the interface (Figure
5.6.3(c)). The air cavities are found underneath the free surface, trapped between the breaking
interfacial waves. These air cavities are subsequently fragmented into air bubbles in the water.
Finally, Figure 5.6.3(d) shows the interface at the fully developed state. Figure 5.6.2 shows time-
and stream wise-averaged flow for two cases
89
: (a) a two-phase Couette flow and (b) a single-phase
Couette water flow at the same Reynolds number of 8000. The color contours correspond to the
stream wise component of the mean velocity, ū, while the wall-normal and span wise components,
(v, w), are shown as vector plot. The maximum Root-Mean-Square (RMS) value of in-plane velocities
represents (after 100 flow-through times) approximately 6-7% of the maximum stream wise velocity
for both cases and does not diminish with time. For the single-phase Couette flow, secondary flow is
represented by four large eddies, while for the two-phase case the secondary flow is more complex
due to the effects of the interface. In our simulations the length of the computational domain, 2πh,
was chosen as in classical simulations of pressure-driven channel ow. However, it is known from
studies of single-phase Couette flow [Lee & Kim 1991; Komminaho et al. 1996; Papavassiliou &
Hanratty 1997] that the domain length should be much longer. In this work we focus on a study of
interface/boundary layer interaction and leave the study of Couette flow in longer channels for future
research. Mean stream wise velocity profiles measured at z/h = 1.5, z/h = 2.5, z/h = 3.5 and z/h = 4,
89
Color plot shows the mean stream wise velocity; vector plot depicts mean in-plane flow. (a) Two-phase
Couette flow at Re = 8000, We = 730 and Fr = 3.6; (b) Single-phase Couette flow at Re = 8000.
locations are shown in Figure 5.6.4
90
. In addition to two-phase Couette results, we show the result
Figure 5.6.3 Snapshots of the Air-Water Interface at Different Times (same source)
(a) t* = 5 (b) t* = 10
(c) t* = 15 (d) t* = 60
Figure 5.6.2 Turbulent statistics: time- and stream wise-averaged velocity field
of simulation for single-phase Couette flow at the same Reynolds number of 8000. Figure 5.6.4 (a)
shows velocity profiles in non-dimensional units, U/Uw versus y/h. Figure 5.6.4 (b) shows the same
data in non-dimensional viscous units according to U+ = (U - Uw)/uτ and y+ = (h - y)/δν. As seen from
Figure 5.6.4 (b), there is no collapse of the results for two-phase Couette flow with the log-law even
for a velocity profile quite far from the interface at z/h = 1.5. Even for single-phase Couette flow, a
particular profile of stream wise velocity does not necessarily collapse with the log-law owing to the
presence of persistent roller structures. Only after averaging of velocity in a vertical direction does
the velocity profile for single-phase Couette flow matches with the log-law.
5.6.8 Influence of the Water Depth
Figure 5.6.5
91
shows a comparison of the fully developed air-water interface from our previous
results
92
. (Figure 5.6.5(a)) and the current simulation (Figure 5.6.5(b)). The results on the left
figure were obtained for an Aspect Ratio of 1.57, whereas in the current simulation the Aspect Ratio
is 4. As seen, the simulation for the higher value of the aspect ratio predicts much less air entrainment.
To confirm our hypothesis of the influence of the water depth on bubble density, we are currently
running simulations for low and high values of the aspect ratio (1.57 and 8) for the same non-
dimensional parameters: Reynolds, Weber and Froude numbers, as in the simulation presented in
this work.
5.6.9 Conclusions
In this work we performed a numerical simulation of a two-phase Couette flow at a Reynolds number
of 8000, Froude number of 3.6, Weber number of 730 and at realistic air-to-water density and
viscosity ratios. Except for Reynolds number and water depth, the parameters of simulation
correspond to experiments currently being performed at the University of Maryland. The VOF
method has been used to predict interface dynamics. To achieve statistically state two-phase
simulations of Couette flow require much longer time compared to simulations of single-phase
Couette flow. Complication of turbulent intensity was found near the interface, whereas diminished
turbulent intensity was observed in the core region. It was found that the bubble density depends on
the water depth. To validate this result, in our ongoing work we compare numerical results obtained
91
(a) Results for an Aspect Ratio of 1.57 and Re = 12000, We = 206, Fr = 3:8 (Kim et al. 2013); (b) Present
results for an Aspect Ratio of 4 and Re = 8000, We = 730, Fr = 3.6
92
Kim, D., Mani, A. & Moin, P. ,”Numerical simulation of bubble formation by breaking waves in turbulent two-
phase Couette flow”, Annual Research Briefs, pp. 37{46. Center for Turbulence Research, Stanford University,
pp. 37-46, 2013.
Figure 5.6.4 Turbulent Statistics for Two-Phase Couette Flow
for different aspect ratios with experimental data. In addition, a simulation is being carried out with
deeper water at an aspect ratio Hliq=h of 8 and the same non-dimensional parameters, Re = 8000, We
= 730, Fr = 3:6.
5.7 Case Study 7 - Slug Flow in Horizontal Air and Water Pipe Flow
Authors : [Zahid I. Al-Hashimy, Hussain H. Al-Kayiem, Rune W. Time & Zena K. Kadhim]
93
The growth of liquid slugs in oil and gas pipelines is a vast and costly problem for the oil firms. A
pressure drop in oil production is the main source of the problem that leads to terrain-induced slug
flow in the pipeline between the production platform and wellhead platform. This type of slug flow
condition can create huge transient surges. The transient nature of the slugs if not appropriately
considered might become climacteric and can hasten the material’s fatigue with the risk of pipe
damage and maintenance costs. Recently, [Al-Hashimy, et al.]
94
has been simulated the slug flow
regime in an air-water horizontal pipe flow. The variables identified to characterize the slug regime
are the slug length and slug initiation. The volume of fluid method was employed assuming unsteady,
immiscible air/water flow, constant fluid properties and coaxial flow.
The simulated pipe segment was 8 m long and had a 0.074 m internal diameter. Three cases of air-
water volume fractions have been investigated, where the water flow rate was pre-set at 0.0028 m3/s,
and the air flow rate was varied at three dissimilar values of 0.0105, 0.0120 and 0.015 m3/s. These
flow rates were converted to superficial velocities and used as boundary conditions at the inlet of the
pipe. The simulation was validated by bench marking with a Baker chart, and it had successfully
predicted the slug parameters. The computational fluid dynamics simulation results revealed that
the slug length and pressure were increasing as the air superficial velocity increased. The slug
initiation position was observed to end up being shifted to a closer position to the inlet. It was
believed that the strength of the slug was high at the initiation stage and reduced as the slug
progressed to the end of the pipe. The pressure gradient of the flow was realized to increase as the
gas flow rate was increasing, which in turn was a result of the higher mean velocity.
93
Zahid I. Al-Hashimy, Hussain H. Al-Kayiem, Rune W. Time & Zena K. Kadhim, “Numerical Characterization Of
Slug Flow In Horizontal Air/Water Pipe Flow”, Int. J. Comp. Meth. And Exp. Meas., Vol. 4, No. 2 (2016).
94
Same as above.-
Figure 5.6.5 Air-Water Interface at Fully Developed State
5.7.1 Slug Flow and Slug Formation in Pipe
Slug flow refers to the phenomenon at which 2-phase liquid-gas movements exist in pipelines over a
broad range of intermediate flow rates, generating improper disorder resulting from the actions of
the liquid and gas plugs, known as slugs. The plug distribution of liquids and gases in slug flows are
highly unique but intermittent, basically because of the nature of the terrain, gas/liquid velocity
fluctuations, pigging, etc. A slug unit consists of an aerated liquid slug as well as an accompanying gas
bubble, controlled within a liquid film of varying thicknesses. The actual thickness of the film in most
cases differs from the minimum value at the front of the following slug towards the maximum value
at the rear of the preceding slug. Consequently, the slug length may remain steady along the direction
of travel while the pressure drops systematically across the sections of the pipe
95
.
The slug formation is a three-step process that is depicted in Figure 5.7.1. Originally, the flow is
stratified where the gas is at the top of the pipe and the liquid at the bottom. As the gas passes over a
wave, there is a pressure drop, then a pressure recovery, creating a small force upward within the
wave. Under the conditions that this upward force is sufficient to raise the wave until it extends to
the top of the pipe, the flow is considered as slug flow. Once the wave reaches the top of the pipe, it
forms into the familiar slug shape with a nose and tail. The slug is forced forward by the gas and thus,
can travel at a greater velocity than the liquid film.
The actual slug movement can be explained by changing the liquid slugs and the gas bubbles moving
above the liquid films, which in turn combine to develop what is known as a slug unit. The slug
frequency is described by the number of slugs passing a particular point along the pipeline over a
particular period of time. Amongst the slug flow characteristics, the slug frequency is an essential
component which relates to significant operational difficulties, like the flooding of downstream
facilities, severe pipe vibration, pipeline structural instability and wellhead pressure fluctuation. It is
generally known that pipe corrosion is substantially impacted by a high slug frequency.
5.7.2 Baker Chart
Flow regime maps for the 2-phase flow in a horizontal pipe have been intensively researched by
many researchers. [Baker]
96
presented a map of a two-phase flow in a horizontal pipe by using
various fluids in addition to demonstrating distinct phases of mass fluxes along with corresponding
fluid properties such as density and surface tension (see Figure 5.7.2). The Baker chart also features
two dimensionless parameters, l and y, to enable its application for various gas/vapor-liquid
combinations different from the standard one (air-water at atmospheric pressure and room
95
Orell, A., “Experimental validation of a simple model for gas–liquid slug flow in horizontal pipes”. Chemical
Engineering Science, 60(5), pp. 1371–1381, 2005.
96
Baker, O., “Simultaneous flow of oil and gas”. Oil and Gas Journal. 53, pp. 185–195, 1954
Figure 5.7.1 Hydrodynamic slug formation (Courtesy of Z. I. Al-Hashimy et al.)
Slug Unit
temperature) for which both parameters equate to unity. The Baker chart was used as a reference
for the simulation of the horizontal slug flow regimes in the present study.
5.7.3 Problem Formulation
In this present work, the Volume of Fluid (VOF) method has been implemented employing the
commercial software Star-CCM+ to simulate the horizontal sections of a pipe for air-water slug flow.
The objective has been to investigate the volume fraction profile and pressure drop along 8 m of the
pipe length will be predicted by the simulation. The [Baker] chart was adopted to justify the slug
presence in the simulation by computing the superficial mass velocities of the water and air. The
simulated horizontal slug flow patterns observed through visualizations of the phase distributions
were qualitatively compared against the flow regimes expected by the [Baker] chart. variation, with
time, in seven different cross sections along the pipe. In addition, the pressure drop along 8 m of the
pipe length will be predicted by the simulation. The [Baker] chart was adopted to justify the slug
presence in the simulation by computing the superficial mass velocities of the water and air. The
simulated horizontal slug flow patterns observed through visualizations of the phase distributions
were qualitatively compared against the flow regimes expected by the [Baker] chart.
The [Baker] flow regime map, as demonstrated in Figure 5.7.2, shows the standardized boundaries
of the various flow pattern regions as functions of the mass flux of the gas phase, G, and the ratio of
the mass flux of the water phase and air, L/G. Where, G was the mass flux of the gas phase (kg/m2 s)
= (gas mass flow rate/tube cross-sectional area) and L was the mass flux of water phase (kg/m2s) =
Figure 5.7.2 Baker chart where (.) Operating conditions of water–air two-phase flow
(water mass flow rate/tube cross-sectional area). The dimensionless parameters, l and y, had been
added so that the chart could be utilized for any gas/liquid combination that differed from the
standard combination. The standard combinations, at which both parameters, l and y, equate to unity,
which are water and air flow under atmospheric pressure and at room temperature. Consequently,
for the present application, where the fluids were air and water, the values of l and y are equal to 1.0.
By taking into account, the predicted values for l and y, the pattern of the two-phase flows with any
gas/liquid at other pressures and temperatures can be forecasted using the same chart. The
parameters l and y were can be calculated from
Eq. 5.7.1
Where σ, μ, ρ are the surface tension, viscosity and density, respectively. The subscripts ‘a’ and ‘w’
refers to the air and water, respectively, at normal temperature and atmospheric pressure; whereas,
the subscripts ‘g’ and ‘l’ refers to the vapor and liquid conditions of the fluid being considered.
5.7.3.1 Boundary Condition
The required boundary conditions depend on the physical models used, where water was designated
as the primary phase and air as the secondary phase for all cases [Al-Hashimy, et al.]
97
. The water and
air were considered incompressible. The most suitable boundary condition for external faces in
incompressible water was the velocity inlet. The outlet was considered as a pressure-outlet
boundary. The boundary conditions used are illustrated schematically in Figure 5.7.3. The velocity
in a multiphase flows is defined as the ratio of the velocity and the volume fraction of the considered
phase in a multiphase system. Actual velocity of phase = (velocity of phase)/(volume fraction of
phase). The average velocity of the flow varied depending on the volume fraction of each phase;
which, when defined as the area fraction of a phase, is expected to change in space and time. The
average velocity for the gas phase and liquid phase, which are called the gas superficial velocity and
liquid superficial velocity, can be given by:
97
Zahid I. Al-Hashimy1, Hussain H. Al-Kayiem, Rune W. Time & Zena K. Kadhim, “Numerical Characterization
Of Slug Flow In Horizontal Air/Water Pipe Flow”, Int. J. Comp. Meth. And Exp. Meas., Vol. 4, No. 2 (2016) 114–
130.
Figure 5.7.3 Boundary condition for water-air slug flow through a pipe
aU
A
AU
U, aU
A
AU
U WW
WW
SWGG
GG
SG ====
Eq. 5.7.2
There were two methods used in specifying the inlet boundary conditions for the simulation of the
slug flow
98
. The first method imposed perturbations at the inlet so that the volume fraction of the
liquid phase entered the pipe as a function of time. The second method, the pipe was initially assumed
to be filled with stratified air and water with 50% volume percentage and zero velocity. For the
present simulation, the initial and inlet region were: the upper half of the pipe was occupied by 50%
void fraction of the gas phase, aa and the lower half by 50% volume fraction of the water phase, aw.
Then, the field function was used to define the inlet water volume fraction as a function of time.
5.7.4 Volume of Fluid (VOF)
The VOF model has been utilized in this study to track the interface between the gas-liquid phases in
order to define the slug flow regime. The VOF technique exhibits an immense capability in tracking
the interface between the two phases using a color function. The color function is Ca = 1 for the entire
ak fluids and Ca = 0 for the void; thus, the interface is located at 0 < Ca < 1. In this method, all the cells
should be occupied by a single fluid or a combination of fluids because the VOF does not allow for
any void cells
99
. The water phase was selected as the primary phase. The tracking of the interface
between the phases was accomplished by the solution of a continuity equation for the volume
fraction of the secondary phase. The volume fraction equation was not solved for the primary phase;
the primary-phase (water phase) volume fraction was computed as
1aa GW =+
Eq. 5.7.3
Since the control volume at the interface location was occupied by fluids, the fluid properties,
particularly the viscosity and density, changed abruptly with the interface motion. The mixture
properties for the density and viscosity appearing in the momentum and mass equations were
calculated as:
μaμaμ
ρaρaρ
GGWWm
GGWWm
+=
+=
Eq. 5.7.4
Using conservation of mass and momentum, the local volume fraction of the water was given by the
following continuity equation:
Fgρ uuρ
xi
Uj
xj
Ui
μ
xix
(p)
x
)UU(ρ
t
)U(ρ
0
z
)W(a
y
)V(a
x
)U(a
t
a
imjimm
ii
jim
im
WWWWWWW
++
−
+
+
−=
+
=
+
+
+
Eq. 5.7.5
Where the first term, on the left-hand side, denotes the rate of the momentum increasing per unit
volume, and the second term denotes the change of the momentum due to convection per unit
volume. On the right side, the first term represents the pressure gradient, the second term represents
98
Al-Hashimy, Z.I., Al-Kayiem, H.H., Kadhim, Z.K. & Mohmmed, A.O., “Numerical simulation and pressure drop
prediction of slug flow in oil/gas pipelines”. WIT Transactions on Engineering Sciences, 89, 2015.
99
Ranade, VV., “Computational Flow Modeling for Chemical Reactor Engineering”, Vol. 5. Academic press, 2001.
the gravitational force, and the third term represents the viscous effect. The external force per unit
volume is given by the last term in the above equation and can be modelled using the continuum
surface force (CSF) model. For turbulence modeling, an SST k−w model in conjunction with implicit
time integration has been used. Details of methodology is available in [Z. I. Al-Hashimy, et al.]
100
.
5.7.5 Results and Discussion
5.7.5.1 Slug Initiation
The determination of the slug initiation had been according to the presence of the first slug in the
flow field. The simulation results at the three air superficial velocities are shown in Figure 5.7.4. It
is obvious that the first slug initiation was faster since the air superficial velocity was higher. It was
reveals the time and location of the slug initiation at a constant water superficial velocity of 0.651
m/s and three different air superficial velocities of 2.443, 2.792, and 2.49 m/s. The slug initiation
position was transferred to a shorter distance from the inlet.
5.7.5.2 Slug Length
For the slug body length and slug frequency, which is a reciprocal of the slug unit period, they could
actually be considered as the mean number of slugs per unit time as observed by a fixed observer.
The measurements of the average slug body by selecting the X coordinate of both the front and rear
ends are shown in Figure 5.7.5. The reference line indicated in each case is located about 4 m
downstream of the inlet. The slug length was estimated as LS = Xfront − Xrear . The slug length was
measured from the reference line up to the front of the slug. There was a proportional relation
between the slug length and the air superficial velocity. Prediction results of the slug length revealed
that when the air superficial velocity increased, the generated slugs became longer compared to the
case of the lower superficial velocity of air. Table 5.7.1 shows the predicted slug length at various
air superficial velocities.
100
Zahid I. Al-Hashimy1, Hussain H. Al-Kayiem, Rune W. Time & Zena K. Kadhim, “Numerical Characterization
Of Slug Flow In Horizontal Air/Water Pipe Flow”, Int. J. Comp. Meth. And Exp. Meas., Vol. 4, No. 2 (2016) 114–
130.
Figure 5.7.4 Slug initiation of the air-water slug flow
5.7.5.3 Slug Volume Fraction
The volume fraction in the slug body or gas void fraction is a crucial parameter for the design of
multiphase pipelines and the associated separation equipment; while, the phase composition is
proportional to its volume fraction. Figure 5.7.6 has provided the results of the simulation for the
predicted void fraction of the air-water slug flow regime at various cross sections from 1 to 7 m along
of the horizontal pipe, for the first three times. The distribution of water and air in the horizontal slug
flow can be vividly noticed. The red color refers to the water phase while the dark blue color refers
to the air phase, and the line between both colors display the presence of an interface. The best
approximation of the slug flow regime is observed compared with the slug flow regime in the Baker
char. The water slugs touched the upper part of the pipe and performed complete slug regime. As
stated before, t = 0 represents the initial conditions where the flow along the pipe was stratified flow,
in which the upper part was occupied by air, and the lower part was occupied by water due to the
gravitational effect. However, the water phase was steady until the generation of the first wave crest
because of the sinusoidal perturbation at the inlet; large waves were initiated, which heightened
steadily, filling the cross section of the pipe at time 0.5 s. The long slug was observed at 0.75 s, and it
continued to grow along the pipe at the downstream sections. Generally, the void fraction increased
with the increase in the gas velocity.
Figure 5.7.5 Slug length calculation of air-water slug flow
Air/Water
Mixture Velocity
(m/s)
Slug length (m)
Initial Time
(s)
Crossing
Time (s)
Case 1
3.049
0.449
0.64
2.02
Case 2
3.443
1.037
0.48
1.942
Case 3
4.141
1.5
0.373
1.641
Table 5.7.1 Slug length at different air-water velocities
In conclusion, the internal air-water two-phase slug flow behavior in a horizontal pipe were
examined and described the numerical procedure used to simulate the case. Slug initiation and
growth was effectively predicted by the 3D transient VOF model combined with the homogeneous
k−ω turbulence model. The volume fraction profile and pressure variation with time in seven
different cross sections along the pipe were examined.
5.8 Case Study 8 – Physical & Numerical Modeling of Unsteady Cavitation
Hydrodynamics
The study of numerical modeling of dispersed unsteady cavitation flows for large scale hydrodynamic
turbomachinery is presented by [Schnerr & Sauer]
101
. The cavitation model allows simultaneous
application of standard VOF techniques, together with our newly developed dispersed VOF method
for predicting growth and collapse of bubble clouds, which calculates the time dependent vapor
distribution within each computational cell. Extensive tests have been performed to demonstrate
quantitatively discretization effects of the numerical method and scaling effects of the cavitation
model. The present model neglects the viscosity of the fluid to demonstrate and to resolve large and
small scale phenomena of developed unsteady cavitation dynamics with the periodic formation of re-
entry jets, shedding and collapse of bubble clouds and the resulting hydrodynamic pressure waves.
Simulations of internal flows. as well as. external flows over NACA-0015 hydrofoils demonstrate the
sensitivity of the results against the reference location of the pressure boundary conditions and of
the damping effect of free surfaces.
5.8.1 Background and Literature Survey
Cavitation generally occurs if the pressure in some region of liquid flow drops below the vapor
pressure and, consequently, the liquid is vaporized and replaced by a ‘cavity.’ Cavitation flow is often
observed in various propulsion systems and high-speed underwater objects, such as marine
101
G¨unter H. Schnerr and J¨urgen Sauer, ”Physical and Numerical Modeling of Unsteady Cavitation Dynamics”,
ICMF-2001, 4th International Conference on Multiphase Flow, New Orleans, USA, 2001.
Figure 5.7.6 Cross section of the fluid domain for the extraction of volume fraction for Case 3
propellers, impellers of turbomachinery, hydrofoils, nozzles, injectors and torpedoes
102
. This
phenomenon usually causes severe noise, vibration and erosion. Even though cavitation flow is a
complex phenomenon which has not been completely modeled, a lot of attention has been gathered
in the CFD community as methodologies for single-phase flow has matured. Solutions of multiphase
flows by CFD methods can be categorized into three groups:
1. This group uses a single continuity equation
103
-
104
. This method is known to be unable to
distinguish between condensable and non-condensable gas
105
.
2. The next group solves separate continuity equations for the liquid and vapor phases by
adding source terms of mass transfer between phase changes. These models are usually
called homogeneous mixture models because the liquid-gas interface is assumed to be in
dynamical and thermal equilibrium and, consequently, mixture momentum and energy
equations are used.
3. The final group incorporated full two-fluid modeling, wherein separate momentum and
energy equations are employed for the liquid and the vapor phases
106
. This method is widely
used in nuclear engineering.
Cavitation can occur in a broad variety of technical devices where it usually degrades their
performance, accompanied with intense erosion of structural components and very loud noise, see
e.g. the review by
107
. Progress in understanding of cavitation phenomena is of great importance and
interest for industry. In the past, several models were developed to simulate cavitation
108
-
109
, which
do in general not model the complicated and highly transient bubble growth and collapse. This
process is responsible for the cavitation damage and therefore, the location where the bubbles
collapse is of great interest and the need for a cavitation model rises that also includes effects based
on bubble dynamics. Since hydrofoils make up so many different types of machines - pumps, turbines,
propellers- the study of as how cavitation affects hydrofoil performance is of special interest. The
type of cavitation most frequently observed at hydrofoils with a well-rounded leading edge is the so-
called traveling bubble cavitation. From experiments it can be seen that for such foils the cavitation
region is made up of individual bubbles rather than by a large vapor-filled cavity. These bubbles
originate from small cavitation nuclei (particles, air bubbles), which are already existing in the bulk
flow. The nuclei reach the low pressure region (suction peak) and grow to vapor bubbles while they
are convected downstream, supposed the static pressure is sufficiently below the vapor pressure.
Then, the bubbles are swept in the region of higher pressure and finally collapse. Many experimental
studies, point out the importance of the nuclei content of the liquid for the inception and development
102
Cong-Tu Ha, Warn-Gyu Park, and Charles L. Merkle, “Multiphase Flow Analysis of Cylinder Using A New
Cavitation Model”, Proceedings of the 7th International Symposium on Cavitation CAV2009 – Paper No. 99
August 17-22, 2009, Ann Arbor, Michigan, USA.
103
Reboud, J. L., Delannoy, Y., 1994, “ Two-phase flow modeling of unsteady cavitation,” Proc. of 2nd International
Symposium on Cavitation, Tokyo, Japan, 39-44.
104
Song, C., He, J., 1998, “Numerical simulation of cavitation flows by single-phase flow approach,” Proc. of 3rd
International Symposium on Cavitation, Grenoble, France, 295-300.
105
Kunz, R. F., Lindau, J. W., Billet M. L., and Stinebring D. R., “Multiphase CFD modeling of Developed and
Supercavitaing Flows,” Proceedings of the Von Karman Institute Special Course on Super cavitation Flows,”,
Rhode-Saint-Genese, Belgium, 2001.
106
Grogger, H. A., Alajbegovic, A., “Calculation of the cavitation flow in venture geometries using two fluid model,”
ASME Paper FEDSM 98-5295, 1998.
107
Arndt, R.E., “Cavitation in Fluid Machinery and Hydraulic Structures”, Ann. Rev. Fluid Mech., 1981.
108
Schnerr, G.H., Adam, S., Lanzenberger, K., Schulz, R, “Multiphase flows: Condensation and cavitation
problems”, Computational Fluid Dynamics REVIEW (eds. M. Hafez and K. Oshima), John Wiley & Sons, Ltd, 1995.
109
Reboud, J.L., Delannoy Y., “Two-phase flow modeling of unsteady cavitation”, Proc. 2nd Int. Symposium. on
Cavitation, Tokyo, Japan, 1994.
of cavitation. The nuclei content affects the tensile strength of the liquid and therefore is responsible
if or if not cavitation occurs at given conditions.
At the beginning clouds form a dispersed sheet attached to the solid surface, which seems to be steady
at first sight. Due to the entrainment of bubbles into the wake the sheet becomes unstable, causing
large parts of the cavity to break off. The resulting dynamics forms by interaction between the
dynamics of individual bubbles and the motion of the liquid fluid. During collapse single bubbles near
solid walls create extremely high pressure pulses which seem to responsible for erosion and
destruction, and by global (hydrodynamic) pressure waves, formed during the collapse of bubble
clouds (e.g. Brennen, 1998)
110
. The aim of the present approach is to improve understanding of the
global pressure dynamics, which is not controlled by the viscosity of the fluid.
5.8.2 Physical Modeling
Our cavitation model bases on the following physical assumptions: Cavitation is modeled as the
growth and collapse process of vapor bubbles. The bubbles originate from nuclei which already exist
in the bulk flow and grow or collapse depending on the surrounding conditions (pressure and
temperature). It is assumed, that the slip between the vapor bubbles and the liquid can be neglected.
The growth of vapor bubbles due to pseudo or gaseous cavitation is not yet taken into account.
Cavitation is assumed to be a dominated by heterogeneous nucleation, hence a homogeneous
nucleation theory, known e.g. from modeling of condensing flows is not employed. The perhaps most
important feature of the model is, that it resolves the interior dispersed structure of the bubble cloud.
From a numerical point of view, the cavitation model calculates the production (bubble growth),
destruction (bubble collapse) and convection of the vapor phase. But due to the underlying modeling
of the nuclei content, it is possible to reconstruct from the vapor content of the cell, the number of
bubbles that are currently in the cell and their radii. Therefore, a certain value of the vapor fraction
directly corresponds to a certain bubble radius R.
5.8.3 Numerical Modeling
The occurrence of cavitation leads to a two-phase flow with phase transition. Entering or leaving the
cavitation region, the mixture density jumps from the pure liquid to a much smaller value or vice
versa. To overcome problems due to a discontinuous density distribution, a special numerical
treatment is required. Front tracking methods (level set, marker particles, surface-fitting) were not
found to be suitable since they require the presence of distinct interfaces to be tracked. In this
context, here the interface is simply the bubble wall, that separates the vapor from the liquid phase.
Because of the huge number of bubbles (typically 1000 per liquid) and consequently a huge number
of interfaces to be tracked, the usage of interface tracking methods would result in enormous CPU
time and storage requirements. Instead, we prefer the usage of a front capturing method, namely the
Volume-of-Fluid technique, proposed by [Nichols & Hirt]
111
. For a detailed description of the
numerical treatment please refer to Sauer
112
(2000).
5.8.4 Modified Volume-of-Fluid Method (VOF) for Simulation of Cavitation Clouds
The Volume-of-Fluid (VOF) method tracks the motion of a certain fluid volume through the
computational domain, irrespective whether the volume contains pure liquid, pure vapor or a
mixture of vapor bubbles and liquid. Within the scope of the VOF approach, the two-phase flow is
treated as a homogeneous mixture and hence only one set of equations is used for description. The
VOF method requires in addition to the continuity and the momentum equations (which are coupled
110
Brennen, C. E., “Cloud cavitation: Observations, calculations and shock waves”, Multiphase Science and
Technology, Vol. 10., pp. 303-321, 1998.
111
Nichols, B.D., Hirt, C.W., “Calculating three-dimensional free surface flows in the vicinity of submerged and
exposed structures”. Journal of Comp. Physics, Vol. 12, pp. 343-448, 1973.
112
Sauer, J., “Instation¨ar kavitierende Str¨omungen - Ein neues Modell, basierend auf Front Capturing (VoF) und
Blasendynamik”. Ph.D. thesis (in German), University of Karlsruhe, Germany, 2000.
by a SIMPLE algorithm), the solution of a transport equation for the cell vapor fraction α which is
defined as the ratio of the vapor (gas) volume to the cell volume, (see Eq. 5.8.4),
Eq. 5.8.1
where u and v are Cartesian components of the velocity vector. The equations of motion are closed
with the constitutive relations for the density and dynamic viscosity:
Eq. 5.8.2
Here the subscripts v and l stand for the properties of pure liquid and pure vapor which are assumed
to be constant. The equations derived are general and describe the motion of two fluids with an
interface between them. As suggested by [Spalding]
113
, the continuity equation is used in its non-
conservative form:
Eq. 5.8.3
The usage of the volume fluxes rather than mass fluxes (conservative form) accounts for the
numerical advantage that the volume fluxes are continuous at the interfaces and thus simplifies the
solution of the pressure correction equation. For standard VOF applications, i.e. both fluids are
assumed to be incompressible and no phase transition takes place, the RHS of Eq. 5.8.3 reduces to
zero, meaning that the flow field is divergence-free. Care has to be taken for discretization of the
volume fraction Eq. 5.8.1. In order to avoid smearing of the interface, special methods are used to
derive the cell face values for the void fraction. For that reason, special scheme was implemented and
the code was verified by several test cases (convection tests, sloshing, dam breaking). Note that the
CICSAM scheme is employed, if there exists a discrete sharp interface to be tracked, e.g. the motion
of the free surface. In the
case of cavitation, the
vapor bubbles and hence
the vapor fraction are
homogenously
distributed in the
computational cell. A
schematic sketch of the
distribution of the
gaseous phase for a
standard VOF application
and for cavitation is
presented in Figure 5.8.1 to explain this difference. In contrast to standard VOF applications,
cavitation leads to a poly dispersed two-phase flow including phase transition. The bubbles grow and
collapse and hence change the vapor fraction in a computational cell, in addition to the convective
transport. The standard VOF method does account for convective transport, but not for phase
transition. With respect to cavitation, the void fraction α may be reformulated as follows:
113
Spalding, D.B., “A method for computing steady and unsteady flows possessing discontinuities of density”.
CHAM report 910/2, 1974.
Figure 5.8.1 Distribution of the Gaseous Phase in a
Computational
cell
Eq. 5.8.4
where Vcell the volume of the computational cell, Vv and Vl are the volumes occupied by vapor and
liquid, respectively and Nbubble is the number of bubbles in the computational cell. As a consequence
of the bubble growth process, the velocity field is no longer divergence-free ( ) and the void fraction
(Eq. 7) has to be extended by a vapor production source term:
Eq. 5.8.5
Eq. 5.8.6
The vapor production is taken into account by the source term on the right hand side of Eq. 5.8.6.
The change of the cell vapor fraction does now depend on the number of bubbles per cell volume
(RHS: 1st term) times the volume
change of a single bubble (RHS: 2nd
term) and the convective
transport. The parameter UV is
defined as the bubble
concentration per unit volume of
pure liquid. Using this definition,
the number of nuclei is explicitly
coupled to the water volume in a
cell. The physical background of
this more formal aspect is, that
relating the number of bubbles to
the water volume (rather than to
the volume of the mixture)
guarantees the conservation of the
number of bubbles. If the nuclei
grow, the vapor fraction rises and
hence the water fraction
decreases. Therefore, the number
of bubbles in the cell does also
decrease. In Figure 5.8.2 the
growth of nuclei in a cell is
schematically depicted. For the initial situation, Figure 5.8.2 left, the cell contains a large water
fraction and hence a large number of nuclei. If the nuclei grow, Figure 5.8.2 middle, they displace
water and at the same time other bubbles. Therefore, the gain of vapor fraction due to nuclei growth
is reduced by a loss of vapor fraction due to bubbles that are displaced out of the cell. Further growth,
Figure 5.8.2 right, leads to a further reduction of the number of bubbles. Since every vapor bubble
originates from a nuclei, the definition of n0 also holds for vapor bubbles. A given volume of water Vl
Figure 5.8.2 Number of Bubbles Depending on
the Water Fraction in a Computational cell
always contains N = n0Vl bubbles, the bubbles can either be nuclei of radius R = R0 or vapor bubbles
with arbitrary radius. The interested reader may refer to [Sauer]
114
for further explanation of
modeling the nuclei content of the flow. Note that for the discretization of the convection terms of
Eq. 5.8.6 the UPWIND differencing scheme is employed. This is consistent with the homogeneous
assumption. A mixture of liquid and bubbles leaves the cell, as shown in Figure 5.8.1. The
composition of the fluid volume that is convected out of the cell has the same composition than the
fluid that is currently in that cell. This physical aspect is numerically taken into account by using
UPWIND discretization. To complete the derivation of the numerical method, a relation to model the
bubble growth is needed. Under the assumptions that bubble-bubble interactions and bubble
coalescence can be neglected and that the bubbles remain spherical, the Rayleigh-Plesset equation,
see [Plesset]
115
, together with the energy equation is well suited to model the bubble growth and
collapse process:
Eq. 5.8.7
where σ is the surface tension constant of water. Note that in our model the Rayleigh-Plesset equation
can be treated as an ordinary differential equation, even when dealing with 2D or 3D flow problems,
and can e.g. be solved by a Runge - Kutta method. For details of the solution procedure we refer to
the work of [Lee et al.]
116
. If the system pressure is sufficiently low and the pressure difference pR -
pis large, the Rayleigh Eq. 5.8.8 may be considered as an adequate description for the so-called
inertia controlled bubble growth:
Eq. 5.8.8
where p(R) is the pressure in the liquid at the bubble boundary and p is the pressure in the liquid
at a large distance from the bubble. Within the scope of this model, p(R) is set equal to the vapor
pressure psat and p to the ambient cell pressure. The Rayleigh relation was used to obtain the results
presented in the following sections. To simulate cavitation in liquids others than cold water, i.e. if
thermal effects are important (organic fluids, hot water), the model is extended by a simplified
equation for the mixture enthalpy ½to account for the temperature change of the mixture caused by
cavitation. For details and compete results see [Sauer and Schnerr]
117
. The advantage of the present
modeling is the option for simultaneous application of both methods, the standard front capturing
method without phase transition and the modified VOF technique to track dispersed voids.
Numerical simulations of unsteady cloud cavitation including free surface effects are interesting
examples for simultaneous application of these two methods.
114
Sauer, J., “Instation¨ar kavitierende Str¨omungen - Ein neues Modell, basierend auf Front Capturing (VoF) und
Blasendynamik”. Ph.D. thesis (in German), University of Karlsruhe, Germany, 2000.
115
Plesset, M.S., Prosperetti, A., “Bubble dynamics and cavitation”, Annual Review of Fluid Mechanics, Vol, 1977.
116
Lee, H.S., Merte, H., “Spherical vapor bubble growth in uniformly superheated liquids”. Int. Journal of Heat
Mass Transfer, Vol. 39, No. 12, pp. 2427-2447, 1996.
117
Sauer, J., Schnerr, G.H., “Unsteady cavitation dynamics -dependence on modeling and boundary conditions”,
Proc. 2nd Japanese-European Two-Phase Flow Group Meeting, September 25-29, Tsukuba, Japan, 2000.
5.8.5 Numerical Results for Unsteady Cavitation Flow Over NACA 0015 Hydrofoil
The layout of the 2D plane test section used
by [Keller & Arndt]
118
for investigation of
the unsteady cavitation flow over a NACA
0015 hydrofoil is shown in Figure 5.8.3.
For comparison with our numerical
simulation the experiment defined by an
inlet velocity U=12 m/s, σref = 1.0 and an
angle of attack αA = 6 degrees was chosen,
because under these conditions in good
approximation a 2D periodic unsteady
cavitating flow was observed. There are
also other cases includes different
modifications concerning the numerical
pressure boundary condition. Here, the
numerical simluation yields a vortex at the
upper side of the foil. (See Figure 5.8.4
119
and [Schnerr & Sauer]
120
for complete
details.
5.8.6 Variation of Location of σref Without Free Surface
The numerical simulation bases on the following additional assumptions: The fluid is cold water at
295.15K with a nuclei concentration n0=108(nucle/m3) water and a nuclei radius R0 = 3x10-5 (m) in
order to match the experimental conditions. The inlet velocity U is set to 12m/s, the mixture is
assumed to be inviscid. The cavitation number is set constant to σref =1.0 at the reference point,
located 1.5 chord length upstream of the leading edge
121
. The series of instantaneous pictures
presented in Figure 5.8.4 shows the vapor fraction distribution during one cycle of the periodic
formation and destruction of the vapor phase. The computed frequency is f ≈ 10.94 Hz and the time
increment is Δt = 0.011 s. The vapor cavity starts growing at the leading edge and grows until a re-
entrant jets forms and breaks off a part of the cavity
122
. The first part starts to collapse and the second
part of the cavity is swept downstream. A secondary vapor region forms, merges with the already
existing vapor cloud and finally collapses. The growth and collapse of the vapor phase do significantly
alter the pressure distribution and thus change the lift and drag of the hydrofoil. The single phase
calculation yields a lift of L = 7300 N/meter span and a drag of D 0 (inviscid calculation), compared
to a time averaged lift of Lc = 200 N z and drag of Dc = 750 N under cavitation conditions. Due to
cavitation, the lift of the hydrofoil has been substantially decreased (drag increased) which is in
agreement with experimental observations of [Keller & Arndt]. Figure 5.8.4 also illustrates the
important effect on the lift which varies to about 100% within one cycle and may even become
negative after the collapse of the dispersed vapor cloud near the trailing edge. Frequency and
quantitative change of the lift up to 100% are in good agreement with the experiment. Since the
nuclei content of the flow is approximated by an average radius and an average nuclei concentration,
parameter variations have been performed to investigate the effect of the nuclei content on the time
118
Keller, A., Arndt, R.A., 1999. Private Communication.
119
Vapor Fraction Distribution and Velocity Vectors. Time increment Δt = T/8, f ≈11Hz, Lc = 0.13m, σref = 1.0,
U =12m/s, n0,re f = 108 nuclei/m3, R0,ref = 3x10-5, water at 293.15 degrees. For reference point ahead Hydrofoil.
120
G¨unter H. Schnerr and J¨urgen Sauer, ”Physical and Numerical Modeling of Unsteady Cavitation Dynamics”,
ICMF-2001, 4th International Conference on Multiphase Flow, New Orleans, USA, 2001.
121
G¨unter H. Schnerr and J¨urgen Sauer, ”Physical and Numerical Modeling of Unsteady Cavitation Dynamics”,
ICMF-2001, 4th International Conference on Multiphase Flow, New Orleans, USA, 2001.
122
See Previous.
Figure 5.8.3 Geometry and Boundary Conditions
for Simulation of Cavitation Flows*
averaged lift and drag. The simulations show, that lift and drag are rather insensitive to a variation
of the number of nuclei, although the time dependent vapor fraction distribution is quite different for
the n0 variations performed. The common fact of all simulations is, that there is one large vortex
created which is convected downstream at the suction side of the hydrofoil. This vortex controls the
Figure 5.8.4 One Cycle of the Periodic Unsteady Cavitation Flow over a NACA- 0015 Hydrofoil.
Vapor Fraction Distribution and Velocity Vectors
pressure distribution and hence affects lift and drag. The amount of vapor that is present during one
cycle is not very significant for lift and drag. [Schnerr & Sauer]
123
.
5.8.7 Interaction of Free Surface and Cavitation Dynamics
To avoid this very strong dependence on the assumption of the reference location with identical
absolute values of the static pressure, the cavitation problem is coupled with a free surface flow,
where the static pressure is constant above the liquid surface, i.e. independent of the location of the
reference point. At first, a steady state cavitation flow develops with a slight increase of the lift of
about 2% compared with single phase flow. The significant effects on the lift only dependent on the
location of the reference point and for identical values of the static pressure at this point follow
directly from the cavitation dynamics inside the test section, i.e. from the interaction of the local
vapor production, the convective transport and the resulting reaction of the velocity and pressure
field. It emphasizes the importance of appropriate boundary conditions and of the inclusion of the
dynamical interaction with the entire test circuit. For further and complete details, readers are
encourage to consult with [Sauer and Schnerr]
124
.
5.9 Case Study 9 - Distribution of 3 - Phase Flow in Vertical Pipe
Citation : Isam M. Abed , 2019. Performance Analysis, Pressure Drop and Phases-Distribution for Oil-
Water-Air Three-Phase Flow Through Vertical Pipe. Journal of Engineering and Applied Sciences, 14:
1365-1373.
DOI: 10.36478/jeasci.2019.1365.1373
URL: https://medwelljournals.com/abstract/?doi=jeasci.2019.1365.1373
The flow distribution air-water-gasoil three-phase flow in vertical 3.175 cm pipe is directly digitized
by using high speed camera
125
. These images will give full description of the flow behavior in the
fully developed region from the beginning of the Perspex pipe. Flow distribution [Abed and Al-
Turaihi, 2013] in pipe, the water phase dominates on wall of pipe of white area while the gasoil
appears in middle as a yellow areas but air-phase appears in middles as droplets of black area. At
water heating, the degree of oscillatory movement moves faster due to the viscosity and density is
less.
5.9.1 Introduction & Literature Survey
The oil-water-air flow is very common in the petroleum industry such as oil production and pipelines
flow
126
. The study of the pressure drop occurs during multiphase flow of fluid through pipes is more
complex due to more number of variables involved. More of the previous works in this area were
done when without heating process in system. These can be divided conveniently into the three-
phase substances, other parameters. Three-phase flow studied in system flowing concurrently or
123
G¨unter H. Schnerr and J¨urgen Sauer, ”Physical and Numerical Modeling of Unsteady Cavitation Dynamics”,
ICMF-2001, 4th International Conference on Multiphase Flow, New Orleans, USA, 2001.
124
Sauer, J., Schnerr, G.H., “Unsteady cavitation dynamics -dependence on modeling and boundary conditions”,
Proc. 2nd Japanese-European Two-Phase Flow Group Meeting, September 25-29, Tsukuba, Japan, 2000.
125
Isam M. Abed, “Performance Analysis, Pressure Drop and Phases-Distribution for Oil-Water-Air Three-Phase
Flow Through Vertical Pipe”, Journal of Engineering and Applied Sciences 14 (4): 1365-1373, 2019.
126
Govier, G.W. and K. Aziz, 2008. The Flow of Complex Mixture in Pipes. 2nd Ed., Society of Petroleum Engineers.
Texas, USA. ISBN:9781555631390, Pages: 792.
counter currently or in a horizontal, 90-elbow bend of R/d = 0.654) and in inclinable
127
-
128
-
129
.
Several a ranges of gas and liquid velocities, the effects of gas, liquid flow rates and Water Liquid
Ratio (WLR) and found that liquid (water and oil) thickness decreased when the gas flow rate is
increased with constant liquid flow rate and increased when the liquid flow rate is increased at
constant gas flow rate. Pressure drop increased when the gas and/or liquid flow rate is increased
130
-
131
. A new measuring method of oil-water-gas three phase flow rate by using of heat transfer and fluid
the natural gas from oil-water-gas three phase mixture. The heat transfer way is used to measure
water fraction with much more safety and has much more accuracy. There is no radiation in
measuring. This kind of three phase flow meter used in many fields
132
-
133
. The pressure drops were
independent of oil viscosity.
CFD technique used to simulate the flow distribution and pressure drop. The Volume of Fluid (VOF)
is a suitable and more efficient model used to simulate the flow of volume one phase to another. There
are several maps of average superficial phase velocities VSL against VSG for various values of f°. A
model used in simulation to predict the flow pattern and the pressure drop with high accuracy. The
objective here is to investigate numerically and experimentally the pressure-distribution, three-
phases-distribution, the effect of temperature changing on pressure along pipe and the effect of
changing the velocities of gasoil-air phases flow on temperature through vertical pipe. The
experimental data have been compared with three-phase experimental data.
5.9.2 Numerical Simulation
The problem of three phase flow consider steady state. This geometry details is accomplished by
using ANSYS Fluent 16.1. To solve CFD problem usually consists of four main components; Geometry;
Mesh generation; Setting up a physical model; Solving it and post processing the computed data. The
type of mesh depends on parameters such as flow field and geometry
134
.
5.9.3 Mixture Properties
The properties of component mixture that appearing in the equations can determined in each control
volume. n general for three system, all properties are calculated in same manner such as, the volume
fraction averaged density, viscosity given by
Eq. 5.9.1
127
Bhaga, D. and M.E. Weber, 1972. Holdup in vertical two and three phase flow Part I: Theoretical analysis.
Canad. J. Chem. Eng., 50: 323-328.
128
Spedding, P.L., E. Benard and N.M. Crawford, 2008. Fluid International Conference on CFD in the Minerals and
flow through a vertical to horizontal 900 elbow bend Process Industries, December 6-8, 1999, CSIRO, III three
phase flow. Exp. Therm. Fluid Sci., 32: Canberra, Australia, pp: 273-280.
129
Oddie, G., H. Shi, L.J. Durlofsky, K. Aziz and B. Pfeffer et al., 2003. Experimental study of two and three phase
flows in large diameter inclined pipes. Intl. J. Multiphase Flow, 29: 527-558.
130
Bhaga, D. and M.E. Weber, 1972. Holdup in vertical two and three phase flow Part I: Theoretical analysis.
Canad. J. Chem. Eng., 50: 323-328.
131
Liao, H., S. Zhou, L. Liu and F. Zhou, 2007. A new measuring method of oil-water-gas three phase flowrate by
using of heat transfer and fluid dynamics. AIP. Conf. Proc., 914: 221-225.
132
See Previous.
133
Yehuda, T., B. Dvora and A.E. Dukler. Modelling flow pattern transitions for steady upward flow through a
vertical to horizontal 900 elbow bend gas-liquid flow in vertical tubes. AIChE J, 1980.
134
Bakker, A., 2006. Applied computational fluid dynamics, mesh generation, computational fluid dynamics
lectures. Fluent Inc., Pennsylvania, USA.
5.9.4 Solving Continuity Equation
The continuity equation was solved for the volume fraction of the phases. The continuity equation
solution is accomplished the tracking of interface between phases:
Eq. 5.9.2
Where, q and p = Represent the primary and secondary phases which makes m is the mass transfer
from the pq phase p to the phase q ; m = The mass transfer from the phase q to the qp phase and Sq =
Zero or constant or user defined mass source "q” for each phase. The volume fraction is calculated
based on:
Eq. 5.9.3
5.9.5 Momentum Equation
The single momentum equation is solved:
Eq. 5.9.4
5.9.6 Energy Equation
A energy equation and shared among the phases have formed:
Eq. 5.9.5
The VOF Model treats Energy (E) and Temperature(T) as mass averaged variables:
Eq. 5.9.6
5.9.7 Boundary Conditions
The boundary conditions and
factors values used in simulation
as shown in Table 5.9.1. The water was set to be the primary phase and the secondary phase was
the (air-gasoil). The drag function between the phases was select “Schiller-Neumann” to use the fluid-
fluid drag function described in first case (Fluent User’s Guide).
5.9.8 Numerical Results
In order to find the static pressure of mixture flow through pipe compare it with the experimental
pressure sensor points were generated and the pressure was found at these points. Figure 5.9.1 (a-
d) represent the effect of water-phase temperature ( 35°C ) on pressure, and its three phases. It
observed that pressure values increases with temperature increasing. Figure 5.9.1 (b-d) show the
Table 5.9.1 Boundary Conditions – Courtesy of [I.M. Abed]
volume fraction of three-phase flow (water-gasoil-air) was used which can give a visualization of
what happened inside the pipe model at V = 0.21 m/sec, V = 0.042 m/sec water gasoil and V = 0.1757
m/sec the effect of velocities changing of gasoil-air, it observed the temperature decreases with
increasing the velocities of gasoil-air. For further details, please consult the work by [Abed]
135
.
5.9.9 Conclusion
It is observed that the pressure increases with increasing temperature. It is shown the instantaneous
pressure as a function of time. Its noted that, the increasing pressure caused increases temperature
and the pressure will drop through the pipe. The flow distribution in pipe, the water phase dominates
on wall of pipe of white area while the gasoil appears in middle as a yellow areas but air-phase
appears in middles as droplets of black area. The effect of velocities changing of gasoil-air, it observed
135
Isam M. Abed, “Performance Analysis, Pressure Drop and Phases-Distribution for Oil-Water-Air Three-Phase
Flow Through Vertical Pipe”, Journal of Engineering and Applied Sciences 14 (4): 1365-1373, 2019.
Figure 5.9.1 Distributions at 35 C – Courtesy of [I.M. Abed]
(a) Pressure
Distribution
(b) Air
Distibution
(c) Gasoil
Distribution (d) Water
Distribution
the temperature decreases with increasing the velocities of gasoil-air. The volume fraction of three-
phase flow (water-gasoil-air) was used which can give a visualization of what happened inside the
pipe model. The effect of velocities changing of gasoil-air, it observed the temperature decreases with
increasing the velocities of gasoil-air
136
.
5.10 Case Study 10 - A Study of the Impact of Mesh Configuration on 3D Fluidized
Bed Simulations
Citation : Naccarato, A. (2015). A Study of the Impact of Mesh Configuration on Three-Dimensional
Fluidized Bed Simulations.
The objective here is to study the influence of computational grid on the accuracy and efficiency of
fluidized bed simulations
137
. Due to their enhanced mixing and heat transfer characteristics, fluidized
bed systems have gained attention in a wide range of industrial applications, including power
generation, fuel synthesis and pharmaceuticals. Traditionally these systems are developed through
extensive experimental work. Laboratory-scale prototypes often exhibit different flow
characteristics than industrial scale systems, making design and optimization even more difficult and
costly. As a result, (CFD) has become a useful tool for design and optimization of these systems. An
important issue in CFD analysis of gas-solid flows in fluidized beds is the influence of mesh on the
results. This study focuses on analyzing the reliability of fluidized bed simulations as affected by
mesh configuration and resolution. Several approaches to constructing the computational grid are
discussed and the influence of mesh configuration on simulation performance and accuracy is
demonstrated. Given its capacity to handle both structured and unstructured grids, cases are
simulated via the open-source platform OpenFOAM®.
5.10.1 Introduction
Due to their increased heat and mass transfer rates and their enhanced mixing characteristics,
fluidized bed systems have gained interest in a variety of engineering applications, particularly in the
oil and gas industry
138
. Detailed understanding of processes involved in these systems is essential
for their design and performance optimization. This has proven to be a difficult and costly process,
particularly for industrial or commercial-scale systems
139
. Traditionally scale-up is done through
experimentation.
The (CFD) has been widely studied as a method to supplement experimental efforts in fluidized bed
design. Even without considering heat transfer or chemical reactions, accurate simulation of
multiphase flow systems, such as fluidized beds, present difficulties due to the dynamic nature of the
solid-fluid interactions. There are two main approaches to multiphase flow analysis: the Eulerian-
Lagrangian and Eulerian-Eulerian models. In the Eulerian-Lagrangian model, the equations of
motion are solved for each solid particle as it interacts with the continuous fluid phase and
surrounding particles. The ability to apply the Eulerian-Lagrangian model are limited due to the high
computational cost required to compute the large number of inter particle interactions. Alternatively,
the Eulerian-Eulerian model treats all solid and fluid phases as interpenetrating continua
140
.
136
Isam M. Abed, “Performance Analysis, Pressure Drop and Phases-Distribution for Oil-Water-Air Three-Phase
Flow Through Vertical Pipe”, Journal of Engineering and Applied Sciences 14 (4): 1365-1373, 2019.
137
Anthony Naccarato, “A Study of the Impact of Mesh Configuration on Three-Dimensional Fluidized Bed
Simulations”, The Department of Mechanical and Industrial Engineering, partial fulfillment of the requirements
for the degree of Master of Science in the field of Mechanical Engineering, Northeastern University, Boston,
Massachusetts, May 2015.
138
Kunii, D. and Levenspiel, O., Fluidization Engineering. Boston: Butterworth-Heinemann, 1991.
139
Van Swaaij, W. P. M., “Chemical Reactors,” in Fluidization, 2nd ed., London: Academic Press, 1985.
140
Gidaspow, D., Multiphase Flow and Fluidization. Elsevier, 1994.
Though this enables analysis of large-scale systems, it requires complex closure models to account
for particle-particle and particle-fluid interactions.
The instantaneous behavior of the flow in fluidized beds has been the subject of extensive
investigation, both experimentally and using CFD. In previous studies, both two-dimensional and
three-dimensional geometries have been considered.
Experimentally, simulations in pseudo-2D conditions have been performed
141
-
142
. The front and back
walls can be made transparent, which aids in optical analysis. Numerically, simulations of fluidized
beds require relatively fine mesh sizes to capture the solid-fluid interactions. In addition, the
unsteady nature requires a transient solver and time averaging data over a long period to properly
assess hydrodynamic characteristics. Given these factors, simulations are often performed as two-
dimensional due to the reduced computational cost. [Cranfield]
143
and [Geldart]
144
observed
differences in bubble characteristics between two- and three-dimensional fluidized beds.
[Cammarata et al.]
145
compared bubble characteristics in two- and three-dimensional simulations
and found the three-dimensional case to be more realistic. [Xie et al.] examined two- versus three
dimensional cases, noting that the differences between the two increases as the fluid velocity is
raised. [Cammarata et al. , Peirano et al.]
146
and [Xie et al.]
147
all conclude that the application of two-
dimensional analysis must be used with caution as its accuracy is highly problem dependent. Both
[Bakshi et al.]
148
and [Verma et al.]
149
simulated 3D cylindrical fluidized beds and showed good
agreement with experimental results. It becomes clear that conducting 3D analysis provides more
realistic representation of the system hydrodynamics. Furthermore as fluidized beds are most often
cylindrical, an accurate numerical case should take the wall curvature into account.
The CFD platform OpenFOAM has gained much interest in recent years. OpenFOAM is a
comprehensive CFD toolbox containing a multitude of built-in solvers and utilities. As it is open-
source, its source code library is readily customizable, making it an attractive option for research.
Numerical discretization is based on the finite volume method and allows for unstructured meshes,
enabling analysis of complex geometries. OpenFOAM also shows good parallelization performance,
making it suitable for use in cases with large number of grid points. In the present study the two-
phase solver twoPhaseEulerFoam, which has developed over several years, is applied. The solver
applies the Eulerian-Eulerian methodology and includes a number of closure model options common
to the two-fluid method. This solver is readily applicable to a two-phase fluidized bed.
The goal of this work is to assess the impact of mesh configuration as applied to three-
dimensional cylindrical fluidized beds. Due to its accommodation of unstructured meshes,
OpenFOAM (version 2.3.1) is used to implement four mesh configurations. Cases are validated against
141
Taghipour, F., Ellis, N., and Wong, C., “Experimental and Computational Study of Gas–Solid Fluidized Bed
Hydrodynamics,” Chem. Eng. Sci., vol. 60, no. 24, pp. 6857–6867, 2005.
142
Goldschmidt, M. J. V, Beetstra, R., and Kuipers, J. a M., “Hydrodynamic Modelling of Dense Gas-Fluidized Beds:
Comparison and Validation of 3D Discrete Particle and Continuum Models,” Powder Technol., vol. 142, 2004.
143
Cranfield, R. R. and Geldart, D., “Large Particle Fluidization,” Chemical Engineering Science, vol. 29, 1974.
144
Geldart, D., “The Size and Frequency of Bubbles in Two- and Three-dimensional Gas-Fluidized Beds,” Powder
Technol., vol. 4, no. 1, pp. 41–55, 1970.
145
Cammarata, L., Lettieri, P., Micale, G., and Colman, D., “2D and 3D CFD Simulations of Bubbling Fluidized Beds
Using Eulerian-Eulerian Models,” Int. J. Chem. React. Eng., vol. 1 (A48), pp. 1–19, 2003.
146
Xie, N., Battaglia, F., and Pannala, S., “Effects of Using Two- Versus Three-Dimensional Computational Modeling
of Fluidized Beds. Part II, budget analysis,” Powder Technol., vol. 182, no. 1, pp. 14–24, 2008.
147
Xie, N., Battaglia, F., and Pannala, S., “Effects of Using Two- Versus Three-Dimensional Computational Modeling
of Fluidized Beds. Part I, Hydrodynamics,” Powder Technol., vol. 182, no. 1, pp. 1–13, 2008.
148
Bakshi, A., Altantzis, C., and Ghoniem, A. F., “Towards Accurate Three-Dimensional Simulation of Dense Multi-
Phase Flows Using Cylindrical Coordinates,” Powder Technol., vol. 1, pp. 242–255, 2014.
149
Verma, V., Deen, N. G., Padding, J. T., and Kuipers, J. a. M., “Two-Fluid Modeling of Three-Dimensional
Cylindrical Gas–Solid Fluidized Beds Using the Kinetic Theory of Granular Flow,” Chem. Eng. Sci., vol. 102, 2013.
the experimental data provided by [Makkawi et al.]
150
. Comparison is done with the numerical results
generated by [Bakshi et al.] using the CFD platform MFiX. MFiX was developed at the National Energy
Technology Laboratory, particularly for multiphase flow simulation and analysi. It is commonly used
in computational fluidized bed analysis. Once a mesh-independent solution is obtained for each mesh
arrangement, their runtimes are compared as a measure of computational performance.
5.10.2 Hydrodynamic Modeling and Governing Equations
In this work the Eulerian-Eulerian model is applied to simulate the conditions given by [Makkawi
et al.]
151
. As both the solid and fluid phases are considered interpenetrating continua, the
conservation equations governing a single-fluid flow can be modified to account for the solid phase.
For this the concept of the phase volume fraction αφ of phase φ where
Eq. 5.10.1
Neglecting chemical reactions and heat transfer effects, the mass conservation of the solid and fluid
phases become
Eq. 5.10.2
Eq, 5.10.3
Where t is the time, ρ, is the density and u is the velocity vector. The subscripts g and s
represent the fluid and solid phases, respectively. Similarly, the momentum equations become
Eq. 5.10.4
where g is the gravitational acceleration vector, p is the shared pressure, ps is the particle pressure
and Ksg is the interphase drag coefficient. Both phases are treated as Newtonian fluids. The resulting
stress tensors are given by
Eq. 5.10.5
150
Makkawi, Y. T., Wright, P. C., and Ocone, R., “The Effect of Friction and Inter-particle Cohesive Forces on the
Hydrodynamics of Gas-Solid Flow: A Comparative Analysis of Theoretical Predictions and Experiments,” Powder
Technol., vol. 163, pp. 69–79, 2006.
151
Makkawi, Y. T., Wright, P. C., and Ocone, R., “The Effect of Friction and Inter-particle Cohesive Forces on the
Hydrodynamics of Gas-Solid Flow: A Comparative Analysis of Theoretical Predictions and Experiments,” Powder
Technol., vol. 163, pp. 69–79, 2006.
Eq. 5.10.6
where μ is the dynamic viscosity, λs is the solid bulk viscosity, τ is the stress tensor and I is the
identity tensor.
5.10.3 Closure Modeling
A multitude of different models have been proposed to handle the various unclosed terms in these
equations. For more information, the reader is referred to [van Wachem et al.]
152
, who provides a
comprehensive summary of many conventional models. [Verma et al.]
153
provides a study on the
impact of several closure model parameters in 3D cylindrical fluidized bed analyses. The models used
in this work are detailed in the following sections.
5.10.3.1 Drag Model
The interphase drag term
Eq. 5.10.7
is a function of the interphase drag coefficient Kgs. Several drag models have been suggested. In this
work the model proposed by [Gidaspow]
154
is used. It applies the [Ergun]
155
model for packed
regions (where αs > 0.2) and the [Wen-Yu]
156
model for dilute regions (where αs < 0.2). The resulting
drag coefficient, which combines form drag (caused by the particle size and shape) and skin drag
(caused by friction between the fluid and a particle surface) is given by
Eq. 5.10.8
where dp is the particle diameter. The drag coefficient Cd , as suggested by [Rowe]
157
, is given by
Eq. 5.10.9
where the particle Reynolds number Rep, as suggested by [Gidaspow], is defined by
152
Van Wachem, B. G. M., Schouten, J. C., van den Bleek, C. M., Krishna, R., and Sinclair, J. L., “Comparative Analysis
of CFD Models of Dense Gas–Solid Systems,” AIChE J., vol. 47, no. 5, pp. 1035–1051, May 2001.
153
Verma, V., Deen, N. G., Padding, J. T., and Kuipers, J. a. M., “Two-Fluid Modeling of Three-Dimensional
Cylindrical Gas–Solid Fluidized Beds Using the Kinetic Theory of Granular Flow,” Chem. Eng. Sci., vol. 102, 2013.
154
Gidaspow, D., Multiphase Flow and Fluidization. Elsevier, 1994.
155
Ergun, S., “Fluid Flow Through Packed Columns,” Chem. Eng. Progress, vol. 48, no. 2, pp. 89–94, 1952.
156
Wen, C. and Yu, Y., “Mechanics of Fluidization,” Chem. Eng. Prog., vol. 62, no. 62, pp. 100–111, 1966.
157
Rowe, P. N., “Drag Forces in a Hydraulic Model of a Fluidized Bed: II,” Trans. Inst. Chem. Eng., vol. 39, 1961.
Eq. 5.10.10
5.10.4 Experimental Setup
Experimental data is obtained from [Makkawi et al.]
158
, who used electrical capacitance tomography
(ECT) to obtain experimental solid volume fraction data from a cylindrical fluidized bed 13.8 cm in
diameter. Glass beads with particle diameters of 350 μm and 125 μm - classified as Geldart B and
Geldart A/B respectively
159
were tested. The static bed height used was 20 cm. Ambient air was used
for fluidization. Velocities of 0.26 m/s, 0.54 m/s (bubbling regime) and 0.80 m/s (slugging regime)
were examined. Data was averaged between heights of 14.3 and 18.1 cm. This work examines only
the bubbling regime of the Geldart B particles.
5.10.5 Numerical Setup
5.10.5.1 Simulation Parameters
Table 5.10.1 contains the simulation parameters applied to this study (Top). The solid volume
fraction is time-averaged between 5 seconds and 40 seconds, as well as summarizes the closure
models used (Bottom).
In OpenFOAM, the Srivastava-Sundaresan frictional stress model is not currently available as part of
the release. As the model combines approaches of both Johnson-Jackson and Schaeffer, which are
both available in OpenFOAM, their implementations in OpenFOAM are used to build the Srivastava-
Sundaresan model. Once the model is coded in C++ and properly structured within the
twoPhaseEulerFoam directory, the solver is re-compiled to include the new frictional stress model.
158
Makkawi, Y. T., Wright, P. C., and Ocone, R., “The Effect of Friction and Inter-particle Cohesive Forces on the
Hydrodynamics of Gas-Solid Flow: A Comparative Analysis of Theoretical Predictions and Experiments,” Powder
Technol., vol. 163, pp. 69–79, 2006.
159
Geldart, D., “Types of Gas Fluidization,” Powder Technol., vol. 7, no. 5, pp. 285–292, 1973.
Table 5.10.1 Simulation Parameters & Closure Model Summary
5.10.6 Boundary and Initial Conditions
5.10.6.1 Fluid Volume Fraction
Initially, the air volume fraction is set as 0.40 within the static bed region, or 0 ≤ y ≤ 0.20 m. Above
the static bed where no particles are present, the volume fraction is set to 1. To accomplish this in
OpenFOAM, it is convenient to set the initial fluid volume fraction to a uniform value of zero
everywhere and use the setFields utility provided by OpenFOAM to set the volume fractions of all grid
points within a specified area to a specified value. In this case, a default value of 1 is applied to the
entire cylindrical volume. Then a value of 0.40 is applied to the cylindrical region 0 ≤ y ≤ 0.20. At the
inlet, outlet and wall boundaries, the volume fraction boundary condition is set to zero gradient.
5.10.6.2 Solid Volume Fraction
Using the same procedure specified for the fluid volume fraction, the solid volume fraction is set to
0.6 within the bed region and 0 elsewhere. The same boundary conditions apply.
5.10.6.3 Pressure
The pressure throughout the cylindrical volume is set to an ambient condition of 101325 Pa. At the
outlet, the pressure remains at ambient condition. At the inlet and walls, a fixedFluxPressure
boundary condition is applied. In OpenFOAM, the pressure gradient is calculated such that the
velocity boundary condition specifies the boundary flux.
5.10.6.4 Temperature
As the case in this study is not examining heat transfer, both the air and solid temperatures are
initially set to 297 K throughout the region. Inlet and outlet air boundary conditions are also set to
297 K. At the walls, a zero gradient boundary condition is applied to the fluid phase. Zero gradient
conditions are applied to inlet, outlet and wall boundaries for the solid phase.
5.10.6.5 Granular Temperature
The granular temperature is initialized to zero. At the inlet, a fixed value of zero is applied. At the
outlet, a zero gradient condition is applied. The Johnson-Jackson boundary condition is applied at the
wall boundary.
5.10.6.6 Fluid Velocity
The fluid velocity field is initialized to 0.54 m/s. At the inlet, an interstitialInletVelocity boundary
condition is applied. In OpenFOAM, this calculates the local interstitial velocity as the specified inlet
velocity divided by the local fluid volume fraction. In this case, the specified inlet velocity is 0.54 m/s.
The volume fraction is a calculated field. At the outlet, a pressureInletOutletVelocity condition is
applied. In OpenFOAM, this boundary condition is used at boundaries where pressure is specified. It
applies a zero gradient condition to any outflow at the boundary and calculates the velocity for any
inflow at the boundary. At the wall boundary, the no-slip condition results in a fixed value of zero
velocity.
5.10.6.7 Solid Velocity
The solid phase velocity is initialized to zero. At the inlet and outlet, fixed value conditions of zero are
applied. At the wall, the Johnson-Jackson boundary condition is applied, resulting in a partial-slip
condition.
5.10.7 Domain Discretization
The flow configuration consists of a cylinder whose cross section is discretized using four grid
construction methods: cut cell, curved Cartesian, cylindrical and hybrid. The cut cell begins with a
structured Cartesian grid and uses trimmed cells around the specified boundary to conform to the
cylindrical shape. All cells outside of the boundary are removed. To accomplish this in OpenFOAM,
the cylindrical geometry is created in a .stl file and included in the case directory. A complex meshing
utility named snappyHexMesh, which is included with OpenFOAM, fits the Cartesian grid to the
boundary. The resulting grid loses some resolution of the wall boundary and creates a more complex
mesh at the wall, but retains a structured Cartesian grid away from the wall curvature. A cut cell mesh
is shown in Figure 5.10.1-(Fig 1). In the curved Cartesian grid, a structured Cartesian mesh is
specified and is fit to the cylindrical wall using a four-corner approach. In this way, the curvature of
the wall is preserved. However, very small cells are created at some points near the wall. A curved
Cartesian mesh is shown in Figure 5.10.1-(Fig 2). The cylindrical mesh is well-suited to handle the
cylindrical geometry studied in this work as it maintains the wall curvature. A cylindrical mesh is
shown in Figure 5.10.1-(Fig 3). A hybrid mesh is also examined using a five-block o-grid type
topology. It applies a structured mesh in the center of the domain and blends into a cylindrical mesh
around the wall. A hybrid mesh is shown in Figure 5.10.1-(Fig 4).
5.10.8 Approach
To compare the grid geometries, a mesh independent solution is sought for each construction
method. The accuracy of the different mesh arrangements are discussed individually. The mesh
independent resolutions for each arrangement are then re-run using 24 Intel Xeon CPU E5-2680
2.8GHz processors. Computing resources were available through the Northeastern University high
performance computing Discovery Cluster. Results are presented in the following section.
Figure 5.10.1 Different Meshing Topologies
5.10.9 Result
5.10.9.1 Fluidized Bed Behavior
Figure 5.10.2 Instantaneous Void Fraction
The fluid volume fraction, often referred to as the void fraction, is used to study the gas-solid flow
Figure 5.10.3 Three-Dimensional Iso-Surfaces of Void Fraction (αg= 0.7)
dynamics within fluidized beds. Instantaneous void fraction profiles for the curved Cartesian, cut cell
and cylindrical grids are shown in Figure 5.10.2. Slices are taken at θ = 0°. Three-dimensional
contours of the void fractions are shown in Figure 5.10.3. Here, contours of αg = 0.7 are shown. As
Figure 5.10.4 Time-Averaged Void Fraction
the small bubbles rise through the height of the bed, they interact and coalesce, forming larger voids.
Figure 5.10.4 shows time averaged void fractions. Again, slices are taken at θ = 0°. As previously
mentioned, the solid volume fraction is time averaged from 5 seconds to 40 seconds. The results are
typical for bubbling fluidized beds. The effect of near-wall interactions are clearly visible in Figure
5.10.4. The partial-slippage of the particle phase results in particles collecting more along the
cylindrical wall. As they rise and coalesce, bubbles are forced toward the centerline of the bed. From
these profiles, it is seen that although there are variations in the instantaneous bubble dynamics
predicted via different meshes, the mean fields are almost insensitive to the choice of mesh
configuration. However, the mean void fraction exhibits considerable variation in azimuthal
direction.
5.10.10 Mesh Sensitivity Studies
5.10.10.1 Curved Cartesian
Figure 5.10.5 shows the grid resolution study for the curved Cartesian mesh method. In general, the
predictions from OpenFOAM compare favorably with the experimental data. As the mesh is refined,
the centerline void fraction decreases and the solution deviates from the experimental data. However
this behavior is consistent
with the Cartesian cut cell
results from MFiX. Based
on the results the 27x27
grid is chosen for further
analysis.
5.10.10.2 Cut cell
Similar results are
obtained for the curved
Cartesian mesh method.
Similar to the curved
Cartesian method, the cut
cell method also under-
predicts the centerline
void fraction.
5.10.10.3 Cylindrical
For the cylindrical mesh,
both radial and azimuthal
studies were performed and show the impact of the radial and azimuthal grid resolutions
respectively. The cylindrical grids show predictions closer to the experimental data than those of the
cut cell and curved Cartesian shown in previous sections. The azimuthal resolution does not have a
significant impact on the results. The radial resolution however has significant impact, primarily in
the center region of the bed. A grid resolution of 18 radial and 40 azimuthal cells is used for
performance evaluation.
5.10.10.4 Hybrid
For the hybrid o-grid type mesh, the azimuthal and radial results from the cylindrical mesh study are
used. Using the azimuthal resolution from the cylindrical study, a center section grid spacing of 13
azimuthal cells per quadrant is used, resulting in a 13x13 center section. This also dictates that 13
azimuthal cells per quadrant be used, resulting in 52 azimuthal cells. Using the radial spacing from
the cylindrical study results in 10 cells radially in the outer section. The results for this mesh are
provided in the following section.
Figure 5.10.5 Curved Cartesian Grid Resolution
5.10.11 Mesh Geometry Efficiency
Table 5.10.2 summarizes the meshes chosen to evaluate performance. These cases were then run
on 24 processors each using the same computing cluster. Before discussing the efficiency, the
resulting predictions o bed characteristics are discussed.
The void fraction profiles are shown in Figure 5.10.6. The solutions provided by each mesh
arrangement are very similar. The cut cell has the most deviation from the experimental results at
the centerline, but still shows reasonably good agreement. To examine the void fraction from a
slightly different perspective, the time averaged void fraction along the height of the cylinder at the
centerline is shown in Figure 5.10.7. This provides a sense of the bed height predicted by the
simulations.
The profile exhibited by all the mesh arrangements is characteristic of a bubbling fluidized bed.
Though some variation is seen in the bed region (where the solid phase is present), all the mesh
arrangements show good agreement in the predicted height of the bed. The pressure drop across the
Figure 5.10.6 Void Fractions for Mesh Efficiency (Sensitivity) Study
Table 5.10.2 Computational Performance Candidates
cylinder height is given in
[Naccarato]
160
. As with the
void fraction, the values are
taken from the cylinder
center. The predictions show
negligible difference. As with
the void fraction, the cut cell
configuration deviates the
most, but still shows
reasonable agreement with
the other meshes.
Figure 5.10.7 also serve to
show that, for grid
independent solutions, the
analyzed mesh construction
methods predict very similar
behavior in terms of time
averaged void fraction,
pressure drop and solid
velocity. The fact that the grid
independent solutions produce similar results shows consistency in the OpenFOAM analysis. In the
resolution studies, it was shown that the mesh has a significant impact on accuracy and performance
of the solution.
As a mesh independent solution is sought, the predictions become independent of the grid
construction method. However, the important issue is that the rate of convergence to grid
independent solution, and thus computation time, are different for various meshing strategies. In
addition, the grid sizes of the mesh independent solutions vary greatly. To evaluate the
computational performance of each mesh arrangement, the mesh independent solutions were
recalculated using the computational
resources discussed. Table 5.10.3
provides the run times for the mesh
independent cases. Given the
decrease in cells in the hybrid mesh, it
is logical that it would have the fastest
runtime. In terms of computational
service units, the difference in
runtimes has a significant impact on
the cost of a fluidized bed simulation.
5.10.12 Conclusion
This study concentrates on 3D fluidized bed simulations and how they are affected by the
computational grid chosen to model the system. The Eulerian-Eulerian formulation, discussed in
the Section 3.10.2, is employed to describe the gas-solid flow in fluidized beds. Simulations are
carried out in OpenFOAM. To evaluate the accuracy of the predictions, void fraction profiles are
analyzed. Resolution studies are performed for curved Cartesian, cut cell and cylindrical meshes. For
the cylindrical mesh, both radial and azimuthal resolutions are considered. Using grid independent
160
Anthony Naccarato, “A Study of the Impact of Mesh Configuration on Three-Dimensional Fluidized Bed
Simulations”, The Department of Mechanical and Industrial Engineering, partial fulfillment of the requirements
for the degree of Master of Science in the field of Mechanical Engineering, Northeastern University, Boston,
Massachusetts, May 2015.
Figure 5.10.7 Axial Time-Averaged Void Fraction
Table 5.10.3 Computational Performance
solutions found in the resolution studies, the computational performance of the grid configurations
are compared against each other.
It is shown that significant savings in terms of computational cost can be realized by choosing
an efficient mesh arrangement. In the case of this work, for a cylindrical fluidized bed, a hybrid o-
grid type mesh produces results similar to those obtained by other meshes, but with a much faster
runtime. A future extension of this work is to conduct simulation of two-phase reacting flow in
fluidized beds. Such extension is useful to study coal and biomass combustion and gasification. Due
to the computational cost of such simulations, it is essential to investigate the impact of domain
decomposition method on parallel computational efficiency for various mesh configurations. For
further information, please consult the [Naccarato]
161
.
161
Anthony Naccarato, “A Study of the Impact of Mesh Configuration on Three-Dimensional Fluidized Bed
Simulations”, The Department of Mechanical and Industrial Engineering, partial fulfillment of the requirements
for the degree of Master of Science in the field of Mechanical Engineering, Northeastern University, Boston,
Massachusetts, May 2015.
5.11 Case Study 11 - Cavitation Characteristics Around a Sphere: An LES
Investigation
Authors : [Mohammad-Reza Pendar and Ehsan Roohi]
162
Article In : International Journal of Multiphase Flow, August 2017.
Citation : Mohammad-Reza Pendar, Ehsan Roohi, Cavitation characteristics around a sphere: An LES
investigation, International Journal of Multiphase Flow, Volume 98, 2018, Pages 1-23, ISSN 0301-9322,
https://doi.org/10.1016/j.ijmultiphaseflow.2017.08.013.
Here we examine partial and super cavitation over a sphere at a constant Reynolds number of 1.5
×106 and a broad range of cavitation numbers (0.36 < σ < 1). Large eddy simulation (LES) and Sauer
mass transfer model were used to simulate the dynamic and unsteady cavitation around the sphere.
Also, the com- pressive volume of fluid (VOF) method is used to track the cavity interface. The two-
phase flow solver of the OpenFOAM package, intephaseChangeFoam is employed. Large-eddy
simulation of cavitating flow over the sphere is compared with the non-cavitating flow at the same
Reynolds number. This work provides a thorough understanding of the fluid dynamic characteristics
of the sphere cavitation such as vorticity field, turbulent kinetic energy, pressure, velocity,
streamlines and boundary layer. Also, detailed analyses of the instantaneous cavity leading edge and
separation point location, vortex shedding, streamwise velocity fluctuation and evolution of the
cavity are reported. Characteristics of the wake of the cavitating flows are compared with the single-
phase results. We report that cavitation suppresses instability in the near wake region and delays the
three-dimensional breakdown of the vortices. The volume fraction con- tours of the cavity cloud
obtained from the numerical simulations are compared with the experimental data at the same
working condition with a suitable quantitative accuracy.
5.11.1 Introduction
Cavitation is attributed to the formation of vapor when the local liquid pressure becomes lower than
its saturated vapor pressure. Cavitation is considered as an unsteady, three-dimensional,
discontinuous or periodic, multiphase and complex physical phenomenon. Cavitation often happens
in hydraulic devices such as turbines, pumps, pipe systems, fuel injectors, underwater vehicles,
submarine, hydrofoils and marine propeller blades as a basic property of the liquid. A dimensionless
number, cavitation number, is
Eq. 5.11.1
categories cavitation, where Pv is the vapor pressure, ρ is the liquid density, and P∞ , U∞ are the free
stream flow pressure and velocity, respectively. Depending on the value of the cavitation number,
several cavitation regimes were reported in liquid flows, i.e.: incipient cavitation, shear cavitation,
sheet/cloud cavitation, and super cavitation.
In the cloud cavitation, the formation, detachment, and collapse of unsteady or periodic sheet cavities
occur around the cavitating body. Cloud cavitation with its unsteady nature has considerable
consequences on hydraulic and marine equipment, including un- steady behaviors, noise, vibration,
and erosion. Super cavitation occurs due to increased velocity of the moving body and consists of a
long and steady cavity region. It can decrease the drag of an underwater high-speed moving body,
thus enabling it to move with a quite higher speed under the water. In general, cloud and super-
cavitation attracted the attention of several researchers during the past and recent decades.
Numerical and experimental investigations of cavitating flow are of great interest to researchers
162
Mohammad-Reza Pendar, Ehsan Roohi, “Cavitation characteristics around a sphere: An LES investigation”,
International Journal of Multiphase Flow, August 2017.
during the past few years. For example, [Franc and Michel]
163
studied the role of the un- steady cavity
closure and re-entrant jet formation in the cloud cavitation. [Brandner et al.]
164
, investigated cloud
cavitation around a sphere experimentally at Re = 1.5 ×106 with cavitation numbers varying between
0.36 and 1.0. They investigated the instantaneous location of the cavity leading edge, separated
laminar boundary layer, shedding mechanism, and shedding frequency. [Shang et al.]
165
(2012)
performed numerical simulations of cavitating flow over a sphere using the Large Eddy Simulation
(LES) approach together with a mixture assumption and a finite rate mass transfer model. However,
they just compared a 3D view of the volume fractions contours of the vapor phase with the
experimental data [Brandner et al.]
166
, at the same working condition. [Roohi et al.]
167
simulated
super cavitating flows over a hydrofoil using the LES approach and the Volume of Fluids (VOF)
technique.
5.11.2 Literature Survey
Ji et al. (2013) simulated cavitating turbulent flow around hydrofoils using the Partially-Averaged
Navier–Stokes (PANS) method and a suitable mass transfer cavitation model. The predicted cavity
characteristic compared well with the experimental data. Shang (2013) simulated cavitation around
the cylindrical submarine. He used K-ω SST turbulence model with VOF method and Sauer mass
transfer model to capture the details of the cavitation mechanisms within broad ranges of cavitation
numbers. Ji et al. (2014) numerically investigated the structure of the cavitating flow around a
twisted hydrofoil using a mass transfer cavitation model and a modified RNG k-ε model with a local
density correction for turbulent eddy viscosity. Cavity structures and the shedding frequency agreed
fairly well with experimental observations. [Yu et al.]
168
simulated the dynamic evolution of
cavitation over 3D geometries using the LES and k −ε turbulence approaches as well as VOF technique
with the Kunz mass transfer model. [Chen et al]
169
considered the collapse regimes of the cavitation
on the submerged vehicles with a constant deceleration. [Roohi et al.]
170
considered cavitating and
super cavitating flow behind a 3D disk with specific emphasis on detailed comparisons of the various
turbulence and mass transfer models. [Cheng et al.]
171
investigated the unsteady cavitating turbulent
flow around twisted hydrofoil using Zwart cavitation model combined with a filter-based density
correction model (FBDCM). Their numerical results simulated the entire process of cavitation
shedding including the re-entrant jet accurately in comparison with the experimental data.
163
Franc, J.P. , Michel, J.M. , 2004. Fundamentals of Cavitation. Kluwer.
164
Brandner, P.A. , Walker, G.J. , Niekamp, P.N. , Anderson, B. , An experimental investigation of cloud cavitation
about a sphere. J. Fluid Mech. 656, 147–176, 2010.
165
Shang, Z. , Emerson, D.R. , Xiaojun, G.U. ,Numerical investigations of cavitation around a high speed submarine
using OpenFOAM with LES. Int. J. Com. Methods , 1250040–1250054, 2012.
166
Brandner, P.A. , Walker, G.J. , Niekamp, P.N. , Anderson, B. . An investigation of cloud cavitation about a sphere.,
16th Australasian Fluid Mechanics Conference, Crown Plaza. Gold Coast, Australia, pp. 1392–1398 ,2007.
167
Roohi, E. , Zahiri, A.P. , Passandideh-Fard, M. , Numerical simulation of cavitation around a two-dimensional
hydrofoil using VOF method and LES turbulence model. Appl. Math. Modell. 37, 6469–6488, 2013.
168
Yu, X. , Huang, C. , Du, T. , Liao, L. , Wu, X. , Zheng, Z. , Wang, Y. , 2014. Study of characteristics of cloud cavity
around axisymmetric projectile by large eddy simulation. J. Fluids Eng. 136 (May), 1–8 .
169
Chen, Y. , Lu, C. , Chen, X. , Cao, J. , 2015. Numerical investigation on the cavitation collapse regime around the
submerged vehicles navigating with deceleration. Eur. J. Mech. B Fluids 49, 153–170 .
170
Roohi, E. , Pendar, M.R. , Rahimi, A. , 2016. Simulation of Three-dimensional cavitation behind a disk using
various turbulence and mass transfer models. Appl. Math. Modell. 40, 542–564.
171
Cheng, H.Y. , Long, X.P. , Ji, B. , Zhu, Y. , Zhou, J.J. , 2016. Numerical investigation of unsteady cavitating turbulent
flows around twisted hydrofoil from the Lagrangian viewpoint. J. Hydrodyn. 28 (4), 709–712 .
[Gnanaskandan and Mahesh]
172
-
173
studied sheet to cloud cavitation transition over a wedge at Re =
200,000 and σ = 2.1. The frequency of the shedding process, mean pressure and velocity fluctuations
were reported accurately. [Luo et al.]
174
summarized the recent progress for the cavitation study in
the hydraulic machinery including turbo pumps and hydro turbines. [Wang et al.]
175
studied unsteady
cloud cavitation around complex geometries experimentally and numerically. They reported
unsteady evolutions of the cavity and re-entry jet from both experimental and numerical results.
[Gnanaskandan and Mahesh] used the homogeneous mixture model to study cavitation over a
circular cylinder at various Reynolds numbers and cavitation numbers. Cavitation is reported to
considerably influence the evolution of pressure, boundary layer, and loads on the cylinder surface.
Also, the effects of an initial void fraction, vorticity dilatation, and wake characteristics were assessed.
[Pendar and Roohi]
176
reported a correlation between the cavity length and diameter with the
cavitation number of the hemispherical head-form bodies. Also, they presented a detailed
comparison be- tween different turbulence and mass transfer models over a broad range of
cavitation numbers, especially very low cavitation numbers around a 3D hemispherical head-form
body and a conical cavitation. Numerical cavitation models are classified into several categories;
among them, two-phase flow methods are the most popular ones. [Kubota et al.]
177
presented a model
constructed on the Rayleigh-Plesset equation called bubble two-phase flow (BTF) model that depicts
cavitation by expressing the evolution of bubble radius as a function of the local pressure. [Merkle et
al.]
178
, [Kunz et al. (2000), Yuan et al. (2001) and Singhal et al. (2002a, b )] derived efficient cavitation
models based on semi-analytical formulas. In their models, phase change sources are related to the
difference of local pressure and vapor pressure. [Schnerr and Sauer]
179
and [Frobenius et al.]
180
improved the model by deriving more complex relations among the bubble radius and local pressure.
There is an increased tendency to use large eddy simulations (LES) to simulate cavitating flow. LES
accurately captures details of eddies in large-scale. Also, it can capture the details of small- scale flow
structures in a cavitating flow. LES regularly allows for medium-scale to small-scale energy transfer
that can capture flow mechanisms with much details for accurate prediction of the cavitation
phenomenon. In recent years, many researchers have been adopted LES method and obtained
promising results ( Wang and Ostoja-Starzewski, 2007; Bensow and Bark, 2010; Dittakavi et al., 2010;
Hu et al., 2014; Gnanaskandan and Mahesh, 2015; Ji et al., 2015 )]. The volume of Fluids (VOF)
method was extensively used to capture the vapor boundary in the cavitating flows. For instance,
172
Gnanaskandan, A. , Mahesh, K. , 2016a. Numerical investigation of near-wake characteristics of cavitating flow
over a circular cylinder. J. Fluid Mech. 790, 453–491 .
173
Gnanaskandan, A. , Mahesh, K. , 2016b. Large eddy simulation of the transition from sheet to cloud cavitation
over a wedge. Int. J. Multiphase Flow 83, 86–102 .
174
Luo, X.W. , Ji, B. , Tsujimoto, Y. , 2016. A review of cavitation in hydraulic machinery. J. Hydrodynamic .
175
Wang, Y. , Wu, X. , Huang, C. , Wu, x. , 2016. Unsteady characteristics of cloud cavitating flow near the free
surface around an axisymmetric projectile. Int. J. Multiphase Flow 85, 48–56 .
176
Pendar, M.R. , Roohi, E. , 2016. Investigation of cavitation around 3D hemispherical head-form body and
conical cavitators using different turbulence and cavitation models. Int. J. Ocean Eng. 112, 287–306.
177
Kubota, A. , Kato, H. , Yamaguchi, H. , 1992. A new modeling of cavitating flows: a numerical study of unsteady
cavitation on a hydrofoil section. J. Fluid Mech. 240, 59–96 .
178
Merkle, C.L. , Feng, J.Z. , Buelow, P.E.O. , 1998. Computational modeling of the dynamics of sheet cavitation. In:
Proceedings of the 3rd International Symposium on Cavitation. Grenoble, France .
179
Sauer, J. , 2000. Instationaren Kaviterende Stromung-Einneues Modell, baserend auf Front Capturing (VOF)
and Blasendynamik (Ph.D. thesis). University of Karlsruhe .
180
Frobenius, M. , Schilling, R. , Bachert, R. , Stoffel, B. , 2003. Three-dimensional, unsteady cavitation effects on
a single hydrofoil and in a radial pump – measurements and numerical simulations, partial two: numerical
simulation. In: Proceedings of the 5th International Symposium on Cavitation. Osaka, Japan .
[Passandideh Fard and Roohi]
181
; Shang (2013); [Roohi et al.]
182
; [Yu et al. (2014) and Kim and Lee
(2015)] used the VOF technique to capture cavitation interface over different sets of geometries
accurately.
As our literature survey shows, even though there are a few studies considering experimental
investigations of cavitating flows over the sphere, i.e., [Brennen (1970), Tassin Leger, Bernal and
Ceccio (1998) and Tassin Leger and Ceccio (1998)] , there are almost no studies considering a
detailed numerical consideration of cavitating flow over the sphere. In this research, we extend our
studies to consider the cavitating flow over a sphere using an open source package, that is,
OpenFOAM. Results are compared with the experimental data [Brandner et al., 2010] in details. To
simulate cavitating flows, we use Sauer mass transfer model in conjunction with the LES turbulence
approach that captures certain mechanisms of cavitation. A compressive velocity form of the VOF
technique is employed to track the interface between the liquid and vapor phases. This research
provides a detailed set of results for the cavitating flows around the sphere such as evolution of the
vortex flow structure, analysis of the cavity leading edge and separation point location as well as the
behavior of pressure, velocity field, vorticity and turbulent kinetic energy around the sphere. Flow
field characteristics are compared with the single-phase results at the same Reynolds number.
According to our literature survey, none of the results mentioned above were reported in previous
studies of the cavitating flows around the sphere.
5.11.3 Numerical Method
5.11.3.1 Governing Equations
Incompressible Navier–Stokes equations for a homogeneous mixture multiphase flow are given as
follows:
Eq. 5.11.2
A multiphase flow modeling should be used to describe a phase change from liquid to vapor that
happens under cavitation. In this study, we consider a “two-phase mixture” method. The method uses
a local vapor volume fraction transport equation together with a source term for the rate of mass
transfer between the two phases due to cavitation as follows:
Eq. 5.11.3
The mixture density ρ and viscosity μ are computed as follows:
Eq. 5.11.4
5.11.3.2 Volume of Fluid Model
A compressive volume of fluid (VOF) method is adopted to track the interface between the vapor and
liquid phases. Where γ is de-fined as follows:
181
Passandideh-Fard, M. , Roohi, E. , 2008. Transient simulations of cavitating flows using a modified volume-of-
fluid (VOF) technique. Int. J. Comput. Fluid Dyn. 22, 97–114 .
182
Roohi, E. , Zahiri, A.P. , Passandideh-Fard, M., 2013. Numerical simulation of cavitation around a two-
dimensional hydrofoil using VOF method and LES turbulence model. Appl. Math. Modell. 37, 6469–6488 .
Eq. 5.11.5
In the VOF equation used in OpenFOAM package, a compressive-velocity (vc) is introduced:
Eq. 5.11.6
where vc is the compressive velocity term suggested in [Rusche]
183
. The last term in Eq. 5.11.6 is
just active at the interface and considered as a surface compression term, see [Roohi et al.]
184
;
[Klostermann et al.]
185
, for more details of the compressive velocity VOF technique.
5.11.3.3 Large Eddy Simulation
The construction of large eddy simulation (LES) turbulence approach is based on computing the large
scale structures that are determined on the computational grid, whereas the smaller sub grid eddies
are modeled. Any variable, i.e. ,f, is separated into grid scale (GS) and sub grid scale (SGS)
components, i.e., where ¯f = G f is the GS component, G = G ( x , Δx) is the filter function, and also Δ =
Δ (x) is the filter width. The filtered Navier–Stokes equations ( Eq. 5.11.2) are given by:
Eq. 5.11.7
Unresolved transport term in the momentum equation, i.e., sub- grid scale stress tensor, τij , can be
decomposed as [Bensow and Fureby]
186
:
Eq. 5.11.8
Prevalent sub grid modeling approaches utilize an eddy or sub- grid viscosity, μk , where μk can be
calculated using a wide variety of approaches. In eddy-viscosity model we have,
Eq. 5.11.9
where Sij is the rate-of-strain tensor for the resolved scale and the sub grid scale turbulent viscosity,
183
Rusche, H. , 2002. Computational Fluid Dynamics of Dispersed Two-Phase Flows at High Phase Fractions (Ph.D.
thesis). Imperial College, University of London .
184
Roohi, E. , Zahiri, A.P. , Passandideh-Fard, M. , 2013. Numerical simulation of cavitation around a two-
dimensional hydrofoil using VOF method and LES turbulence model. Appl. Math. Modell. 37, 6469–6488 .
185
Klostermann, J. , Schaake, K. , Schwarze, R. , 2013. Numerical simulation of a single rising bubble by VOF with
surface compression. Int. J. Numer. Methods Fluids 71 (8), 960–982 .
186
Bensow, R.E. , Fureby, C. , 2007. On the justification and extension of mixed methods. LES J. Turbul. 8, N54 .
μk, is closed by a “Local Eddy-Viscosity” model. Here, the “one equation eddy viscosity model
”(OEEVM) sub grid scale is used. To obtain turbulence kinetic energy k, OEEVM solves the following
equation:
Eq. 5.11.10
Sub grid scale turbulent viscosity, μk is then computed by:
Eq. 5.11.11
while cε and ck are set as 1.048 and 0.094 in OpenFOAM, respectively.
5.11.3.4 K- ω SST Turbulence Model
In addition to LES, we used K- ω shear stress transport (SST) turbulence model. [Menter]
187
mixed
the K- ω model for the near- wall region and K- ε model for the far field regions. The new model was
called as K- ω SST turbulence model. In this model, turbulence kinetic energy and specific dissipation
rate are computed as follows:
Eq. 5.11.12
The model coefficients such as α3 , β3 , σk3 , σω3 are linear combinations of the corresponding
coefficients of the K- ω and modified K- ε turbulence models, and defined in [Pendar and Roohi]
188
.
5.11.3.5 Mass Transfer Modeling
We used two mass transfer models, i.e., Sauer model and Kunz model. Sauer derived a mass transfer
model given by Eq. 5.11.13 [Sauer]
189
; [Schnerr and Sauer]
190
:
Eq. 5.11.13
187
Menter, F.R.. Two-equation eddy-viscosity turbulence models for engineering applications. AIAAJ, 1994.
188
Mohammad-Reza Pendar, Ehsan Roohi, “Cavitation characteristics around a sphere: An LES investigation”,
International Journal of Multiphase Flow, August 2017.
189
Sauer, J. , 2000. Instationaren Kaviterende Stromung-Ein neues Modell, baserend auf Front Capturing (VOF)
and Blasendynamik (Ph.D. thesis). University of Karl-sruhe .
190
Schnerr, G.H. , Sauer, J. , 2001. Physical and numerical modeling of unsteady cavitation dynamics. In:
Proceedings of 4th International Conference on Multiphase Flow. New Orleans, USA .
Sauer model is a function of the bubble diameter and number of bubbles per unit volume. In Eq.
5.11.13 , Rb is supposed to be equal for all the bubbles:
Eq. 5.11.14
In the interChangePhaseFoam solver, the initial number of bubbles ( n0 ) is set as 1.6 ×109 . [Schnerr-
Sauer] mass transfer model does not consider the interaction of bubbles, transfer of local mass-
momentum and non-spherical bubble geometries. The model is drained from the Rayleigh–Plesset
equation considering the force balance over spherical bubbles. This characteristic is important in the
prediction of accurate cavity cloud, especially in the super cavitating flow [ Wu et al.]
191
2005 ). [Kunz
et al.]
192
suggested a semi-empirical cavitation model. This model is one of the most widely-employed
mass transfer models implemented in the OpenFOAM. The production and destruction process of the
liquid phase is defined with two different terms:
Eq. 5.11.15
The first term on the right-hand side states production of the vapor phase and is proportional with
the pressure departure from the vapor pressure. The second term takes into account condensation
and is proportional to the third power of the volume fraction. Empirical constants of Cdest and Cprod
are set as 1000 and 75 in
OpenFOAM; respectively. The
characteristic time scale is defined
as
Eq. 5.11.16
Kunz mass transfer model
reconstructs the re- entrant jet
and interface of the cavity with a
suitable accuracy, especially in the
cavity closure point.
5.11.4 Numerical Setup
5.11.4.1 The
interPhaseChangeFoam
Validation for
Cavitation
Before presenting the results of
cavitating flows over the sphere,
the accuracy of the employed
numerical solver is investigated
191
Wu, J. , Wang, G. , Shyy, W. , 2005. Time-dependent turbulent cavitating flow computations with interfacial
transport and filter-based models. Int. J. Num. Methods Fluids 49, 739–761 .
192
Kunz, R.F. , Boger, D.A. , Stinebring, D.R. , Chyczewski, T.S. , Lindau, J.W. , Gibeling, H.J. , 2000. A preconditioned
Navier–Stokes method for two-phase flows with application to cavitation. J. Com. Fluids 29, 849–875 .
Figure 5.11.1 Cp Distribution Over the Hemisphere Head-Form
Body at σ = 0.2
with the experimental and numerical data. We evaluate the accuracy of the interPhaseChangeFoam
solver in simulating a variety of incompressible, turbulent, cavitating flows. For validation purposes,
we consider cavitation over two different cases: a hemispherical nose-shaped bluff body and a disk
cavitation. We compare our LES results with the experimental data of [Rouse and McNown (1948])
and Final Technical Report NAVSEA Hydro ball is- tics Advisory Committee (1975), respectively. The
diameter of the hemisphere and disk are D . Reynolds numbers for the hemispherical head-form
body, and disk cavitation are considered as 4.4×106 and 2.8×104, respectively, and the cavitation
numbers vary be- tween 0.1–0.2.
Figure 5.11.1 compares the time-averaged Cp distribution with the experimental data of [Rouse and
McNown (1948)]; a suitable agreement is observed. It also indicates the suitability of the scheme in
predicting bluff-body partial cavitation. The dynamics of cavitating flow strongly depends on the
employed turbulence approach, which is handled by either of the LES and k-ω SST models. Numerical
results are compared suitably with the analytical relations and experimental data.
5.11.4.2 Discretization and Code Validation
Table 5.11.1 provides details of the employed discretization scheme used in obtaining the results
reported in the current study. Second order accuracy is considered for discretization of all terms in
the continuity and momentum equations. To access the accuracy of the employed numerical scheme
to evaluate inertial scales of the flow field, the power spectrum density (PSD) of the drag coefficient
fluctuations of the cavitating flow at σ = 0.5 and non-cavitating flow around the sphere at the same
free-stream Reynolds number are contrived in Figure 5.11.2. One point should be reminded here
that the local Reynolds number around the cavitating sphere may fall to around 3.1×103 due to vapor
formation at the cavity region, this reduced local Reynolds number results in not a very distinct
inertial range. Usually, the inertial range is evident for high Reynolds number flows where a clear
scale separation exists, i.e., the non-cavitating case.
5.11.4.3 Pressure-Velocity Coupling: PIMPLE Algorithm
The velocity-pressure coupling is performed using the PIMPLE algorithm, which is a hybrid of PISO
and SIMPLE employed in the OpenFOAM. Like SIMPLE and PISO, the PIMPLE scheme consists of three
parts:
• momentum predictor
• pressure solver
• momentum corrector.
In the PIMPLE algorithm an outer correction loops, i.e., cycling over a given time step for a number of
iterations, and equation under-relaxation between outer correctors are allowed for stability, as
shown in Figure 5.11.3. If no outer corrector loops are used, the algorithm is the same as the PISO
algorithm. PIMPLE solver also includes dynamic time- stepping (automatic time step adjustment to
Table 5.11.1 Summary of Discretization Schemes used
hold a constant CFL number) [Robertson et al.]
193
. The PIMPLE algorithm enables a more robust
pressure–velocity coupling by coupling a SIMPLE outer-corrector loop with a PISO inner-corrector
loop. This algorithm shows a better numerical stability for larger time-steps or higher Courant
number compared to PISO. Here, we employed two PISO iterations and one SIMPLE iteration.
193
Robertson, E. , Choudhury, V. , Bhushan, S. , Walters, D.K. , 2015. Validation of OpenFOAM numerical methods
and turbulence models for incompressible bluff body flows. J. Com. Fluids 123, 122–145 .
Figure 5.11.2 The Power spectrum density (PSD) analysis for the drag coefficient over the sphere for
cavitating at σ = 0.5 and non-cavitating flow.
5.11.4.4 The Sphere Problem
Figure 5.11.4 shows a schematic of the computational domain and illustrates the boundary
conditions imposed on the domain for the sphere test case. The mean flow is spatially uniform along
the x- axis and the sphere is placed at the center of the water tunnel at the origin. The diameter of the
sphere is 0.15 m. All cases were simulated based on the data of Australian Maritime College’s Tom
Fink Cavitation Tunnel [Brandner et al., 2010 ], a closed recirculating variable-pressure water tunnel.
The test section has a size of 0.6 m ×2.6m, and a constant velocity U∞ is specified at the in- flow
Figure 5.11.3 Flowchart of the PIMPLE solution procedure
boundary at 9 m/s. A reference static pressure p ∞ is used to adjust the cavitation number. The
spherical surface is specified as no-slip wall condition. Details of the tunnel set-up and operation are
given in [Brandner et al. (2004)] . Here, the most relevant non-dimensional parameters are Reynolds
(Re = ρU ∞ D/μ) and cavitation numbers ( σ = (P − Pϑ ) / 0.5 ρU2∞ ). In all cases, a Reynolds number
of Re = 1.5 ×106 was considered. The fluid properties are specified as:
Eq. 5.11.17
5.11.4.5 Grid Sensitivity
Analysis
The quality of the computational
grid has a direct influence on the
accuracy of numerical results. The
grid convergence for the cavity
length and diameter is reported in
Table 5.11.2 based on the
computations at σ = 0.5 for four
sets of grids. The grid spacing near
the surface of the sphere is of the
same size in all three directions.
The table indicates that Grid 3
with around 5×106 cells provides a
converged solution for the cavity
characteristic. Thus, the
simulations reported in this paper
are obtained using Grid 3. In this
grid, the normalized wall distance
Figure 5.11.4 Computational domain and boundary conditions
Figure 5.11.5 The structured meshes around the sphere
of the first layer of grid nodes near the wall is 6.236×10–4. As Figure 5.11.5 illustrates, structured
quadrilateral meshes were utilized. Simulations were performed as 3D even though the sphere
geometry is axisymmetric. It is because the flow is three-dimensional and unsteady due to the vortex
shedding behind the body at the investigated Reynolds/cavitation numbers. The grid size is
progressively increased in other regions, where the variations of flow proportion are comparatively
lower. For a typical simulation case at σ = 0.5; mean values of y+ are 2.19 and 5.73, and minimum
values of y+ are around 0.205 and 0.425 for Grid-4 and Grid-3, respectively. Results and Discussion
5.11.4.6 Comparison with the Experiments
In this section, the relatively stable, three-dimensional and un- steady cavities over the sphere are
simulated at various cavitation number regimes. The numerical results are compared with the
experimental result of [Brandner et al.], who studied cavitation at Re = 1.5 ×106 with a σ ranging from
1.0 to 0.36. In the case of an extremely unsteady cavity, the unsteadiness affects the entire cavity up
to its detachment. However, the condition is entirely different at smaller cavitation numbers, i.e.,
cavity clouds are short and relatively thin at large cavitation numbers, and the unsteadiness is
confined in a relatively limited region so that the cavity cloud can be considered as stable at least
from a large scale view. Figure 5.11.6 illustrates 3D views of the cavitating flow past the sphere
over a broad range of cavitation numbers, i.e., 0.1 ≤ σ ≤1.0 compared with a series of low-speed
Figure 5.11.6 3D views of cavity cloud (iso surface of the vapor volume fraction) over the sphere at
various cavitation numbers: experimental results taken by the low-speed photographer, Re = 1.5 ×10 6 (
Brandner et al., 2010 ) (right frames), numerical result- LES/Sauer models (left frames), numerical
result- LES/Sauer models for super cavitating flow (two last frames).
photographic images of cavitation which is obtained from experimental data [Brandner et al., 2010].
All numerical results except one frame are obtain using Grid 3. Comparison of Grid 3 and Grid 4
predictions for the cavity shape at σ= 0.5 shows no sensible difference between both solutions. As
Figure 5.11.6 indicates, there are suitable quantitative agreements between the current numerical
solutions with those of the experiment, demonstrating that the numerical method can handle
cavitating flows over the sphere.
5.11.4.7 Cavitation Regimes
Figure 5.11.7 depicts formation and development of the cloud cavity. Cavitation behavior can be
categorized in three different regimes based on how the cavity is shed into the sphere wake: At high
cavitation numbers (0.95 < σ < 1.0), a small, stable cavity cloud with breakup due to the re-entrant
jet is formed. Cavitation inception was observed to occur near φ=93 ◦at σ=1. Experimental studies of
[Achenbach]
194
at the same Reynolds number showed that transition in single phase flow over the
sphere appears to occur in attached flow around ϕ= 95 ◦, with turbulent separation taking place near
ϕ = 120°. Therefore, the boundary layer at the cavity separation point is laminar; however; the
expansion of the cavity bubbles results in boundary layer separation [Arndt et al.]
195
. As depicted in
Figure 5.11.7 a, at σ= 1.0, a stable cavity is formed just over the sphere surface with Lcav = 0.16 D in
length. At lower cavitation numbers (0.4 < σ < 0.9), a moderate length cavity cloud is established
which is sufficient enough for the formation of the reentrant jet. Cavity breakup occurs followed by a
vortex shedding in the cavity cloud. As depicted in Figure 5.11.7b, the instabilities of the cavity with
194
Achenbach, E. , 1972. Experiments on the flow past spheres at very high Reynolds numbers. J. Fluid Mech. 54.
195
Arndt, R.E. , Song, C.C.S. , Kjeldsen, M. , He, J. , Keller, A. , 2001. Instability of partial cavitation: a
numerical/experimental approach. 23rd Symposium on Naval Hydrodynamics ISBN: 978-0-309-25467-0 .
Table 5.11.2 Grid sensitivity study on the cavity length and diameter (σ = 0.5)
a cyclic shedding increases. In very low cavitation number, i.e. σ < 0.4, an extended super cavity cloud
forms without any considerable re-entrant jet or large-scale breakup, as shown in Figure 5.11.7c.
Cavity closure occurs downstream of the sphere in the liquid at the super caveating regime.
Figure 5.11.7 The depiction of three different modes of cavitation around the sphere from the inception
cavitation to super cavitation, left: numerical data, right: experimental images ( Brandner et al., 2010 ).
5.11.4.8 Turbulent Kinetic Energy in the Cavity
5.11.9 presents nine consecutive frames of temporal variation of the cavity cloud captured during
one complete cavitation cycle at σ = 0.1. The right side images illustrate a 2D view of the volume
fractions of the vapor phase in the mid-plane (solid black line) colored by turbulent kinetic energy
(TKE). The left side frames demonstrate the iso-surfaces of the volume fractions. t indicate the
dimensionless time defined as t = t U∞/D. The typical periodical time of the cavity required to reach
the maximum length is about t = 18 at σ = 0.1. Owing to a growing re-entrant jet, the cavity starts
decreasing in length at t = 20.4.
However, the first breakdown occurs near the bottom of the sphere at t = 6. This could be attributed
to the accumulation of re-entrant jet fluid interacting with the cavity sheet. The cavity sheet on the
sphere starts decreasing in size (t = 8.4), and fully vanishes (t = 10.8) due to the emission of the
collapse front, which is the positive pressure wave emanating from the initial accumulation of re-
entrant jet [Brandner et al.]
196
. The other frames also indicate that re-entrant jet movement is non-
axisymmetric. The new cavity sheet starts to appear and grow again, i.e., t = 13.2, which is the
196
Brandner, P.A. , Clarke, D.B. , Walker, G.J. , 2004. Development of a fast response probe for use in a cavitation
tunnel. 15th Australasian Fluid Mechanics Conference. The University of Sydney, Sydney, p. 4 .
Figure 5.11.8 Nine consecutive frames of temporal variation of the cavity cloud
periodic characteristic of the cavity clouds evolution past a sphere. This right-frame figures
demonstrate that inside the cavity is close to laminar condition while high density of the turbulent
kinetic energy variations are concentrated above the leading edge of the cavity clouds on the surfaces
of the sphere where the transition to turbulence occurs in the shear layer, near the outer inter- face
of the cavity, cavity closure regions, re-entrant jet and the sub- sequent wake.
The strongest effect is observed on the re-entrant jet interaction with the cavity interface. These
statements are in agreement with the observation of [Ahuja et al.]
197
on cavitating flow over blunt
bodies. Frames of t = 18 and t = 20.4 show that the terminal section of the evacuated regions inside
197
Ahuja, V. , Hosangadi, A. , Arunajatesan, S. , 2001. Simulations of cavitating flows using hybrid unstructured
meshes. J. Fluids Eng. 123, 331340 .
5.11.9 Time evolution of cavitation patterns obtained from the simulation, left: 3D contours of vapor
volume fraction, right: in plane cavity boundary (solid line) and flood contours of turbulence kinetic
energy (TKE), LES, Sauer, σ = 0.1.
the cavity, where the re-entrant jet condensed the vapor, also experiences a high level of turbulence
kinetic energy.
5.11.4.9 Cavity Leading Edge
As Figure 5.11.10 (a–b) illustrate the fluid behavior and locations of the separation point are
different in the single and multi- phase flow. The figure compares cavitating (σ = 0.45) and non-
cavitating flow at Re = 1.5 ×106 with the same outlet pressure. For single-phase flow, as reported by
[Achenbach], the flow transition occurs around ϕ= 95 °in the supercritical regime, i.e., 4×105 < Re <
1.5 ×106 approximately, while the turbulent separation point in the supercritical regime takes places
near ϕ = 120°.
The separation point remains nearly constant below and above Re = 1.5×106 . The location of the
boundary layer separation and
formation of detached shear layer in
the cavitating flow (σ = 0.45) is
closer to the leading edge stagnation
point, i.e., it occurs at 96 °,
corresponding to X/D = 0.044, in
comparison with the single- phase
flow, which takes place at around
118°, corresponding to X/D = 0.23.
At σ = 0.45, cavity starting point is
located at 76°, confirming that
boundary layer is laminar at the
cavity inception point and the
separation point and the separation
point of the shear layer moved aft in
multiphase flow condition.
However, in the experimental data
reported in [Arakeri, 1975;
Ramamurthy and Bhaskaran, 1977;
Brandner et al., 2010], the cavity inception point is reported to be located after the separation point.
A similar observation to our numerical results was reported in the simulation reported in
[Gnanaskandan and Mahesh, 2016]. This discrepancy is due to the use of a homogeneous mixture
Figure 5.11.10 (a , b) separation point for cavitating (Left frame) and non-cavitating flows (right
frame)
(a) Boundary Layer Seperation Point
(ϕ≈96 and Cavity Inceptopn Point
ϕ≈76)
(b) Boundary Layer Seperation Point
(ϕ≈118) For a single Phase Flow
Figure 5.11.11 Formation of the re-entrant jet (red lines) at
different cavitation numbers. (For interpretation of the
references to color in this figure legend, the reader is referred
to the web version of this article.)
model in the numerical simulations and the lack of nucleation and bubble dynamics in the employed
model. In our model, cavitation starts once the pressure falls below the vapor pressure, while in real
words cavitation does not start instantly at the place where the pressure drops below pv , but it
happens downstream of the separation point.
5.11.4.10 Re-Entrant Jet Analysis
Figure 5.11.11 compares re-entrant jet behavior at various cavitation numbers, i.e., σ = 0.7, 0.5 and
0.2. The blue and red solid lines illustrate boundary of the cavity cloud and velocity streamlines,
respectively. Our results show that cavity length becomes sufficient enough for a re-entrant jet to
form at σ= 0 . 9; this directly affects the breakup of the sheet cavity. Initial breakdown typically occurs
at about mid length of the cavity, at several circumferential sites from which fronts emanate; the
sheet cavity then breaks down into cavitating filaments. For cavitation numbers between 0.8 and 0.5,
where re-entrant jet phenomena dominate and shed- ding is most coherent, the mechanism for sheet
cavity breakdown to cloud cavitation can be easily seen. At σ = 0.5, cavity lengths have grown to about
two sphere diameters. The reentrant-jet behavior becomes dominant and tends to be more
Figure 5.11.12 Comparison of different turbulence models (LES/ k- ω SST): Instantaneous volume
fraction contours
axisymmetric, causing nearly simultaneous breakdown of the entire sheet cavity circumference. For
σ = 0.2 the cavity length becomes so large that the re-entrant jet barely reaches the sphere. With the
plunging of the re-entrant jet fluid, only the bottom of the sheet cavity is affected. Occasionally
sufficient re-entrant jet fluid accumulates to cause a short breakdown of the sheet cavity.
5.11.4.11 LES vs. k- ω SST Approach
Figure 5.11.13 demonstrates 3D views of the cavity cloud behind the sphere. As is clearly identified
in this figure, the LES solution suitably captures the unsteady vapor shedding of the cavity behind the
sphere. This observation is in agreement with the experimental results, while k- ω SST provides a
time-averaged solution. Figure 5.11.12 shows volume fraction contours of LES and k- ω SST
approach. The k- ω SST is unable to model the instabilities of the cavity accurately while it predicts a
thick re- entrant jet.
5.11.4.12 Vorticity and Velocity Fields
Generally speaking, the effective Reynolds number decreased inside the cavity as the working fluid
and velocity changed in the void. Moreover, vorticity dilatation is reported to play a vital role in this
reduction [Gnanaskandan and Mahesh]. Fluid expansion occurs at the cavity inception point
compared to a non-cavitating condition which subsequently activates vorticity dilatation. The
dilatation term, i.e., ω(. v), which is due to volumetric expansion/contraction, alongside the
baroclinic torque, i.e., (1/ρ2m )( ρm × p) , which represents the generation of vorticity due to
misaligned pressure and density gradients, are zero at non-cavitating conditions. It is worth
Figure 5.11.13 Comparisons of the velocity streamlines of cavitating flow with the non-cavitating flow
conditions
mentioning that vorticity dilatation is present even in incompressible cavitating flows simulations,
since phase change is accompanied by a change in density, hence divergence, i.e., at the steady state,
Eq. 5.11.2 reads:
Eq. 5.11.18
At the cavity inception, pressure becomes a
function of density and vapor volume fraction,
which results in more vorticity production in
the shear layer due to the baroclinic torque
contributions; however, as the negative of the
dilatation term contributes in vorticity
production, an extended region of positive
vorticity dilatation behind the sphere (shown
by red color in frame c) results in a lower
vorticity magnitude around the sphere.
However, a negative dilatation (blue color) is
stretched out further behind the sphere over
the cavity interface. Frames in Figure
5.11.13 compare the vorticial region in
cavitating and non-cavitating flows at the same
working condition. Evidently, cavity formation
spreads the reverse flow region while it decreases the vortex strength. Hence the formation of vapor
suppresses turbulence effects in the sphere wake.
5.11.4.13 Features of the Cavitating Flow
The mean values of the water volume
fraction are plotted in Figure 5.11.15. As
the cavitation number decreases, the
minimum of αmean decreases. The figure
indicates that a decrease in the cavitation
number from 0.45 to 0.36 drastically
increases the mean vapor fraction at 65° < φ
< 80 °, but the void fraction decreases as the
reentrant jet hits the sphere surface.
Contours of the mean and the instantaneous
void fractions are illustrated and compared
(see [Pendar and Roohi]
198
) as 2D sections in
the z plane at different cavitation numbers
from LES/Sauer results. The difference in
mean and instantaneous vapor volume
fraction contours is due to the difference of
mean and instantaneous pressures. At σ =
1.0, the instantaneous cavitation inception
region is observed to appear near ϕ ≈ 95
°and gets a stable form about 0.12D in length.
Even though the high-density liquid is
198
Mohammad-Reza Pendar, Ehsan Roohi, “Cavitation characteristics around a sphere: An LES investigation”,
International Journal of Multiphase Flow, August 2017.
Figure 5.11.15 Distribution of the mean values of
water volume fraction at various cavitation numbers
Figure 5.11.14 Comparisons of mean pressure
coefficient over a broad range of cavitation number
present near the back of the sphere in the instantaneous frame, the mean cavity extends in the whole
vorticial regions behind the sphere, i.e., the length of the average cavity is more than 0.5D. As the
cavitation number decreases, the instantaneous and mean cavity sizes approach together. However,
the cavity breakup due to re-entrant jet movement does not permit the instantaneous cavity to
remain attached to the surface at the rear of the sphere. Mean cavity frames indicate that cavity is
asymmetric, and vapor concentration is higher inside the vortices at all cavitation numbers. For
additional info, please consult the [Pendar &Roohi]
199
.
Figure 5.11.14 shows the mean pressure coefficient distribution on the sphere surface at various
cavitation numbers. As the flow accelerates, the pressure coefficient decreases to its minimum value
at approximately 70–73° from the frontal stagnation point. It then in- creases as the flow decelerates
in the adverse pressure gradient region, terminated by flow separation. This region is followed by
an- other constant and slight pressure reduction region (100°−140° at high cavitation numbers) in
the cavity region. Subsequently, pressure increases as the flow approaches 180°, which is attributed
to the formation of the second stagnation point due to either reverse vortex or re-entrant jet flow
contact with the sphere surface.
5.11.5 Conclusions
We simulated cavitation around the sphere numerically and compared the results with experimental
data, where applicable. Simulations were performed under the framework of OpenFOAM over a broad
range of cavitation numbers. Cavitating and non- cavitating flow were compared with each other in
details at the same working conditions. LES turbulence approach was utilized and pressure
coefficients, streamwise velocity fluctuation, separation point location, cavity leading edge, temporal
evolution of the cavity, vortex shedding and mean volume fraction are reported. Numerical
prediction of the cavity interface showed a suitable ac- curacy in comparison with the experimental
data. The contours of turbulent kinetic energy (TKE) were examined, and high density of TKE was
found at the cavity interface, separated shear layer and re-entrant jet interaction with the cavity
interface. The mean and instantaneous void fractions were compared, and distinctive pat- terns,
especially at higher cavitation numbers, were observed. Vorticity dilatation is found to be a major
parameter in affecting the vorticity in the wake of the multi-phase flow. Also, it is found that
occurrence of the cavitation effectively reduces the Reynolds number in the near wake and
suppresses turbulence. For additional information, please consult the work by [Pendar and Roohi]
200
.
199
See Above.
200
Mohammad-Reza Pendar, Ehsan Roohi, “Cavitation characteristics around a sphere: An LES investigation”,
International Journal of Multiphase Flow, August 2017.
