in FL U ID F LO W A N D H EA T T R A N SF ER S IM U LA TIO N S F O R C O M PL EX I N D U ST R IA L A P PL IC A TIO N S 2018 ISBN 978-91-7485-415-2 ISSN 1651-4238 Address: P.O. Box 883, SE-721 23 Västerås. Sweden
Address: P.O. Box 325, SE-631 05 Eskilstuna. Sweden E-mail: info@mdh.se Web: www.mdh.se
From Reynolds averaged Navier-Stokes towards smoothed particle hydrodynamics
Mälardalen University Press Dissertations No. 282
FLUID FLOW AND HEAT TRANSFER SIMULATIONS
FOR COMPLEX INDUSTRIAL APPLICATIONS
FROM REYNOLDS AVERAGED NAVIER-STOKES TOWARDS SMOOTHED PARTICLE HYDRODYNAMICS
Md Lokman Hosain 2018
Copyright © Md Lokman Hosain, 2018 ISBN 978-91-7485-415-2
ISSN 1651-4238
Mälardalen University Press Dissertations No. 282
FLUID FLOW AND HEAT TRANSFER SIMULATIONS FOR COMPLEX INDUSTRIAL APPLICATIONS
FROM REYNOLDS AVERAGED NAVIER-STOKES TOWARDS SMOOTHED PARTICLE HYDRODYNAMICS
Md Lokman Hosain
Akademisk avhandling
som för avläggande av teknologie doktorsexamen i energi- och miljöteknik vid Akademin för ekonomi, samhälle och teknik kommer att offentligen försvaras fredagen den 14 december 2018, 13.00 i Delta, Mälardalens högskola, Västerås. Fakultetsopponent: Professor Moncho Gomez Gesteira, University of Vigo
Abstract
Optimal process control can significantly enhance energy efficiency of heating and cooling processes in many industries. Process control systems typically rely on measurements and so called grey or black box models that are based mainly on empirical correlations, in which the transient characteristics and their influence on the control parameters are often ignored. A robust and reliable numerical technique, to solve fluid flow and heat transfer problems, such as computational fluid dynamics (CFD), which is capable of providing a detailed understanding of the multiple underlying physical phenomena, is a necessity for optimization, decision support and diagnostics of complex industrial systems. The thesis focuses on performing high-fidelity CFD simulations of a wide range of industrial applications to highlight and understand the complex nonlinear coupling between the fluid flow and heat transfer. The industrial applications studied in this thesis include cooling and heating processes in a hot rolling steel plant, electric motors, heat exchangers and sloshing inside a ship carrying liquefied natural gas. The goal is to identify the difficulties and challenges to be met when simulating these applications using different CFD tools and methods and to discuss the strengths and limitations of the different tools. The mesh-based finite volume CFD solver ANSYS Fluent is employed to acquire detailed and accurate solutions of each application and to highlight challenges and limitations. The limitations of conventional mesh-based CFD tools are exposed when attempting to resolve the multiple space and time scales involved in large industrial processes. Therefore, a mesh-free particle method, smoothed particle hydrodynamics (SPH) is identified in this thesis as an alternative to overcome some of the observed limitations of the mesh-based solvers. SPH is introduced to simulate some of the selected cases to understand the challenges and highlight the limitations. The thesis also contributes to the development of SPH by implementing the energy equation into an open-source SPH flow solver to solve thermal problems. The thesis highlights the current state of different CFD approaches towards complex industrial applications and discusses the future development possibilities.
The overall observations, based on the industrial problems addressed in this thesis, can serve as decision tool for industries to select an appropriate numerical method or tool for solving problems within the presented context. The analysis and discussions also serve as a basis for further development and research to shed light on the use of CFD simulations for improved process control, optimization and diagnostics.
“Essentially, all models are wrong, but some are useful”
– George E. P. Box
Acknowledgements
The research in this PhD thesis was conducted at the Future Energy Center, Mälardalen University, Västerås, Sweden, with financial support from The Knowledge Foundation, SSAB, ABB, Mälarenergi and Eskilstuna Energi & Miljö.
My first and foremost thanks go to my main supervisor Prof. Rebei Bel-Fdhila for his continuous and invaluable guidance, support, suggestions and inspiration throughout this thesis work.
I would like to acknowledge my co-supervisor Prof. Konstantinos Kyprian-idis, Prof. Erik Dahlquist and Dr. Hailong Li for their guidance and support during my thesis work. Many thanks to Prof. Emeritus Dan Loyd and Dr. Jan Sandberg for reviewing this PhD thesis and providing valuable comments and suggestions.
I am very thankful to Alex J. C. Crespo and Jose M. Domínguez from the University of Vigo, Spain for hosting me and supporting me during the imple-mentation of the thermal models in the open-source SPH code DualSPHysics. My special thanks go to my colleagues and friends at my department for many fruitful discussions.
Finally, I would like to show my deepest gratitude to my beloved wife Nupur Akther; without her support this PhD would have been impossible. I would also like to thank my sister-in-law Fahima Akther for all the mental support and inspiration from the first day I arrived in Sweden. I would also like to show gratitude towards my parents for all the inspiration I received from them during my studies.
Md Lokman Hosain
October, 2018. Västerås, Sweden.
Summary
The energy demand and environmental impacts from the industrial sector are growing concerns within the European Union (EU) due to the need to comply with the strict energy and environmental policy. Optimal process control can significantly enhance energy efficiency of heating and cooling processes in many industries. Process control systems typically rely on measurements and so called grey or black box models that are based mainly on empirical correla-tions, in which the transient characteristics and their influence on the control parameters are often ignored. A robust and reliable high-fidelity numerical technique, to solve fluid flow and heat transfer problems, such as computa-tional fluid dynamics (CFD), which is capable of providing a detailed under-standing of the multiple underlying physical phenomena, is a necessity for optimization, decision support and diagnostics of complex industrial systems. There are several different options within CFD methods and tools, however, choosing the right numerical tool to solve advanced engineering problems, and particularly in industrial research and development (R&D) is often diffi-cult, and the consequences of choosing the wrong tool can be very costly. This thesis deals with several energy-intensive complex industrial applications. The goal is to identify the difficulties and challenges to be met when simulating these applications using different CFD tools and methods and to discuss the strengths and limitations of the different tools.
The thesis focuses on performing high-fidelity CFD simulations of a wide range of industrial applications to highlight and understand the complex nonlinear coupling between the fluid flow, heat transfer and other phenomena inherent to the investigated processes, e.g. combustion or induced transients. The industrial applications studied in this thesis include the runout table (ROT) cooling process and slab reheating furnace in a hot rolling steel plant, rotating machines such as electric motors and generators, heat exchangers and sloshing inside a ship carrying liquefied natural gas (LNG). The mesh-based finite volume CFD solver ANSYS Fluent is employed to acquire detailed and accurate solutions of each application and to highlight challenges and limitations. The limitations of conventional mesh-based CFD tools are exposed when attempting to resolve the multiple space and time scales involved in large industrial processes. They are not capable of addressing the multiple jet impingement on a fast-moving strip that we encounter in the ROT cooling process, and are often only partly successful, as in the slab reheating furnace. Therefore, a mesh-free particle method, smoothed
particle hydrodynamics (SPH) is identified in this thesis as an alternative to overcome some of the observed limitations of the mesh-based solvers. SPH is introduced to simulate some of the selected cases to understand the challenges and highlight the limitations.
The thesis also contributes to the development of SPH by implementing the energy equation into an open-source SPH flow solver to solve thermal problems. The comparison between the solutions from finite volume and SPH methods presented in this thesis clearly indicates their strengths and limita-tions for different types of problems. The thesis highlights the current state of different CFD approaches towards complex industrial applications and dis-cusses the future development possibilities.
The overall observations and the hypothesis, based on the industrial prob-lems addressed in this thesis, can serve as decision tool for industries to select an appropriate numerical method or tool for solving problems within the pre-sented context. The analysis and discussions also serve as a basis for further development and research to shed light on the use of real-time CFD simula-tions for improved process control, optimization and diagnostics.
Sammanfattning
Energibehovet och miljöpåverkan från industrisektorn är växande problem inom Europeiska unionen (EU) på grund av behovet av att följa den stränga energi- och miljöpolitiken. Optimal processstyrning kan avsevärt förbättra energieffektiviteten hos uppvärmnings- och kylprocesser i många industrier. Styrsystem för processer baserar sig vanligtvis på mätningar och så kallade gray- eller black-box modeller som huvudsakligen bygger på empiriska ko-rrelationer, där de tillfälliga egenskaperna och deras påverkan på kontroll-parametrarna ofta ignoreras. En robust och tillförlitlig numerisk teknik, för att lösa fluidflöde och värmeöverföringsproblem, så som Computational Fluid Dynamics (CFD), som kan ge en detaljerad förståelse för de olika underlig-gande fysikaliska fenomenen, är en nödvändighet för optimering, beslutsstöd och diagnostik av komplexa industriella system. Det finns flera olika alter-nativ inom CFD-metoder och verktyg, men det är ofta svårt att välja rätt nu-meriska verktyg för att lösa avancerade tekniska problem, särskilt inom indus-triell forskning och utveckling, och konsekvenserna av att välja fel verktyg kan vara mycket kostsamma. Avhandlingen behandlar flera energiintensiva komplexa industriella applikationer. Målet är att identifiera de svårigheter och utmaningar som behöver överkommas när man simulerar dessa applikationer med hjälp av olika CFD-verktyg och -metoder och att diskutera styrkor och begränsningar hos de olika verktygen.
Avhandlingen fokuserar på att utföra CFD-simuleringar för ett brett spektrum av industriella applikationer för att belysa och förstå den komplexa olinjära kopplingen mellan fluidflöde, värmeöverföring och andra inneboende fenomen för de undersökta processerna, t.ex. förbränning eller inducerade transienter. De industriella applikationer som studeras i denna avhandling inkluderar kylning av tunna stålplåtar och uppvärmning av stålskivor vid varmvalsning inom stålindustrin, roterande maskiner som elmotorer och generatorer, värmeväxlare och skvalpning i tankar inuti transportfartyg för flytande naturgas. Den nätbaserade CFD-lösaren ANSYS Fluent har använts för att få detaljerade och noggranna lösningar för varje applikation och för att identifiera utmaningarna och begränsningarna. Begränsningarna hos konventionella nätbaserade CFD-verktyg avslöjas när lösningar söks för multipla rums- och tidsskalor som ingår i stora industriella processer. De är inte kapabla att hantera de multipla jetstrålar på en rörlig stålplåt som vi stöter på i kylprocessen av stålplåtar och ofta är de endast delvis framgångsrika, till exempel för industriella värmeugnar. Därför identifieras
en nätfri partikelmetod, Smoothed Particle Hydrodynamics (SPH) i denna avhandling som ett alternativ för att övervinna några av de observerade begränsningarna hos nätbaserade lösare. SPH används i denna avhandling för att simulera några av de utvalda fallen för att förstå utmaningarna och belysa begränsningarna.
Avhandlingen bidrar också till utvecklingen av SPH genom att implementera energiekvationen i en SPH-flödeslösare, med öppen källkod, för att kunna lösa termiska problem. Jämförelsen mellan lösningarna från nätbaserade och SPH metoder som presenteras i denna avhandling visar tydligt på metodernas styrka och begränsningar för olika typer av problem. Avhandlingen belyser nuvarande CFD-metoder för komplexa industriella applikationer och diskuterar framtida utvecklingsmöjligheter.
De övergripande observationerna och hypotesen, baserad på de industriella problem som behandlas i denna avhandling, kan fungera som beslutsverktyg för industrier i att välja en lämplig numeriskt metod eller verktyg för att lösa problem inom den presenterade kontexten. Analysen och diskussionerna utgör också grunden för vidareutveckling och forskning för att belysa användningen av CFD-simuleringar i realtid för förbättrad processkontroll, optimering och diagnostik.
List of Papers
This thesis is based on the following papers, which are referred to in the text by their Roman numerals:
I Hosain, M. L., Bel Fdhila, R., Daneryd, A., 2015. Heat transfer by liquid jets impinging on a hot flat surface. Appl. Energy 164, 934-943. II Hosain, M. L., Bel Fdhila, R., Sand, U., Engdahl, J., Dahlquist, E., Li,
H., 2016. CFD Modeling of Real Scale Slab Reheating Furnace, in: 12th International Conference on Heat Transfer, Fluid Mechanics and Thermodynamics, HEFAT2016.
III Hosain, M. L., Fdhila, R.B., 2015. Literature Review of Accelerated CFD Simulation Methods towards Online Application. Energy Procedia 75, 3307-3314.
IV Hosain, M. L., Bel Fdhila, R., Rönnberg, K., 2017a. Taylor-Couette flow and transient heat transfer inside the annulus air-gap of rotating electrical machines. Appl. Energy 207, 624-633.
V Hosain, M. L., Fdhila, R.B., 2017. Air-Gap Heat Transfer in Rotating Electrical Machines: A Parametric Study. Energy Procedia 142, 4176-4181.
VI Hosain, M. L., Rönnberg, K., Bel Fdhila, R., 2017b. Air Flow inside Rotating Electrical Machines: A Comparison between Finite Volume and SPH Method. NAFEMS World Congress, NWC17.
VII Hosain, M. L., Sand, U., Fdhila, R.B., 2018. Numerical Investigation of Liquid Sloshing in Carrier Ship Fuel Tanks. IFAC-PapersOnLine 51-2, 583-588.
VIII Hosain, M. L., Bel-Fdhila, R., Kyprianidis, K., 2018. Simulation and validation of flow and heat transfer in an infinite mini-channel using Smoothed Particle Hydrodynamics. Energy Procedia 00, 00-00. (Ac-cepted for publication)
IX Hosain, M.L., Domínguez, J.M., Crespo, A.J.C., Bel-Fdhila, R., Kypri-anidis, K., 2018. Smoothed Particle Hydrodynamics modeling of tran-sient conduction and convection heat transfer. (Journal Manuscript)
Part of this thesis (Paper I, II and III) was previously included in the Licentiate thesis “Towards Accelerated Simulations for Fluid Flow and Heat Transfer of Large Industrial Processes” (Hosain, 2016).
Contents
Page 1 Introduction . . . 1 1.1 Background . . . 1 1.2 Research challenges . . . 3 1.3 Research framework . . . 51.4 Objective of the thesis . . . 6
1.5 Contributions to knowledge . . . 7 1.6 Thesis outline . . . 8 2 Literature Review . . . 10 3 Methodology . . . 15 3.1 Modelling approach . . . 15 3.2 Different approaches in CFD . . . 16 3.2.1 Governing equations . . . 17
3.2.2 Energy transport equation . . . 18
3.2.3 Mixture fraction transport equation . . . 18
3.3 Mathematical Models for RANS . . . 18
3.3.1 RANS transport equations . . . 18
3.3.2 Turbulence transport equations . . . 19
3.3.3 Energy transport equation . . . 20
3.3.4 Volume of Fluid (RANS-VOF) . . . 21
3.4 Mathematical Models for SPH . . . 21
3.4.1 SPH form of the governing equations . . . 22
3.4.2 Pressure formulation . . . 23
3.4.3 Boundary conditions . . . 23
3.4.4 SPH thermal implementation . . . 24
3.5 Industrial applications addressed using RANS . . . 24
3.5.1 Hot rolling process . . . 25
3.5.2 Rotating machines . . . 30
3.5.3 LNG vessels in carrier ships . . . 32
3.6 Industrial applications addressed using SPH . . . 33
3.6.1 Rotating machine . . . 34
3.6.2 LNG vessel in carrier ship . . . 34
3.6.3 Transient heat conduction . . . 34
3.6.4 Transient heat convection . . . 36
4 Results and discussion . . . 39
4.1.1 Hot rolling process . . . 39
4.1.2 Rotating machines . . . 45
4.2 Smoothed Particle Hydrodynamics . . . 48
4.2.1 Rotating machines . . . 48
4.2.2 LNG vessel in carrier ships . . . 49
4.2.3 Heat conduction . . . 52
4.2.4 Heat convection . . . 54
4.3 Discussion . . . 56
5 Summary of appended papers . . . 62
6 Conclusions . . . 67
7 Future work . . . 69
References . . . 71
Appendix . . . 79
List of Tables
Page
1.1 Relation between the papers and the research questions . . . 5
3.1 Mesh information for the FVM models . . . 33
3.2 Tank sloshing case specifications . . . 35
List of Figures
Page Figure 1.1: Schematic showing the relationship between the research
topics and the papers. . . 5
Figure 2.1: Hierarchical classification of methods in CFD . . . 11
Figure 3.1: Methodological approach for CFD simulations. . . 16
Figure 3.2: Different approaches of discretization for CFD simulations. . 16
Figure 3.3: Hot rolling process in steel industries. . . 25
Figure 3.4: Single impinging jet 3D model . . . 26
Figure 3.5: Multiple impinging jet 3D model. . . 27
Figure 3.6: Mesh for impinging jet cooling model . . . 27
Figure 3.7: Slab re-heating furnace in 2D. . . 28
Figure 3.8: Furnace model with boundary conditions . . . 29
Figure 3.9: Mesh for the furnace model . . . 29
Figure 3.10: Rotating machine model with boundary conditions . . . 30
Figure 3.11: Mesh for the rotating machine model. . . 31
Figure 3.12: LNG Tank model with dimensions . . . 32
Figure 3.13: SPH models for the rotating machine. . . 34
Figure 3.14: Heat conduction model with discretization . . . 35
Figure 3.15: Mini-channel with boundary conditions . . . 36
Figure 3.16: Numerical discretization for the mini-channel . . . 37
Figure 3.17: Tube bank heat exchanger . . . 38
Figure 3.18: Numerical discretization for the tube bank heat exchanger model . . . 38
Figure 4.1: Schematic of impinging jet cooling . . . 39
Figure 4.2: Interface of water jet for different inlet velocities. . . 40
Figure 4.3: Heat transfer coefficient for different inlet velocities. . . 41
Figure 4.4: Comparison of simulated jet diameter with correlation. . . 41
Figure 4.5: Temperature field for single and multiple jets . . . 42
Figure 4.6: Water splashing due to the interaction between jets . . . 42
Figure 4.7: Path lines of velocity inside the furnace . . . 43
Figure 4.8: Iso-surfaces of mass fraction and temperature. . . 44
Figure 4.9: Volume average temperature of the steel slab . . . 44
Figure 4.11: Average velocity profile in the air-gap of the motor . . . 46
Figure 4.12: Flow and temperature distribution in the air-gap of the motor 46 Figure 4.13: Temperature contour on internal surface of the stator. . . 46
Figure 4.14: Heat transfer coefficient on the rotor surface. . . 47
Figure 4.15: Air velocity profile inside the motor from FVM and SPH model 48 Figure 4.16: Air velocity contours close to the motor wafters. . . 48
Figure 4.17: Velocity profile inside the air-gap of the motor: FVM vs. SPH 49 Figure 4.18: Visualization of tank sloshing at different time instances. . . . 50
Figure 4.19: Simulated and measured Pressure on the tank wall . . . 50
Figure 4.20: Simulated forces on the tank wall: FVM vs. SPH . . . 51
Figure 4.21: Simulated and Froude-scaled forces on the tank wall . . . 51
Figure 4.22: Temperature contour of heat conduction in aluminium . . . 52
Figure 4.23: Temperature profiles of heat conduction in aluminium . . . 52
Figure 4.24: Temperature contour of heat conduction in water . . . 53
Figure 4.25: Temperature profiles of heat conduction in water. . . 53
Figure 4.26: Velocity and temperature contour in the mini-channel. . . 54
Figure 4.27: Temperature profiles in the mini-channel . . . 54
Figure 4.28: Velocity and temperature field in the tube bank heat exchanger 55 Figure 4.29: Temperature profiles in the tube bank heat exchanger. . . 56
Nomenclature
Abbreviations
2D Two dimensions 3D Three dimensions BC Boundary Condition
CFD Computational Fluid Dynamics CPU Central Processing Unit
CUDA Compute Unified Device Architecture DBC Dynamic Boundary Condition
DNS Direct Numerical Simulation EU European Union
FDM Finite Difference Method FEM Finite Element Method FFD Fast Fluid Dynamics FMM Fast Multipole Methods FVM Finite Volume Method GHG Greenhouse Gas
GPGPU General Purpose Graphic Processing Unit HPC High Performance Computing
LBM Lattice Boltzmann Method LES Large Eddie Simulation LNG Liquefied Natural Gas
MAC Marker And Cell
MPI Message Passing Interface OpenCL Open Computing Language OpenMP Open Multi Processing
POD Proper Orthogonal Decomposition R&D Research and Development
RANS Reynolds Averaged Navier Stokes equations ROM Reduced Order Modelling
ROT Runout Table RQ Research Question
SPH Smoothed Particle Hydrodynamics SVD Singular Value Decomposition TC Thermocouple
VOF Volume of Fluid Symbols
C Constant [-]
c Speed of sound [m/s]
cp Specific heat capacity [J/(Kg.K)]
Cr Courant number [-] d Nozzle diameter [m] D(Z) Jet diameter [m] Dh = 2gp, Hydraulic diameter [m] Dmin Minimum D(Z) [m] d p Particle spacing [m] E Total energy [J] F Force [N] f Mixture fraction [-]
f r Frequency [1/s] g Gravitation acceleration [m/s2] Gk Generation of turbulence kinetic energy due to the mean velocity
gradients [-]
gp Air-gap width between the rotor and the stator [m]
H Height of tank [m]
h Smoothing radius [m]
h(r) Liquid film thickness [m] H1 Height of initial water level [m]
ht Heat transfer coefficient [W/m2K]
k Turbulence kinetic energy [m2/s2] L Characteristic length [m]
Nu Nusselt number [-]
Nu0 Nusselt number at stagnation point [-]
Nud =
ht.d
κ , Nusselt number based on d [-] NuDh =
ht.Dh
κ , Nusselt number based on hydraulic diameter [-]
p Pressure [Pa] Pr Prandtl number [-] q00 Heat flux [W/m2] r Radial position [m] r1 Radius of region I [m] r2 Radius of region II [m]
r3 Radius of region III [m]
ra Vector position of particle a [m]
rb Vector position of particle b [m]
Re = uL ν , Reynolds number [-] S Source term [J] S1, S2 Sensor [-] T Temperature [◦C] t Time [s]
T1 Time for a full roll motion [s]
u Velocity [m/s]
u∗ Friction velocity at the nearest wall [m/s] u0 Fluctuating velocity [m/s] Uf Fluid velocity at inlet [m/s]
W Smoothing kernel function [-]
w Width of tank [m]
x Cartesian axis direction [m] x1 Distance of S1from bottom wall of the tank [m]
x2 Distance of S2from left wall of the tank [m]
y Distance to the nearest wall [m]
y+ = u
∗y
ν , Non-dimensional wall distance [-] YM Contribution of the fluctuating dilatation in compressible
turbu-lence to the overall dissipation rate [-] Z Distance downward from the nozzle [m] z0 Distance between nozzle and strip [m] Zi Elemental mass fraction for element i [-]
Special characters
δ Hydrodynamic boundary layer thickness [m] δT Thermal boundary layer thickness [m]
ε Turbulence dissipation rate [m2/s3] γ Isotropic constant [-] κ Thermal conductivity [W/m.K] λ Scaling factor [-] µ Dynamic viscosity [kg/m.s] ν Kinematic viscosity [m2/s] ω Specific rate of dissipation [1/s] φ Viscous dissipation [-]
ρ Density [kg/m3]
ρ0 Reference density [kg/m3]
τi j Stress tensor [-]
θ Rolling angle [degree] Subscripts
ε Turbulence dissipation rate ∞ Free stream fluid
µ Dynamic viscosity a Particle a
b Particle b e f f Effective
f Fluid
f uel Fuel stream inlet g Gas
h Heat
k Turbulence kinetic energy m Mass
min Minimum
ox Oxidizer stream inlet t Turbulent
1. Introduction
This chapter presents the research background, research questions formulated based on the research gaps, the research framework, objective of the thesis and the contributions to knowledge. The relationship between the research topics and the papers are also presented. This chapter includes the thesis out-line and the limitations of the thesis.
1.1
Background
Industrial processes and products, e.g. the runout table (ROT) cooling process in hot rolling steel industries (Cho et al., 2008; Mishra et al., 2015; Vakili, 2011), industrial furnaces and boilers (Dong, 2000; Stopford, 2002; Zhang et al., 2010), microchips and power electronics in high voltage products (Soon & Ghazali, 2008; Subramanyam & Crowe, 2000; Winder, 2004), motors and generators (de Almeida et al., 2012; Mecrow & Jack, 2008; Saidur, 2010), and marine applications (Johnson & Andersson, 2016; Vergara et al., 2012; Winebrake et al., 2007) are recognized as some of the major intensive energy consumers in these industries. Many of these processes often rely heavily on non-renewable energy resources. For instance, in hot rolling steel industries, large steel slabs are typically heated in furnaces in which fossil fuels like liq-uefied petroleum gas (LPG) are used as a primary source for combustion. The steel sector is an important and leading business area in many European Union (EU) countries and has been identified as critical owing to the large amount of greenhouse gas (GHG) emissions (Pardo et al., 2012). Another rapidly grow-ing sector contributgrow-ing significantly to high energy consumption is electric motors. Electric motors consume half of all electricity in industrialized coun-tries (de Almeida et al., 2012). Within the EU, they consume about 60-80% of energy used in the industrial sector and about 35% in the commercial sector. EU regulations and policies on energy and environment (“EU Commission Regulation (EC) No 640/2009”, 2009) are targeting a strong reduction in the impact of GHG emissions on the environment (Patyk, 2013; Saidur, 2010).
Optimizing existing products and improving process control for industries has a necessity to reduce energy consumption and GHG emissions. Energy-intensive processes or products often involve a wide range of complex multi-physical phenomena that a control system tends to govern towards optimum operations. The physical phenomena in the industrial processes and products
discussed in this thesis involve turbulent flow and heat transfer. The detailed dynamic behavior of complex fluid flow and heat transfer and their influence on the control parameters are generally not taken into account in control sys-tems that rely on measurements, black box models or empirical correlations. For example, in the re-heating furnace in a steel plant (Hosain et al., 2016), large slabs inside the furnace are heated to about 1250 ◦C by following a predetermined temperature profile. The heating profile must be adhered to in order to achieve a specified quality of steel. The pre-heating zone in the fur-nace is roughly 20 m long, 11 m wide and 10 m high, and between 6 and 10 thermocouples are placed very close to the roof and the side walls to measure the gas temperature. The measurements are then used in the control system to estimate the surface and average temperature of the slabs. The question is, how reliable and efficient can the control system be, given that it mostly relies on a data-fitting approach based on a few measurement points? The best choice would be to directly measure the surface temperature of the slab; however, this is currently impossible owing to the limitations of the available thermocouple technologies.
Process control, such as the system described above, can be improved by employing more advanced models and methods such as computational fluid dynamics (CFD), which are capable of providing all the necessary input de-tails and features. CFD is a very robust tool for analyzing the flow and heat transfer accurately. It can provide detailed insight into processes in which complex and fully non-linear phenomena may be present. High fidelity sulations based on CFD can be used to evaluate the current performance, im-prove online control and help optimize operation of industrial processes. How-ever, it is often very challenging to perform CFD simulations for large indus-trial processes and complex products. This is due to the existence of multiple space and time scales in the industrial processes and the limitations of the nu-merical techniques. In conventional CFD methods, the nunu-merical domain is discretized using mesh elements, and the accuracy of the model is completely dependent on the quality of the mesh and the physical, chemical and me-chanical phenomena involved. The mesh generation is often the most impor-tant and time-consuming pre-processing step for the mesh-based CFD solver. Moreover, the mesh needs to be locally refined in order to resolve interesting local features. The presence of microscale features (e.g. boiling, combustion) and macroscale features (e.g. burners in the furnace or water jets at the ROT cooling process in industrial processes make it very challenging to generate a suitable mesh and perform simulation within a useful timeframe for the results to be used in the design steps or in online control. In many cases, a very coarse mesh is applied to simulate the whole process to obtain an overall flow pattern; however, this approach sacrifices accuracy by neglecting small-scale features (Huang et al., 2008; J. G. Kim et al., 2000; Morgado et al., 2015). Despite sev-eral limitations, CFD simulations are still commonly used to model, analyze and improve industrial flow and heat transfer applications. CFD simulations
can also be used in the online control tool by running the simulations in real time, considering coarse discretization, where the relative effect of different control parameters on the process performance, rather than absolute accuracy, is the main concern. Another possibility may be to create a lookup table from a series of offline CFD simulations, and use the lookup table to control the process. A further option is to simplify the process geometry by applying ap-propriate boundary conditions when possible, and simulate a small section of the process to get an accurate solution (Hosain et al., 2016).
Recent technological development of parallel computing devices has sig-nificantly improved the numerical performance of conventional mesh-based CFD solvers. Despite this improved performance, simulating the whole pro-cess in detail by resolving the local flows using mesh-based commercial CFD solvers remains beyond reach. Mesh-free CFD methods based on simplified physics can be an alternative for overcoming some of the limitations of con-ventional mesh-based solvers. Smoothed Particle Hydrodynamics (SPH) has been identified as a potential mesh-free particle-based method in this thesis, mainly due to its mesh-free feature, flexibility, fast-solving capability and good support for visualization. The attraction of SPH is that it provides the opportunity for easy balancing of the speed and accuracy of the simulation, which is a very big advantage from the online control perspective. However, the main idea in this thesis is not to replace based methods with mesh-free particle-based methods, but to complement them, or choose the best meth-ods to fit the purpose. The theories behind the mesh-based and the mesh-free methods employed in this thesis are explained in detail in chapter 3.
1.2
Research challenges
The most popular methodology used to address industrial applications using CFD simulations uses the mesh-based finite volume method (FVM), where the Reynolds Averaged Navier–Stokes (RANS) equations are discretized and solved in commercial or open-source packages. This is mainly because of the well-established knowledge of the approach and its applicability to a wide range of engineering fields. FVM-based CFD solvers are very robust for solv-ing complex problems related to multiphase flows and heat transfer. They are mesh-based solvers and have been widely used to solve very complex prob-lems for several decades. However, solving industrial probprob-lems involving high deformation, multiple solid movements with strong and complex fluid–solid or fluid–fluid interactions remains a big challenge for such solvers and the overall approach. Industrial problems with fluid–fluid or fluid–solid interac-tions require extra care during the mesh generation phase. The limitainterac-tions, difficulties and challenges in solving complex industrial problems have not been rigorously discussed in the literature.
Mesh-based methods are used successfully to simulate large processes such as full 3D furnaces (Huang et al., 2008; Marino et al., 2002; Morgado et al., 2015). However, in these cases the detailed combustion chemistry and the lo-cal geometrilo-cal details are ignored. To date, no 3D simulations have been pub-lished for industrial processes based on FVM that cover both microscale and macroscale features. Particle-based methods such as SPH (Auer, 2008; Krog & Elster, 2012) are gradually emerging and gaining popularity in the CFD community because of their fast solving capability, flexibility and simplicity. The SPH approach is currently being widely used for visual fluid and ther-mal effects in films and video games, where accuracy is not very important. Recent developments in SPH towards engineering applications, the level of accuracy achieved and the diversity of its applicability (J. Monaghan, 2012) have opened doors for new types of industrial applications (Shadloo et al., 2016). The SPH user community is small and growing, thus the propagation and development of this method towards industrial applications has been slow compared to other, conventional methods. The types of industrial applications of interest in this thesis have not been previously addressed by the SPH user community. Therefore, the limitations and challenges of SPH for many in-dustrial applications are still unknown due to lack of study. As mentioned earlier, the learning curve is one of the limiting factors for use of emerging methods such as SPH for industry. Recently, in their SPH studies, Shadloo et al. (Shadloo et al., 2016) demonstrated that its diverse applicability (J. Mon-aghan, 2012) has a lot to offer for industrial applications. Special attention and substantial efforts are required from scientists and R&D engineers to enlarge the capability of SPH for new types of applications. Furthermore, comparisons between different methods aimed at selecting the right method for a particular application needs to be addressed.
Based on the research challenges and the knowledge gap discussed above, three research questions (RQ) are formulated in this thesis:
• RQ1
What are the limitations of RANS when used to simulate complex in-dustrial applications?
• RQ2
Under what circumstances can SPH replace or complement RANS? • RQ3
What is the potential of using SPH in on-line control tools?
The research questions are formulated in a general manner, however, the conclusions are based on selected applications within the research framework (section 1.3). The research questions are discussed in detail together with con-cluding remarks in section 4.3.
Table 1.1: Relation between the papers and the research questions
Research question Papers
RQ1 I,II,III,IV,V
RQ2 VI,VII,VIII,IX
RQ3 VII
Fluid Flow and Heat Transfer Simulations for Complex Industrial Applications
FVM SPH
Eulerian Vs. Lagrangian
Paper I Cooling at ROT Paper II Slab reheating furnace
Paper III Literature review
Paper IV Rotating machines: Taylor-couette flow
Paper VI Rotating machines: FVM vs. SPH
Paper VII Liquid sloshing in Tank
Paper VIII Heat transfer in mini-channels
Paper IX SPH Thermal model
Paper V Rotating machines: Parametric analysis
Figure 1.1: Schematic showing the relationship between the research topics and the papers
1.3
Research framework
The work in this thesis mainly aims to use CFD to solve energy-intensive com-plex industrial processes, where flow and heat transfer problems are critical. The work is performed in tight collaboration with several industries to define the current challenging cases that need to be studied. The industrial
applica-tions studied in this thesis are the ROT cooling process, presented in Paper I, the slab reheating furnace in hot rolling steel plant, investigated in Paper II, the electric motor, studied in Papers IV, V and VI, and the tank sloshing in a LNG carrier ship, presented in Paper VII. The studied problems cover both single and multi-phase flows. The cases also cover heat transfer in the form of conduction, convection and radiation, as well as combustion. In the first stage of this work, the industrial applications are solved using the Eulerian mesh-based finite volume RANS CFD solver ANSYS Fluent. This task was performed to underline the limitations of RANS and highlight the challenges of simulating large and complex industrial applications. To overcome some of the observed limitations of RANS, the search is directed towards finding alter-native methods that are more flexible and faster compared to RANS methods (Paper III).
In the later stage of this work, the Lagrangian particle method SPH is iden-tified as a potential alternative to compensate for some of the weaknesses of RANS methods. To evaluate the applicability and the performance of the SPH solver for industrial problems, the rotating machine (Paper VI) and tank slosh-ing (Paper VII) cases are simulated to benchmark the SPH solutions with the solutions from the finite volume solver.
Finally, the research work is directed towards SPH development, where the energy equation is implemented in the open-source SPH code DualSPHysics to simulate thermal problems. To validate the thermal implementation in Du-alSPHysics and to illustrate its accuracy, several laminar heat transfer cases, heat transfer in infinite mini-channel (Paper VIII) and heat transfer in heat exchangers (Paper IX) are simulated.
The included scientific papers (Paper I - Paper IX) are briefly summarized in chapter 5. The appended papers can be linked to the research questions presented in section 1.2 and to the research topic as illustrated in Table 1.1 and Figure 1.1, respectively. The analysis presented in this thesis is limited to the studied cases presented in the included papers. The research questions are answered in this thesis mainly based on the observations and hypotheses made in the appended papers. The answers to the research questions are presented in section 4.3 in the form of a discussion, which is limited to the studied cases. However, the observations illustrated in this thesis may serve as a decision tool to select a suitable CFD approach to deal with the type of industrial problems analyzed within this framework.
1.4
Objective of the thesis
The overall objective of the thesis is to perform high fidelity fluid flow and heat transfer simulations for several industrial processes and products to better understand the underlying physical phenomena, to identify a few energy-intensive processes and products to numerically investigate in detail
using the most popular CFD methods in commercial packages, and highlight the challenges and their limitations. Another key objective of this thesis is to identify alternative CFD methods that are suitable and sufficiently flexible for use in different industrial applications, to overcome some of the limitations of conventional CFD methods. Furthermore, the thesis aims to discuss the potential use of CFD simulation from a real-time application perspective and shed light on online process control using high fidelity simulations.
The goals of the thesis can be explicitly described by the following points:
• To build CFD models for selected energy-intensive processes and products related to multiphase flow, free-surface flow and heat transfer. Moreover, to validate the results using analytical solutions or available data from published literature (RQ1).
• To discuss the usefulness and limitations of the methods commonly used in commercial CFD packages (RQ1).
• To find alternative methods that can overcome the underlying limita-tions of RANS methods for industrial applicalimita-tions (RQ1).
• To introduce SPH for industrial flow and heat transfer simulations and discuss the current limitations (RQ2).
• To discuss the type of applications where SPH can be used for online process control purposes (RQ3).
1.5
Contributions to knowledge
The main contribution of this doctoral research is towards the industrial applications. The thesis also contributes to scientific knowledge from both the fundamental and applied perspective. Selected energy intensive industrial processes are investigated using high fidelity CFD simulations, the difficulties and challenges are highlighted and possible ways to overcome these are discussed.
The overall contribution of the thesis can be briefly summarized as follows:
• Performing high fidelity simulations of selected energy-intensive pro-cesses and products to provide detailed insight to enhance the under-standing of the underlying complex fluid flow and heat transfer phe-nomena. The simulated applications involve ROT cooling in hot rolling
steel industries, slab re-heating furnace, sloshing dynamics in carrier ships fuel tanks, rotating machines, and heat exchangers.
• Discovering unknown phenomena involved in the studied industrial ap-plications and presenting hypotheses. Discussing and highlighting the difficulties and challenges involved in simulating such industrial pro-cesses using different CFD approaches.
• Performing sensitivity analysis to evaluate the impact of different con-trol parameters on thermal performance.
• Providing the state of the art by reviewing literature relevant to the stud-ied topics in this thesis. Performing a literature survey and classifying available CFD methods applicable to different types of industrial and engineering applications from a real-time simulation perspective. • Introducing and using SPH for industrial flow and heat transfer
ap-plications and evaluating its potential usefulness to thermal problems. Discussing the challenges and limitations of SPH for industrial ther-mal simulations and indicating future directions based on these obser-vations.
• Implementing SPH thermal equations in an open-source SPH-based CFD solver, DualSPHysics, using C++. Using and validating the SPH thermal implementation by solving thermal problems related to heat conduction and convection. Discussing the limitations of SPH for ther-mal problems. Highlighting the future challenges to simulating complex industrial flow and heat transfer.
1.6
Thesis outline
This thesis is written based on the appended papers and contains the following chapters:
Chapter 1 Introduction
This chapter presents the research background, research questions for-mulated based on the research gaps, the research framework, objective of the thesis and the contributions to knowledge. The relationship be-tween the research topics and the papers are also presented. This chapter includes the thesis outline and the limitations of the thesis.
Chapter 2 Literature review
This chapter presents a literature review in the field of multiphase flows and heat transfer to illuminate the state of the art of the selected
in-dustrial applications. It also presents a literature review on available advanced CFD methods.
Chapter 3 Methodology
This chapter presents a detailed explanation of the overall methodology to address an industrial application using the CFD approach. All the numerical models for the simulated cases and the governing equations are presented.
Chapter 4 Results and discussion
This chapter presents the key results from the performed simulations and provides a detailed discussion of the studied topic while answering the research questions.
Chapter 5 Summary of appended papers
This chapter summarizes the included papers and the author’s contribu-tion to the papers.
Chapter 6 Conclusions
This chapter presents the major conclusions of the thesis. Chapter 7 Future work
This chapter suggests the potential future direction of the research topic presented in this thesis.
2. Literature Review
This chapter presents a literature review in the field of multiphase flows and heat transfer to illuminate the state of the art of the selected industrial applications. It also presents a literature review on available advanced CFD methods.
CFD simulation techniques have been used to solve a variety of industrial fluid flow and heat transfer problems for several decades. The area of inter-est of the research presented in this thesis is to solve engineering problems related to single-phase and multiphase flows and heat transfer. The literature review presented in this chapter mainly covers literature in this context, while providing a broad perspective on applicability of different CFD methods to industrial applications.
The extent of applicability of CFD simulations to industrial applications is completely dependent on the physical phenomena and the time scale associ-ated with the application. Industrial processes and products are often so large and complex that it becomes too difficult to solve them numerically using CFD techniques. The recent developments of high-performance computing (HPC) resources have revolutionized the usage of CFD simulation for large and plex problems. Today, the use of HPC with supercomputers is the most com-mon approach for CFD engineers. The algorithms involved in the methods are usually parallelized so that simulations can be run in parallel using supercom-puters with multicore architecture. Nevertheless, simulating entire processes such as ROT cooling or the furnace using CFD while resolving microscopic features like boiling and combustion, remains unapproachable with currently available computing capabilities. The only way to overcome this limitation at present is to simplify the models and use methods with simplified physics. This thesis explores the applicability, capability and efficiency of different CFD methods for complex engineering problems from a perspective of in-creasing the speed of simulation.
There are two classes of CFD methods; these are the Eulerian approach and Lagrangian approach. In the Lagrangian approach, fluid is represented by a set containing a large number of particles that possess properties such as mass, ve-locity and temperature. All the particles are then traced along the flow and the time evolution of different properties is calculated based on the interactions between the particles. In the Eulerian approach, the fluid is represented by us-ing control volumes as mesh elements whose coordinates are fixed. The fluid
flowing through these control volumes is observed and fluxes are calculated to measure the rate of change of properties such as velocity and temperature. Methods developed based on the Eulerian approach are called mesh-based methods, and methods developed based on the Lagrangian approach are called mesh-free particle methods. Both classes of methods have pros and cons. The mesh-free characteristic is one of the biggest advantages of Lagrangian CFD methods for R&D engineers, as meshing is the most time-consuming and chal-lenging pre-processing phase for Eulerian CFD solvers. In recent decades, researchers have developed methods that combine Lagrangian and Eulerian frameworks to complement the weaknesses of both classes. These methods are classified as hybrid methods (Figure 2.1).
CFD
Conventional Methods
● Finite Volume Method (FVM) ● Finite Difference Method (FDM) ● Finite Element Method (FEM) ● Spectral Methods Accelerated Methods Advanced Numerical Methods Mesh Based Methods
● Reduced Order Modeling (ROM) ▪Proper Orthogonal Decomposition(POD) ▪ Singular value Decomposition (SVD) ● Marker & Cell (MAC)
Mesh free methods
● Smoothed Particle Hydrodynamics(SPH) ● Fast Multipole Method (FMM) ● Method of Fundamental Solutions (MFS) ● Finite Pointset Method (FPM)
● Moving Particle Semi-Implicit Method(MPS)
Hybrid methods
● Fast Fluid Dynamics (FFD) ● Particle in Cell Method (PIC) ● Vortex in Cell Method (VIC) ● Lattice Boltzmann Method (LBM)
Hardware Techniques Parallel programming CPU ● MPI ● OpenMP ● Cloud Computing GPGPU ● CUDA ● OpenCL ● Cloud Computing CPU+GPGPU
Figure 2.1: Hierarchical classification of methods in CFD (Hosain & Fdhila, 2015)
Mesh-based conventional methods are the most well-established and pop-ular methods, and are mature enough to handle complex problems with high accuracy. These methods are extremely reliable, however they come at a very high numerical cost, which limits their use in fluid flow and heat transfer simulations for large industrial processes. Therefore, simulations using these methods are only used for small-scale problems (Mazumder & Lu, 2013).
Large industrial processes have also been addressed using FVM in Huang et al.(Huang et al., 2008) and Morgado et al.(Morgado et al., 2015); however, these have performed poorly from a speed perspective. Mathematically sim-plified mesh-based methods like reduced order modelling (ROM) (Lappo & Habashi, 2009; Lieu et al., 2006) can, in many cases, provide enhanced numer-ical performance, and enable simulations to be performed in real time. How-ever, the accuracy is usually reduced in such applications. Therefore, when using mesh-based methods, one needs to balance the speed and accuracy of the simulations. The main drawback, however, is that the entire workflow, in-cluding mesh generation, needs to be repeated to tune the accuracy and speed, making this a less user-friendly option for R&D engineers.
On the other hand, mesh-free particle-based CFD methods have several ad-vantages over mesh-based solvers. Due to the inherent Lagrangian properties, the convection of the particles happens due to the interaction forces, therefore the equations involved in this approach are simpler than those in mesh-based solvers. The most popular method in this class is the SPH method, mainly due to its simplicity, flexibility and promising performance. The SPH method produces satisfactory results for problems involving disruptive free surfaces, multiple fluids, elastic fracture, thermal matter diffusion and chemical precip-itation (J. Monaghan, 2012). It can also be applied to physiological problems such as soft tissue and blood flows. SPH is known to be robust for free-surface and multiphase flows (J. Monaghan, 2012; Randles et al., 2016). This is be-cause, for free-surface flow, such as the impinging jet problem and sloshing in a tank, there is no need to solve the two phases (air and water) to identify the interface between them. The surface tension of the water itself creates the air– water interface. SPH has recently been used to solve a wide range of industrial applications (Shadloo et al., 2016). The recent diverse applications (Shadloo et al., 2016) of SPH include mainly aerospace (Ortiz et al., 2004; Siemann & Groenenboom, 2014), car and automotive (Barcarolo et al., 2014; Oger et al., 2009), energy production, e.g. marine (Baeten, 2009; Hosain et al., 2018), oil and gas (Violeau et al., 2007), hydropower (Manenti & Ruol, 2008; Tomas-icchio et al., 2012) and industrial processing, for example, casting, grinding, high speed cutting, mixing and separation, friction stir welding, solidifica-tion, oxidasolidifica-tion, droplet breakup and spray coating (Shadloo et al., 2016). The SPH method is not a suitable choice for problems with high Reynolds number turbulent flows, steady flows, slow dynamic flows and flow without complex interfaces (Shadloo et al., 2016). This is because the SPH method still requires development in several modules, e.g. robust boundary conditions and turbu-lence. The SPH method is still far from being well-established enough to re-place the mesh-based FVM solver. However, in its current state, the flexibility of SPH has a lot to offer the industrial applications.
Hybrid methods are also of interest for free-surface flows, multiphase flows and heat transfer simulations. In recent developments, researchers have been trying to combine different methods to develop new methods that combine
benefits from both Eulerian and Lagrangian frames of reference. An example of these is fast fluid dynamics (FFD), as used by Zuo and Chen (Zuo & Chen, 2009, 2010) to simulate air flow inside buildings in real time. Another method, Lattice Boltzmann Method (LBM), solves the Boltzmann equation instead of the Navier Stokes equations and is popular for thermal problems. Geveler et al.(Geveler, Ribbrock, Mallach, & Göddeke, 2011) implemented LBM to solve various complex fluid flow cases, achieving real-time performance.
This literature review demonstrates that there is no unique recipe or method that can work for all types of industrial flow simulations. Mesh-based solvers are reliable, robust and have a well-known degree of accuracy; however, they are numerically too demanding to be used for large industrial processes. On the other hand, the mesh-free and hybrid methods are very flexible and easy to use. However, the knowledge gap on applicability, accuracy, stability and convergence rate limits their extensive use in industrial R&D. Therefore, the application of mesh-free and mesh-based methods for large industrial appli-cations remains a dilemma.
In this thesis, the conventional mesh-based FVM solver is used to analyze flow and heat transfer for selected industrial applications. The results pre-sented in this thesis provide detailed insight into each simulated application. The difficulties and challenges involved in simulating industrial processes are highlighted based on the experiences gathered from the performed simula-tions. Hypotheses are formulated, based on the results of the simulations, on how to use the simulation results to improve the processes. The promising flexibility of the SPH method and its diverse applications inspires its usage for industrial heat transfer simulations. One of the goals of the thesis is to introduce and use SPH for industrial heat transfer simulations; however, no commercial or open-source SPH thermal solver is currently available. A small number of thermal simulations (Cleary, 1998; Rook et al., 2007; Sigalotti et al., 2003; Szewc et al., 2011) based on SPH have been performed; however, these do not comprehensively cover the knowledge of applicability of SPH for industrial heat transfer applications. Within the framework of this thesis, in Pa-per IX, as a first step towards using SPH for industrial heat transfer simulation, the energy conservation equations are implemented into an open-source SPH flow solver called DualSPHysics (Crespo et al., 2015). The SPH thermal im-plementation is used to solve a few classical CFD problems, and the solutions are validated using analytical solutions. The solutions from the SPH thermal solver are also compared with the solution from the FVM solver to benchmark the solutions. The challenges faced and the limitations observed while using the SPH thermal solver are discussed. Moreover, method comparison is also one of the key focuses of this thesis for evaluating the efficiency of different methods for industrial applications. The SPH thermal solver will be released in future as an open-source package for the SPH user community to open up the area of thermal simulations using SPH. The main idea behind this develop-ment is to have a flexible thermal solver, the accuracy and speed of which can
be adjusted easily to fit the demand of a specific industrial process. In future, the results from both the SPH and FVM thermal solvers could be combined to synthesize the knowledge of a process from both overall and detailed solution perspectives. The SPH thermal solver and the FVM thermal solver can both be used where they fit best, in complementary fashion. For example, some parts of the process can be simulated using the SPH thermal solver, and other parts of the same process can be simulated using the FVM thermal solver. The re-sults can then be combined for a full picture of the process. This development is a small step towards the future goal of this work, which is to direct research towards real-time simulations for industrial processes. The ultimate goal will be to use CFD simulation in online control tools for decision support and to operate the processes in an energy-efficient way.
3. Methodology
In this chapter, the approach to performing the CFD simulations for industrial processes is illustrated. The theories and models are also presented in detail.
3.1
Modelling approach
A methodological approach is followed in this thesis to simulate and analyze the industrial applications. The approach can be divided into the following four main steps (Figure 3.1).
Step 1. A background review is performed to understand the research area and to gather information on related works published by other researchers before proceeding. The process is then analyzed in detail and the scope and the expected outcome from the numerical study are defined based on the formulated hypothesis. To reach the defined goal, sufficient information is generated about the process to be able to build the numerical domain and to select the most realistic boundary conditions.
Step 2. The numerical domain is developed based on the information col-lected in the previous step; the domain is then discretized using mesh or particles depending on the chosen CFD approach. Suitable mathemati-cal models are then employed to solve a well-defined problem.
Step 3. After obtaining the first solution, post-processing is performed. A mesh grid-sensitivity analysis is also performed to ensure that the so-lution is grid-independent in the case of mesh-based solvers. The final solution is then validated using available theories, experiments or mea-surements. If the results are not valid, then the model is revisited to make possible adjustments and step 2 is repeated.
Step 4. The valid results are then analyzed and hypotheses are made based on the simulation results. Detailed insight regarding the process is provided and possible improvements are suggested based on the phenomena re-vealed by the simulations.
Background review Process analysis
Model Development Solve & Post-process Analyse Hypotheses Validate results
CAD
Discretise
Boundary & Physics Make hypotheses
Figure 3.1: Methodological approach for CFD simulations
3.2
Different approaches in CFD
Ω
(a)Ω
Influence domain Particle ii
(b)Figure 3.2: Different approaches of discretization for CFD simulations (a) Mesh (b) particles
Two different approaches, based on Eulerian and Lagrangian reference frames, respectively, are used in this thesis to perform high fidelity CFD simulations for industrial applications. The CFD methods developed based on the Eulerian reference frame are called mesh-based methods. In this approach, the numerical domain Ω is discretized using mesh elements (Figure 3.2a) and a set of highly nonlinear equations, the Navier–Stokes equations (section 3.2.1), are solved over all the mesh elements. In this thesis, the time-averaged versions of the original Navier–Stokes equations, RANS equations are solved. This idea, where the Reynolds decomposition is applied to separate the flow variables into mean (time-averaged) and fluctuating
components to derive the RANS equations, was proposed by Reynolds Osborne (Reynolds, 1895). The RANS equations are principally used to describe turbulent flows, this is the most common way to model turbulent flows in most commercial CFD packages. There are other approaches, such as DNS (direct numerical simulations) and LES (large eddie simulation), to solve the Navier–Stokes equations. However, both of these approaches are numerically much more demanding than the RANS approach, and are therefore not a preferred option for large problems in industrial R&D. The equations involved in the RANS modelling approach are presented in detail in section 3.3. The most popular mesh-based FVM method is employed in this thesis.
CFD methods developed based on the Lagrangian reference frame are called mesh-free particle-based methods. In this approach, the fluid is represented by a set of fluid particles (Figure 3.2b) that have properties like mass, position, velocity and temperature. The original set of Navier–Stokes equations is solved in this approach; however, the convection of the particles occurs automatically due to the interaction forces between the particles. Thus, the nonlinear convective terms in the original Navier–Stokes momentum equations (section 3.2.1) are neglected. The most popular Lagrangian mesh-free particle method, SPH, is employed in this thesis. The Navier–Stokes equations are approximated using SPH kernel approximation operators, thus the SPH form of the equations are solved. The equations involved in the SPH modelling approach are presented in detail in section 3.4.
3.2.1
Governing equations
A system of transport equations employed to model any fluid flow mainly in-volve the conservation of mass and momentum. Additional equations must also be solved; for example, the energy conservation equation, to model the heat transfer, turbulence equations, to model the turbulence, and species trans-port equations, for combustion. The mass and momentum equations are pre-sented below.
The mass conservation equation can be written as follows: ∂ ρ
∂ t + ∂ ∂ xi
(ρui) = 0 (3.1)
The momentum conservation, in the original Navier–Stokes equation, is described by the following equation:
∂ ∂ t(ρui) + ∂ ∂ xj (ρujui) | {z } convective term = −∂ p ∂ xi + ∂ ∂ xj µ∂ ui ∂ xj | {z } diffusive term +Fi (3.2)
where, ρ is density, ui is velocity in tensor notation, p is pressure, µ is
dynamic viscosity and Fiis external force.
3.2.2
Energy transport equation
The energy conservation equation can be expressed as follows:
ρ cp ∂ T ∂ t + ui ∂ T ∂ xi | {z } convective term = ∂ ∂ xi κ∂ T ∂ xi + φ (3.3)
where, T is thermal energy, cp is specific heat capacity, κ is thermal
con-ductivity and φ is the viscous dissipation or the rate of internal heat generation per unit volume.
3.2.3
Mixture fraction transport equation
The mixture fraction concept is applied in Paper II to model the combustion, under the assumption of equal mass diffusivities of the species involved in the system. The individual species transport equation is then reduced to a single transport equation for the mixture fraction f = Zi− Zi,ox
Zi, f uel− Zi,ox as follows: ∂ ∂ t(ρ f ) + ∂ ∂ xi (ρuif) = ∂ ∂ xi µ σ ∂ f ∂ xi + Sm+ Suser (3.4)
where, µ is viscosity and σ is a constant.
3.3
Mathematical Models for RANS
The computational transport equation systems, the RANS equations, employed to model the ROT cooling (Paper I), the slab re-heating furnace (Paper II), the rotating machines (Paper IV - Paper V) and sloshing in tank (Paper VII) are presented in this section.
3.3.1
RANS transport equations
RANS is a time averaged version of the original Navier–Stokes equations pre-sented in section 3.2.1. Reynolds decomposition (Reynolds, 1895) is applied to decompose the flow variables into mean (time-averaged) and fluctuating components to derive the RANS form of the governing equations. The decom-position of flow variables gives rise to a special nonlinear term (−ρui0uj0) in
requires additional modelling to close the RANS equations. This Reynolds stress term is mainly responsible for the modelling of turbulent quantities, which gives rise to many turbulence models, for example, two equation mod-els, like k − ε or k − ω turbulence models. The model equations for k − ε and k− ω turbulence models are presented in section 3.3.2. The RANS version of the momentum conservation equations can be written as follows:
∂ ∂ t(ρui) + ∂ ∂ xj (ρujui) + ∂ ∂ xj ρ ui0uj0 = − ∂ p ∂ xi + ∂ ∂ xj τi j+ Fi (3.5)
where, u and u0 represents the time-averaged and the fluctuating velocity, respectively. The diffusion term is rewritten using the Newtonian fluid stress tensor τi j, where τi jis modelled as follows:
τi j= µ ∂ ui ∂ xj +∂ uj ∂ xi −2 3 ∂ uk ∂ xk δi j (3.6)
The Reynolds stress term (−ρui0uj0) is defined as,
−ρui0uj0= µt ∂ ui ∂ xj +∂ uj ∂ xi −2 3 ρ k+ µt ∂ uk ∂ xk δi j (3.7)
where, µ and µt are laminar and turbulent viscosity, respectively.
3.3.2
Turbulence transport equations
The Reynolds stress term(−ρui0uj0) can be modelled in various ways. In this
thesis, two different turbulence models, the k − ε and the k − ω models are employed.
3.3.2.1 k− ε turbulence model
Industrial flow problems are most often turbulent and thus require the turbu-lence to be modelled by modelling the Reynolds stress term in the momentum equation. There are several options of turbulence models available in the sci-entific literature. The k − ε model (Launder & Spalding, 1974) is the most ro-bust and economic turbulence model for industrial processes (Li et al., 2017). The k − ε turbulence models are employed to model the turbulence in the sim-ulations of the ROT cooling process (Paper I), the furnace (Paper II) and the rotating machines (Paper IV - Paper VI). The equations describing the turbu-lence kinetic energy(k) and the turbulence dissipation rate (ε) are as follows:
∂ ∂ t(ρk) + ∂ ∂ xj (ρkuj) = ∂ ∂ xj µ+ µt σk ∂ k ∂ xj + Gk− ρε −YM (3.8)
∂ ∂ t(ρε) + ∂ ∂ xj (ρεuj) = ∂ ∂ xj µ+ µt σε ∂ ε ∂ xj + ρC1Sε − ρC2 ε2 k+√ν ε (3.9)
where turbulence viscosity µt= ρCµ
k2 ε , C1= max 0.43, k εp2Si jSi j k εp2Si jSi j+ 5 , C2= 1.9, σk= 1.0 and σε = 1.2 (ANSYS Inc., 2018).
3.3.2.2 k− ω turbulence model
The SST k − ω turbulence model developed by (Menter, 1994) is used for the simulation of liquid sloshing in a rectangular tank (Paper VII). This turbu-lence model provides both robustness and stability in this type of process. The following equations represent the transport of the turbulent kinetic energy(k) and the vorticity(ω), respectively.
∂ ∂ t(ρk) + ∂ ∂ xj (ρkuj) = ∂ ∂ xj Γk ∂ k ∂ xj + Gk−Yk (3.10) ∂ ∂ t(ρω) + ∂ ∂ xj (ρωuj) = ∂ ∂ xj Γω ∂ ω ∂ xj + Gω−Yω+ Dω (3.11)
The effective diffusivity terms for k and ω are given by: Γk= µ +
µt σk and Γω= µ + µt σω
, respectively. The turbulent viscosity is given by: µt = α∗
ρ k ω , where α∗ is a low Reynolds number region correction dampening factor. Gk,
represents the generation of turbulence kinetic energy due to mean velocity gradients. Yk, represent the dissipation rate of k. Gω, represents the generation
of ω. Yω, represent the dissipation rate of ω. Dω, is the cross-diffusion term
related to Γkand Γω.
3.3.3
Energy transport equation
The energy transport equation (3.3) is usually written in the form of total en-ergy as follows (ANSYS Inc., 2018):
∂ ∂ t(ρE) + ∂ ∂ xi [ui(ρE + p)] = ∂ ∂ xj κe f f ∂ T ∂ xj + ui(τi j)e f f + Sh (3.12)
where E is the total energy, κe f f = κ + cp
µt
Prt
is the effective thermal con-ductivity, Shis heat of the chemical reaction and(τi j)e f f is the deviatoric stress
tensor, defined as (τi j)e f f = µe f f ∂ ui ∂ xj +∂ uj ∂ xi −2 3µe f f ∂ uk ∂ xk δi j (3.13)
3.3.4
Volume of Fluid (RANS-VOF)
The volume of fluid (VOF) model is in principle an interface-tracking method integrated into the RANS model as it is formulated in the CFD commercial code ANSYS Fluent (ANSYS Inc., 2018). This is a very robust approach for simulating multiphase flows. This approach is employed in this thesis to simu-late the multiphase flow simulations, the ROT cooling (Paper I) and the liquid sloshing in tank (Paper VII). In this formulation, each phase has its individual continuity equation, however both phases share the same set of momentum equations.
For RANS–VOF, the continuity transport equation, also called the volume fraction equation, for the gas phase is given by (ANSYS Inc., 2018):
1 ρg ∂ ∂ t(αgρg) + ∂ ∂ xi αgρguig = 0 (3.14)
where αg, ρg and uig are the volume fraction, the density and the velocity
of the gas phase in tensor notation, respectively. The interpolation near the liquid–gas interface surface is calculated by using the geometric reconstruct method developed by Youngs (Youngs, 1982). The method assumes that the interface between two fluids has a linear slope within each cell, and uses this linear shape to calculate the advection of fluid through the cell faces. This method is the most accurate method currently available in ANSYS Fluent. In the RANS–VOF approach, the momentum equation presented in section 3.3.1 is solved, and the same equation is solved for both phases.
3.4
Mathematical Models for SPH
SPH is simply an interpolation method where any function can be evaluated by using the values of different properties of a set of particles. This section presents the SPH form of the governing equations presented in section 3.2.1, together with the necessary fundamentals to illustrate the SPH methodology.
