Publicidad

Publicidad

Publicidad

Publicidad

Publicidad

Publicidad

Publicidad

Publicidad

Publicidad

Publicidad

Próximo SlideShare

Efficiency Optimization of Realtime GPU Raytracing in Modeling of Car2Car Com...

Cargando en ... 3

22 de Sep de 2016•0 recomendaciones## 1 recomendaciones

•695 vistas## vistas

Sé el primero en que te guste

ver más

Total de vistas

0

En Slideshare

0

De embebidos

0

Número de embebidos

0

Descargar para leer sin conexión

Denunciar

Ingeniería

Impact of unsteadiness on uncertainty in automotive aerodynamic flows using OpenFOAM in collaboration with Jaguar Land Rover (JLR)

Akshat SrivastavaSeguir

Publicidad

Publicidad

Publicidad

Efficiency Optimization of Realtime GPU Raytracing in Modeling of Car2Car Com...Alexander Zhdanov

mchr dissertation2Marco Chrappan Soldavini

lapointe_thesisJamie LaPointe

Dissertation A. SklavosAlexandros Sklavos

Pulse Preamplifiers for CTA Camera Photodetectorsnachod40

add_2_diplom_mainAlexander Litvinenko

- CRANFIELD UNIVERSITY School of Aerospace, Transport and Manufacturing M.Sc. Thesis Academic Year: 2015-2016 Akshat Srivastava The Impact of Unsteadiness on Uncertainty in Automotive Aerodynamics Simulation using OpenFOAM Supervisor: Dr. Panagiotis Tsoutsanis © Cranﬁeld University, 2016. All rights reserved. No part of this publication may be reproduced without the written permission of the copyright holder.
- Except where acknowledged in the customary manner, the material presen- ted in this thesis is, to the best of my knowledge, original and has not been submitted in whole or part for a degree in any university. ________________________ Akshat Srivastava
- Abstract The Detached Eddy Simulation (DES) is performed for ﬂow over sphere. The simula- tions are carried out based on free-stream Mach number M∞ = 0.2 and sphere diame- ter D = 1m in sub-critical regime at Re = 10,000. A cartesian grid is generated using CfMesh in OpenFOAM and computations are performed using PIMPLE Foam solver. For this Reynolds number at near to the equator of the sphere, ﬂow separates laminarly and in the separated shear layer the transition to turbulence occur at certain distance. The frequency spectrum using probes at different locations are described and discussed in details. The three main instabilities of different frequencies shed from sphere surface namely, the large-scale vortex shedding at St = fvs D/U = 0.203, the Kelvin Helmholtz and a frequency lower than the vortex shedding frequency known a low-frequency which attributes to the shrinkage and enlargement of recirculation bubble. Additionally, turbu- lence statistics are compared with previous experimental and numerical results available in literature for sub-critical Reynolds number. Speciﬁc consideration is dedicated to com- puting the mean ﬂow statistics and parameters such as mean angular pressure and skin friction coefﬁcient, mean lift and drag coefﬁcient, among others, to validate the solver and turbulence model used. Keywords: turbulence, sphere ﬂow, OpenFOAM, vortex-sheding, low-frequency, wake v
- Acknowledgements The work described in this report is the result of my 3 months thesis performed at Cran- ﬁeld University, UK. Many people contributed their guidance for completion of this thesis work. I would like to thank everyone who helped me in one way or another and few people in particular. First and foremost, I would like to thank Jaguar and Land rover (JLR) for providing me an opportunity to work in this industrial thesis. My supervisor Dr. Panagiotis Tsoutsanis has been a great help through his valuable guidance, support and direction. It is my ﬁrst experience working in turbulence subject, hence, his knowledge and expertise guided me to understand the project better. Finally, I would like to thank all the other people for their help at various stages through the project. I heartily appreciate all your sincere efforts. vi
- Contents Abstract v Acknowledgements vi List of Figures xii List of Tables xiii 1 Introduction 1 1.1 Background and Motivation . . . . . . . . . . . . . . . . . . . . . . . . 1 1.2 Literature Review . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2 1.2.1 Experimental Background . . . . . . . . . . . . . . . . . . . . . 2 1.2.2 Previous Numerical Investigation . . . . . . . . . . . . . . . . . 4 1.3 Thesis Objectives . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6 1.4 Outline . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7 2 Physics and Modelling 8 2.1 Governing Equation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8 2.2 Turbulence models and Numerical methods . . . . . . . . . . . . . . . . 9 2.2.1 RANS principle . . . . . . . . . . . . . . . . . . . . . . . . . . . 10 2.2.2 LES principle . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13 2.2.3 Filtered Navier-Stokes equation . . . . . . . . . . . . . . . . . . 15 2.3 Turbulence closure model . . . . . . . . . . . . . . . . . . . . . . . . . . 16 2.4 RANS-LES Hybrid approach . . . . . . . . . . . . . . . . . . . . . . . . 17 2.4.1 Detached Eddy Simulation (DES) . . . . . . . . . . . . . . . . . 18 2.4.2 Delayed Detached Eddy Simulation (DDES) . . . . . . . . . . . 19 2.5 Improved Delayed Detached Eddy Simulation (IDDES) . . . . . . . . . . 20 2.5.1 Modiﬁcation of the Sub-grid length-scale . . . . . . . . . . . . . 21 2.5.2 DDES branch of IDDES . . . . . . . . . . . . . . . . . . . . . . 23 2.5.3 WMLES branch of IDDES . . . . . . . . . . . . . . . . . . . . . 23 vii
- Contents 2.5.4 Hybrid branch of DDES and WMLES . . . . . . . . . . . . . . . 25 3 Software and Methodology 27 3.1 OpenFOAM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 27 3.1.1 Utilities and Solvers . . . . . . . . . . . . . . . . . . . . . . . . 28 3.1.2 Case structure in OpenFOAM . . . . . . . . . . . . . . . . . . . 29 3.2 OpenFOAM Discretization . . . . . . . . . . . . . . . . . . . . . . . . . 30 3.2.1 Spatial discretization . . . . . . . . . . . . . . . . . . . . . . . . 32 3.2.2 Time discretization . . . . . . . . . . . . . . . . . . . . . . . . . 34 3.2.3 Momentum-Pressure Coupling . . . . . . . . . . . . . . . . . . . 34 3.2.4 Implementation of Turbulence Model . . . . . . . . . . . . . . . 35 3.3 Simulation Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . 36 3.4 Solvers, Smoothers and Preconditioners . . . . . . . . . . . . . . . . . . 37 4 Computational Methodology 39 4.1 Computational domain . . . . . . . . . . . . . . . . . . . . . . . . . . . 39 4.2 Initial and Boundary conditions . . . . . . . . . . . . . . . . . . . . . . . 40 4.3 Time step selection . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 42 4.4 Mesh Generation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 43 4.4.1 Procedure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44 4.4.2 Reﬁnement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47 4.5 Mesh dependent study . . . . . . . . . . . . . . . . . . . . . . . . . . . 51 5 Results and Discussions 55 5.1 Frequency spectrum analysis . . . . . . . . . . . . . . . . . . . . . . . . 55 5.2 Instantaneous ﬂow . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 62 5.3 Mean ﬂow parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . 67 5.4 Mean ﬂow statistics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 71 6 Conclusion and Future work 78 6.1 Conclusion on thesis . . . . . . . . . . . . . . . . . . . . . . . . . . . . 78 6.2 Recommendations for future work . . . . . . . . . . . . . . . . . . . . . 80 Bibliography 82 Appendices 88 A controlDict 88 B fvSolution 93 viii
- Contents C fvSchemes 97 D meshDict 100 E Mesh comparative study 103 ix
- List of Figures 2.1 Energy spectrum of length scales. a) High energy region, b) transfer of energy region c) dissipation region [36] . . . . . . . . . . . . . . . . . . 13 2.2 Filtering operation for a ﬂow variable [38] . . . . . . . . . . . . . . . . . 15 2.3 Examples of three mesh design during grid reﬁnments [38] . . . . . . . . 19 2.4 Sub-Grid length scale [38] . . . . . . . . . . . . . . . . . . . . . . . . . 22 2.5 Blending function proﬁles [38] . . . . . . . . . . . . . . . . . . . . . . . 24 3.1 Case Structure of incompressible IDDES simulation . . . . . . . . . . . . 30 3.2 Finite Volume Method . . . . . . . . . . . . . . . . . . . . . . . . . . . 31 3.3 General overview of log ﬁle . . . . . . . . . . . . . . . . . . . . . . . . 37 3.4 Schematic overview of OpenFOAM simulation . . . . . . . . . . . . . . 38 4.1 Schematic of computational domain for simulation . . . . . . . . . . . . 40 4.2 ICEM CFD mesh . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41 4.3 Velocity magnitude contour for structured mesh generated using cfMesh . 45 4.4 Computational domain geometry . . . . . . . . . . . . . . . . . . . . . . 45 4.5 Patch ﬁle example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 46 4.6 File format conversion from STL to FMS format using command surfa- ceToFMS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 46 4.7 Volume reﬁnement using sphere and cone objects . . . . . . . . . . . . . 48 4.8 Patch reﬁnement for sphere . . . . . . . . . . . . . . . . . . . . . . . . . 48 4.9 Prismatic layers using boundaryLayers dictionary . . . . . . . . . . . . . 49 4.10 Velocity contour for mesh validation . . . . . . . . . . . . . . . . . . . . 50 4.11 Pressure contour for mesh validation . . . . . . . . . . . . . . . . . . . . 50 4.12 Y+ contours; (a) Course Mesh, M1 (b) Medium Mesh, M2 (c) Fine Mesh, M3 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 52 4.13 Cut plane and Zoom view; (a) Course Mesh, M1 (b) Medium Mesh, M2 (c) Fine Mesh, M3 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 52 4.14 Time history of Lift and Drag Coefﬁcient plots for entire simulation time t=9.048, showing transition stage passes after 75D/U time units or 1.1sec. 53 x
- List of Figures 4.15 FFT analysis at Probe location-9 showing non-dimensional vortex shed- ding frequency for (a)M1=0.181 (b)M2=0.211 and (c)M3=0.203 . . . . . 54 5.1 Location of computational probes and lines . . . . . . . . . . . . . . . . 55 5.2 FFT analysis of the streamwise velocity ﬂuctuation at probe P9 (x/D = 2.0, r/D = 0) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 57 5.3 Time history and FFT analysis at different locations: (a,b) radial velocity and FFT of it at probe P1, (c,d) radial velocity and FFT of it at probe P2, (e,f) radial velocity and FFT of it at probe P9, (g,h) radial velocity and FFT of it at probe P4 . . . . . . . . . . . . . . . . . . . . . . . . . . . . 59 5.4 Energy dissipation in downstream of sphere wake (a) Probe location P9 (x/D = 2.0, r/D = 0), (b) Probe location P4 (x/D = 3.0, r/D = 0.6) . . 60 5.5 (a)Time history of streamwise velocity at probe P9, and (b) time history of pressure coefﬁcient at P2 . . . . . . . . . . . . . . . . . . . . . . . . . 61 5.6 Cross-correlation between streamwise velocity ﬂuctuation at probe P9 and pressure coefﬁcient at probe P2 . . . . . . . . . . . . . . . . . . . . 62 5.7 Vortex shedding at every quarter time period using Q-iso-surfaces (advan- cing from (a) to (d)), in X-Y plane . . . . . . . . . . . . . . . . . . . . . 65 5.8 Vortex shedding at every quarter time period using Q-iso-surfaces (advan- cing from (a) to (d)), in X-Z plane . . . . . . . . . . . . . . . . . . . . . 66 5.9 Instantaneous contours of pressure coefﬁcient, Cp; (a) Coarse mesh, M1; (b) Medium mesh, M2; and (c) Fine mesh, M3 . . . . . . . . . . . . . . . 68 5.10 Instantaneous contours of non-dimensional skin-friction coefﬁcient,(τ/(ρU2 Re0.5)); (a) Coarse mesh, M1; (b) Medium mesh, M2; and (c) Fine mesh, M3 . . . 69 5.11 Angular distribution of mean pressure coefﬁcient and skin friction coefﬁ- cient around sphere; compared with experimental results of Kim & Durbin[14] at Re = 4200, Bakic[16] at Re = 50000 and DNS results of Seidle et al.[24] at Re = 5000. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 70 5.12 Streamwise velocity proﬁle along the wake centre line . . . . . . . . . . 71 5.13 Streamwise velocity proﬁle for M1, M2 and M3 at three locations in the wake, compared with the experimental data of Kim & Durbin at Re=3700 72 5.14 Mean velocity proﬁles along the wake centre line . . . . . . . . . . . . . 73 5.15 Mean streamwise and radial (cross-stream) velocity proﬁle at different locations in the wake of sphere . . . . . . . . . . . . . . . . . . . . . . . 75 5.16 Fluctuating mean streamwise and radial (cross-stream) velocity proﬁle at different locations in the wake of sphere . . . . . . . . . . . . . . . . . . 75 5.17 Contours of normalised mean Reynolds stresses for (a) Coarse mesh, M1; (b) Medium mesh, M2; and (c) Fine mesh, M3 . . . . . . . . . . . . . . . 76 xi
- List of Figures 5.18 Contours of normalised mean shear stress and Turbulent kinetic energy for (a) Coarse mesh, M1; (b) Medium mesh, M2; and (c) Fine mesh, M3 . 77 E.1 Vortex shedding at same time period for all three mesh using Q-iso-surfaces, in X-Y plane . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 103 E.2 Instantaneous streamwise velocity contours for; (a) Coarse mesh, M1 (b) Medium mesh, M2 and (c) Fine mesh, M3 . . . . . . . . . . . . . . . . . 104 E.3 Instantaneous cross-stream velocity contours for; (a) Coarse mesh, M1 (b) Medium mesh, M2 and (c) Fine mesh, M3 . . . . . . . . . . . . . . . 105 E.4 Instantaneous Mach number contours for; (a) Coarse mesh, M1 (b) Me- dium mesh, M2 and (c) Fine mesh, M3 . . . . . . . . . . . . . . . . . . . 106 xii
- List of Tables 2.1 Values of constants in Spalart-Allmaras model . . . . . . . . . . . . . . . 17 3.1 Utilities in OpenFOAM . . . . . . . . . . . . . . . . . . . . . . . . . . . 28 3.2 Incompressible solvers in OpenFOAM . . . . . . . . . . . . . . . . . . . 29 4.1 Initial values for simulation . . . . . . . . . . . . . . . . . . . . . . . . . 42 4.2 Summary of simulation time and DESModelRegions for all three mesh . 43 4.3 M1, M2, M3 representa the coarse, medium and ﬁne mesh while exper- imental data for vortex shedding Strouhal number and separation angle from Achenbach [1, 2] and drag coefﬁcient from Schlichting [55] . . . . . 51 5.1 Probes locations used initially for ﬁnding the correct positions to captures the main frequencies associated with the ﬂuctuations . . . . . . . . . . . 56 5.2 Mean ﬂow statistical data, DES (present simulation) results compared with DNS and LES results at Re=10000 . . . . . . . . . . . . . . . . . . 67 5.3 Mean ﬂow statistics compared with DNS results of Rodriguez et al.[7] at Re = 3700 and LES results of Constantinescu & Squires[29] at Re = 104 . 74 xiii
- Nomenclature Abbrevations Cd Drag Coefﬁcient Cf Skin-friction Coefﬁcient CFD Computational Fluid Dynamics CFL Courant Number Cl Lift Coefﬁcient Cp Pressure coefﬁcient CV Control Volume DDES Delayed Detached Eddy Simulation DES Detached Eddy Simulation DNS Direct Numerical Simulation FFT Fast Fourier Transform FV Finite Volume GAMG Geometric-algebraic multi-grid solver IDDES Improved Delayed Detached Eddy Simulation LES Large Eddy Simulation PBiCG Preconditioned Bi-Conjugate Gradient PCG Preconditioned Conjugate Gradient PISO Pressure Implicit with Splitting of Operators xiv
- Nomenclature RANS Reynolds Averaged Navier-Stokes S-A Spalart-Allmaras turbulence model SGS Sub-Grid Scale SIMPLE Semi-Implicit Method for Pressure-Linked Equations St Strouhal number URANS Unsteady Reynolds Averaged Navier-Stokes WMLES Wall Modeled Large Eddy Simulation Greek Symbols ∆ Filter width m δ Boundary layer thickness m ε Energy dissipation rate m2/s3 κ Von Karmann constant − µ Dynamic viscosity m2/s ν Kinematic viscosity m2/s νt Turbulent viscosity m2/s τw Wall shear stress N/m2 ˜ν Modiﬁed turbulent kinematic viscosity m2/s Roman Symbols ρ∞ free-stream density kg/m3 P Cell centroid − R Neighbouring Cell centroid − ˜d DES length m c Speed of sound m/s Ck Kolmogorov constant −
- Nomenclature dw Wall distance m f Frequency 1/s fb Step function - IDDES − fe Elevating function - IDDES − k Wave number 1/s lhyb Hybrid RANS-LES length scale m M∞ free-stream Mach Number − Q Second invariant tensor − U∞ free-stream velocity m/s uτ Friction velocity m/s vivj Velocity components m/s y+ Distance in wall units − Mathematical Symbols ¯u ﬁltered velocity m ∇ Nabla operator − lDES DES model length scale m q Energy source term − Re Reynolds number − t Time s u Velocity ﬂuctuations m/s xvi
- Chapter 1 Introduction 1.1 Background and Motivation The ﬂow around bluff bodies such as vehicle aerodynamics, ﬂow around wings at hight angle of attack, interaction of gust with buildings, heat transfer improvements, among others are some of the large number of examples which are of great interest for vari- ous engineering applications. Prediction of ﬂow around such bluff bodies which shows massive separation, are still remain one of the greatest challenges to the Computational Fluid Dynamics (CFD). Truth be told, the investigation of turbulent ﬂow past canonical geometries can be valuable to explore these complex ﬂow structures and additionally to give valuable data for validation of CFD models (e.g. LES, DES models). In this sense, the fundamental approach of the present work is to investigate the turbulent ﬂow past a sphere at sub-critical Reynolds number (laminar boundary layer separation; transition to turbulence occurs in the separated shear layer). Prediction of ﬂow at supercritical Reyn- olds number (turbulent boundary layer separation), increments the burden on the model, essentially through the need to predict the growth of boundary layer and separation, which is under the control of RANS model in characteristic DES applications. The cost of en- tire domain LES at supercritical Reynolds number is not a long way from that of Direct Numerical Simulation due to resolution needed to capture the turbulence structure, inside the slender attached boundary layer. The unsteady ﬂow past a sphere at sub-critical Reynolds number has an intricate nature characterized by the transition form laminar to turbulent ﬂow in the detached shear layer, the presence of a turbulent wake behind the sphere and unsteady shedding of vortices. This turbulent ﬂow has been object of numerous experimental and numerical studies [1, 2, 3, 4], most of studies provided the data of ﬂow visualization, angular distribu- tion of skin-friction and pressure coefﬁcients over the sphere surface, vortex shedding frequency and drag coefﬁcient, among others. In the most recent decades Reynolds- 1
- 1. Introduction Averaged Navier-Stokes equations (RANS), Large Eddy Simulations (LES) and Direct Numerical Simulation (DNS) have turned out to be effective tool for giving time-accurate helpful data about the ﬂow behaviour. However, one of the important requirements of the simulation of complex turbulent ﬂow is the expensive measure of computational assets expected to convey them out. That is why, majority of numerical simulations of the ﬂow over sphere have been carried out in the laminar regime [5, 6]. However, for turbulent re- gime there are still very few time-accurate calculations carried out [4, 7]. Besides, a large number of the numerical works reported since now have been performed utilizing differ- ent turbulent models, including Large Eddy Simulations (LES) [8, 9, 10] and Detached Eddy Simulations (DES) [11]. While the geometry is straightforward, the ﬂow around the sphere is very complex to analyse, having a signiﬁcant number of difﬁculties that are hard to precisely capture in nu- merical models. In this work, ﬂow ﬁeld behaviour are obtained using Detached Eddy Sim- ulation (DES), a hybrid method which basically reduces to Reynolds-Averaged Navier- Stokes (RANS) treatment close to the wall and turns into Large Eddy Simulation (LES)in the region away from solid surfaces, conditionally grid density should be sufﬁcient[12]. DES is a nonzonal method which is computationally feasible for high Reynolds number ﬂows, yet likewise determines time-dependent, three-dimensional turbulent motions as in LES. Past simulation results of this strategy have been good, yielding sufﬁcient expecta- tions over a wide range of ﬂows and likewise demonstrating that the computational cost has a weak reliance on Reynolds number, like RANS method, yet at same time give more reasonable description of unsteady effects. Despite the fact that extensive research available, analysis of mechanism for transition in shear-layer, behaviour and quantitative estimation of wake structure are still rare. There is a serious lack of detailed experimental and numerical data for sphere case, such as low frequency ﬂuctuations, separation angle, recirculation length, force coefﬁcients, among others, at higher Reynolds numbers. However to the best of our knowledge, there is no complete study for sphere case which consider the effects of low frequency ﬂuctuations in wake. While low-frequency ﬂuctuations in the wake of some other bluff bodies have been examined by few numerical studies. 1.2 Literature Review 1.2.1 Experimental Background Turbulent ﬂow past the sphere has been the subject of various experimental investigations [1, 2, 3, 13, 14, 15]. The essential interest for these investigations included visualization of primary vortical structure in the wake, understanding the mechanism of vortex shedding, 2
- 1. Introduction estimation of frequencies present in the wake, mean pressure coefﬁcient around sphere and streamwise drag. These studies also attempted to understand and explain the mech- anism through which wake become unstable. As the Reynolds number increases beyond the Re = 280, experiments demonstrate that the wake starts to shed vortices in a consistent manner. With the further increment in Reynolds number the shedding process truns out to be more unpredictable and complex, and, in the long run, the wake structure becomes chaotic. Since vortex loops diffuse very quickly, the examination of the wake conﬁgura- tion by the method of classical visualization techniques becomes troublesome. As far as anyone is concerned, except for the recent investigation by Bakic [16] at Re = 5 × 104, none of the above experimental investigation had provided the data for velocity compon- ents and Reynolds stresses in the wake which would be necessary for fully validating the expectations of a time-accurate numerical simulations. Chomaz et al. [13] recognized the two primary instability modes present in the wake, when vortex shedding is there. For Re > 280 large-scale vortices shed from the surface of sphere. The vortex shedding or the ﬁrst mode is identiﬁed to the large-scale shedding in the wake. At the limit between the recirculation zone and the exterior ﬂuid, this instability shows itself as a progressive wave movement with alternate ﬂuctuations produced by the shear. These ﬂuctuations decide the periodic shedding of the vortices that structure behind the sphere. The recirculation zone is deﬁnitely not axisymmetric. Beginning at Re = 800 there is a second high frequency mode (or spiral mode) connected with the small-scale shear-layer Kelvin-Helmholtz (K-H) instability on the fringe of the recirculation zone. This unsteadiness is capable for the distortion of large vortex structure and produce the vortex rings (subsequently vortex tubes), which shed in a quasi-coherent form inside of the detached shear layers, hence results in a production of small scale vortices, and, in the long run, transition to turbulence in the wake. The high frequency mode or the spiral mode instability is present just in an area limited to the wake immediately downstream of the sphere and in the detached shear layers, where it is more dominating then the ﬁrst or vortex shedding mode. These two instability modes can exists together all the while upto a threshold Reynolds number, however, experiment results shows some about its value. Although, most of the experiments discussed so far, caught both modes at Re = 104, results of Kim et al. [14] and Bakic [16] capture both modes up to Re = 105 and Chomaz et al were able to capture both modes at Re = 3 × 104. While Achenbach [2] failed to detect both modes beyond Re = 6×103 and Sakamoto and Haniu [3] beyond Re = 1.5×104. The relationship between frequencies and the structure of wake is the another issue of great interest. Sakamoto et al.[3] researched this in their experiment using hot wire as well as ﬂow visualization techniques. Their observe that, laminar hairpin-shaped vortices begins to shed at Re = 280 to form a completely laminar wake in periodic and regular 3
- 1. Introduction fashion. These hairpin vortices are shed regularly from Re = 280 to around 420 with frequency of same strength and in the same plane, so the the lateral forces coefﬁcient per- pendicular to shedding plane is zero all times. While from Re = 420to480,they observed that shedding direction starts oscillating which is conformed by DNS study of Mittal [17]. At the point when Reynolds number surpasses 800, periodically shedding vortex tube now covers whole near-wake region, and hairpin like vortices which were laminar earlier now becomes turbulent, however entire vortex sheet is still laminar which is separating from the sphere. Even now, as compared to the ones at low Reynolds number, the large struc- ture vortices still appear to keep up a hairpin-shaped form. Correspondingly, some scale vortex loops formed as small-scale vortex tubes shed into it, and as the move far from the sphere, interface with the large vortices. Kelvin-Helmholtz instability is subjected to these smaller vortex tubes which are laminar initially. Baric in his experiment was able to capture transition of these vortical structures into turbulence as accompany by roll-up and pairing processes. The vortex sheet begins to undergoes transition from laminar to turbulence at Re = 3 × 103 and ends around Re = 6 × 103 when it becomes fully turbu- lent. The experiment of Baric conforms that, change in the wake structure and integral parameters is very little with the increase in Reynolds number until very close to the crit- ical Reynolds number or until the drag crisis. That is, at separation the boundary layer over the sphere is laminar up to Recrit. Due to the complete transition to turbulence in the detached shear layer, stabilizing effect is generated which happens from Re = 7×103 to Recrit and results in more regular shedding pattern of the large-scale vortices. Con- versely, with the Reynolds number, the Strouhal number associated with the shear layer increases strongly since due to the smaller wavelengths the shear layer becomes unstable. At Re = 104 the value of Strouhal number is in the range of 1.8 − 2.5 and is detectable generally in the region of detached shear layer. Taneda [15] observe for Reynolds num- ber in between 104 −105 that oscillating wake in the azimuthal plane, rotates slowly and irregularly around the axis through center of the ﬂow, oriented parallel to the main ﬂow direction. Again, even Taneda in his experiment, did not observe any change in wake structure upto critical Reynolds number 1.2.2 Previous Numerical Investigation Several time-accurate simulations of laminar ﬂow over sphere using ﬁnite-element meth- ods were accounted among others by Mansoorzadeh et al. [18], Shen and Loc [19], Kalro and Tezduyar [20] and Aliabadi and Tezduyar [21], while Johnson and Patel [6] and Shirayama [22] used ﬁnite-difference method approaches. Depending on the authors, generally the onset of vortex shedding was seen in the range of Re = 280 − 400 and the considered Reynolds number were upto 103. As compared with the experimental data for Re 275−285, the onset of vortex shedding in these simulations are relatively spread very 4
- 1. Introduction large which in turns implies the different level of accuracy of these codes. These codes contributes in better understanding of vortex structure in the wake ad vortex-shedding mechanisms. Tomboulides and collaborators [4, 8] study the transition of near wake to turbulence by performing laminar, DNS and LES simulations. They correctly captured the onset of vortex shedding at around Re = 250−285 in their laminar simulation. For LES and DNS simulations, they limited the maximum Reynolds number of 2×104 and 103 respectively. To solve the incompressible Navier-Stokes equations the numerical method employed is a spectral element-Fourier algorithm, while for LES simulation the SGS model utilised was based on renormalization group theory.The reported value of Strouhal numbers re- lated to the shedding and spiral modes by Tomboulides and Orszag [4] is very close to the experimental value measured by Sakamoto and Haniu [3]; the Strouhal number for shedding was St = 0.2 which is within 10% of the experimental value. Another group, Kim and Choi [23] used LES for ﬂow over sphere from Re = 3.7 × 103 to 104 to study the change in the wake structure. These investigators used hybrid discretization (in lam- inar acceleration region, upwind and central difference elsewhere) and used the immersed boundary method in cylindrical coordinates to calculate the turbulent ﬂow past sphere. At low Reynolds number, the quantitative (velocity proﬁle in wake) agreements with the Experimental data of Kim and Durbin was goodwhile for both Reynolds number the mean pressure and drag coefﬁcient and shedding frequency were also in range of experimental results. DNS simulation is performed by another group, Seidl et al. [24] at Reynolds number of 5,000. They were able to capture the formation of initially laminar vortex tube successfully in the detached shear layers, and in addition the mechanism of roll-up and pairing and transition of these vortices. They also able to get correctly the values of drag coefﬁcient, Strouhal number, etc with their simulation. Schmid [25] performed several LES simulation using different SGS models (Smagorinsky, dynamic and no model) at Re = 5 × 104. To precisely capture the initial formation of vortex tube and its transition to turbulence, they utilizes the local grid reﬁnement in the separated shear layer using the ﬁnite volume method. They observed that the inﬂuence of SGS model is somewhat minor on mean ﬂow quantities. They had compared their data with the experimental observations of Bakic and overall agreement of mean ﬂow velocity proﬁle and its ﬂuctu- ations in the near wake region at same Reynolds number was in agreement. While this was conversely with the RANS simulation of Poon et al. [26], which was done on same Reynolds number ﬂow and in their agreement was poor for integral quantities as well as wake characteristics. The main observation for unmatched results is that they predicted the transition downstream then the experimental observed location which would effect the prediction of mean drag coefﬁcient value. Since the value of turbulent kinetic en- ergy is very high in the free stream, it can be possible that these problems caused due 5
- 1. Introduction to the set up of RANS or the mesh density in the separated shear layer. Drikakis [27] investigated the steady RANS simulation at subcritical and supercritical Reynolds num- ber using artiﬁcial compressibility solver using κ − ε model in conjunction at near wall, while another researcher group Koschel et al. [28] used no turbulence model at all for un- structured ﬁnite-element scheme. The achievement of these simulation results for getting mean quantities like pressure of drag coefﬁcient around sphere was restricted. Some of the recent simulation like, Constantinescu and Squires [29] simulate the ﬂow over sphere at Re = 104 using Large Eddy Simulation (LES) and Detached Eddy Sim- ulation (DES). They utilises the 0-type grid which is generated by revolving 2D grid in azimuthal direction and observed that both methods reproduce the main ﬂow characterist- ics and vortex shedding phenomena successfully. This group then again performed Direct Eddy Simulation (DES) for ﬂow over sphere at subcritical and supercritical regimes at two different Reynolds number Re = 104 and Re = 105 [30], able to capture the mean ﬂow parameters this time which were in good agreement with the experimental results. As far as DNS results are concerned there is not much data available for time-accurate instantaneous and statistical ﬂow data because for three-dimensional (3D) simulation and time-accurate results demands running simulation for much longer time, adding to the computational resources there are also ﬁne grid for DNS simulation which further put load on resources. Then recently Lehmkuhl et al. [31] carried out simulation for ﬂow dynamics of wake behind sphere at Re = 3700 and 10,000, they performed some through analysis on unstructured grid by rotating it in azimuthal direction, further more they also consider the low-frequency ﬂuctuation which effect the shrinkage and enlargement of re- circulation zone. They have concluded that the vortex formation region is related to the base-suction coefﬁcient Cpb. They are also able to successfully capture all three dominant instabilities, i.e.large-scale vortex shedding, small-scale Kelvin-Helmholtz instability and modulation of the recirculation which occur at very low frequency fm, further to their analysis, they also pointed out that with increase in Reynolds number the length of recir- culation zone decreases. Their results are in good agreement with experimental results. 1.3 Thesis Objectives The main task of the thesis is to simulate ﬂow over automotive body taking sphere as a test case here. Its is known that ﬂow over bluff bodies causes turbulence in the wake which effects the aerodynamic properties. There are some low-frequency ﬂuctuations in the wake which is hard to capture and require longer simulation time in order to predict it accurately. In previous section we have discussed some of the instabilities associated with the ﬂow over sphere and effect of low-frequency among them which causes shrinkage and 6
- 1. Introduction enlargement of recirculation bubble. Next two chapters described that hybrid RANS-LES model could be an appropriate approach for such kind of ﬂows. Therefore, following are the important consideration which discussed in this study throughout: 1. An open source numerical tool which can able to simulate the incompressible, un- steady turbulent ﬂow. 2. A turbulence model which can able to capture turbulent ﬂow features such as vortex shedding, among others, and even then it should be computationally less expensive. 3. A good mesh in for open source tool since it is known that tools like OpenFOAM are highly sensitive to mesh quality. 4. Selection of suitable initial and boundary conditions, accurate discretization schemes and solver settings. 5. Time period selection in order to capture the the clear footprints of low-frequency ﬂuctuations. 6. Validation of results for instantaneous and mean ﬂow parameters with previous ex- perimental and numerical results at comparable Reynolds number. 1.4 Outline The general outline of thesis is as follow, the ﬁrst chapter-1 highlights the previous experi- mental and numerical background of ﬂow over sphere case and provides the overall intro- duction to the shedding mechanism. Chapter-2 discuss the hybrid numerical method util- ised in thesis, a detail discussion of DES, DDES and IDDES approach is given. Chapter-3 provides the detail procedure of numerical tool used and set up for the case with some basic focus on governing equations used in solver. Chapter-4 discuss the computational domain, mesh procedure with CfMesh and reﬁnements used for generating all the meshes. Chapter-5 discuss the results and validate the numerical results of thesis with experimental and numerical results present in literature. The last chapter-6 conclude the research with some of the recommendations for future work. 7
- Chapter 2 Physics and Modelling 2.1 Governing Equation The objective of this thesis is to simulate the ﬂow around sphere at subcritical Reynolds number of 10,000 which represent the external ﬂow aerodynamics as a test case. Sine the ﬂow is at low Mach number M = 0.2 (Incompressible ﬂow) and subjected to Newtonian ﬂuid properties, hence to describe the ﬂuid dynamics of the ﬂow here, Navier-Stokes equation can be assumed as a governing equation. There are basically ﬁve equations consists in a Navier-Stokes equation, ﬁrst one is the continuity ((2.1), represents mass is conserved), three momentum equations for each direction ((2.2), represents momentum is conserved) and last one is the energy equation (2.3, represents energy is conserved). Dρ Dt = ∂ρ ∂t +∇.ρu = 0 (2.1) ρu Dt = ∂ρu ∂t +∇.(ρuu) = −∇p+∇.(µ∇u)+ f (2.2) Dρe Dt = ∂ρe ∂t +∇.(ρue) = −∇pu+∇.(µu∇u)−∇q (2.3) where, D/Dt = ∂/∂t + u∇ is know as Substantial derivative. Whereas ρ, p,e are the density, pressure and total internal energy. While u represents the velocity magnitude for all three directions and the symbol ∇ refers to as Nabla operator which is deﬁned as: 8
- 2. Physics and Modelling ∇ = ∂ ∂x , ∂ ∂x , ∂ ∂x (2.4) Since the ﬂow is consider as incompressible ﬂow because of low Mach regime, hence it results in a homogeneous and constant density across whole domain. The assumptions made here, results a simpler form of Navier-Stokes equation due to the absence of any external forces such as body forces or gravity. Also, the temperature is considered con- stant and assumed that it doesn’t have any inﬂuence on the ﬂow ﬁeld dynamics. All of the assumptions made here reduces the number of unknowns to just four (all three velocity components and pressure), while the energy equation can be omitted, equation 2.3. Hence the resulting equations would be: ∇.u = 0 (2.5) ∂u ∂t +∇.(uu) = − ∇p ρ +∇.(ν∇u) (2.6) 2.2 Turbulence models and Numerical methods The external ﬂow in Automotive engineering is inherently connected to the turbulence. It is a phenomena which exists in various engineering and industrial applications. Due to its wide existence, it is one of the most researched topic of CFD so far and hence there are various ways available by which different turbulent scale which exists in a turbulent ﬂow can be computed. Among all the techniques available, Direct Eddy Simulation is the one which provides the most ’exact’ solution of Navier-Stokes equation since it solves all the scales in turbulence and hence doesn’t require modelling at all. However DNS has some serious drawbacks: 1. It has a very very high requirement of computational power (e.g. cost of DNS scale is ∝ Re3), hence it make DNS very costly for daily use or for initial test simulations. 2. Since the number of cell require to carry out DNS simulation is ∝ toRe9/4, hence large domain size would result in millions of cells for large Reynolds number and reducing the domain would results some non-physical changes in ﬂow dynamics. For Automotive applications we need a large far ﬁeld to damp out any possibility of wall effect behind the body of interest. 9
- 2. Physics and Modelling Then there is another method which models the smallest scale (kolmogorov scale) and computes the most important large scales, knows as Large Eddy Simulation (LES). Whereas the third one and the most used one in industries is the Reynolds Averaged Navier-Stokes equation (RANS) which model a very wide range of turbulent length scales. Now days, a hybrid approach is emerged which combines the advantages of RANS and LES together, this method is used in thesis. Firstly some of the basic principles of RANS and LES are discussed. 2.2.1 RANS principle The Navier-Stokes equations 2.5 and 2.6 can be represents in cartesian coordinate system, xi(i = 1,2,3). Hence the incompressible equations can be written as: ∂uj ∂xj = 0 (2.7) Dui Dt ≡ ∂ui ∂t +uj ∂ui ∂xj = − 1 ρ ∂ρ ∂xi +ν ∂ui ∂xj∂xj (2.8) where ui is the cartesian components of velocity In RANS (Reynolds-Averaged Navier-Stokes equation) method, we averaged out all the unsteadiness in the ﬂow and regarded as a part of turbulence. Hence the ﬂow velocity is represented as the sum of two terms: ui(xi,t) = ¯ui(xi)+ui(xi,t), (2.9) where, ¯ui(xi) = lim T→∞ 1 T T 0 ui(xi,t)dt (2.10) Where T represents the averaging interval, it should be large as compared to the typ- ical time scale of turbulent ﬂuctuations. While ui represents the time averaged value of ﬂuctuation. For unsteady ﬂow problems, ensemble averaging is used in place of time averaging. The ensemble averaging can be explained as variable that can be controlled (boundary conditions, energy, etc.) for a set of ﬂows who are identical but initial conditions are generated randomly. This will give ﬂows that differ considerably from one another. Hence 10
- 2. Physics and Modelling an ensemble average is deﬁned as an average over large set of such ﬂows. Can be written as: ¯ui(xi) = 1 N N ∑ n=1 uni(xi,t) (2.11) Where N represents the number of members of the ensemble. For Reynolds averaging (unsteady ﬂow) we apply the ensemble average approach to the incompressible continuity equation 2.7, gives ∂ ¯uj ∂xj = 0 (2.12) We take the mean of the left hand side of the momentum equation 2.8, since mean of convective term is not a easy task because of nonlinearity. Hence equation can be written as: Dui Dt = ∂ ¯ui ∂t + ∂(uiuj) ∂xj (2.13) Using equation 2.9 for non linear term gives: uiuj = ( ¯ui +ui)( ¯uj +uj) (2.14) = ¯ui ¯uj +uj ¯ui +ui ¯uj +uiuj = ¯ui ¯uj +uj ¯ui +ui ¯uj +uiuj = ¯ui ¯uj +uiuj (2.15) Since, uj ¯ui = uj ¯ui = 0 (2.16) Using equation (2.15) with equation (2.13), we get Dui Dt = ∂ ¯ui ∂t + ¯uj ∂ ¯ui ∂xj + ¯ui ∂ ¯uj ∂xj + ∂(uiuj) ∂xj (2.17) Using incompressible mean velocity, equation (2.17) simpliﬁes to 11
- 2. Physics and Modelling Dui Dt = ∂ ¯ui ∂t + ¯uj ∂ ¯ui ∂xj + ∂(uiuj) ∂xj (2.18) Now taking the mean of the other terms in momentum equation results in Reynolds (RANS) equation. ∂ ¯ui ∂t + ¯uj ∂ ¯ui ∂xj = − 1 ρ ∂ ¯p ∂xi +ν ∂ ¯ui ∂xj∂xj − ∂uiuj ∂xj (2.19) Equation (2.19) can be written in a simpliﬁed form as: ρ ∂ ¯ui ∂t + ¯uj ∂ ¯ui ∂xj = ∂ ∂xj − ¯pδij + µ ∂ ¯ui ∂xj + ∂ ¯uj ∂xi −ρuiuj (2.20) On the left hand side, the term in square brackets represents the sum of three stresses; namely, − ¯pδij represents the mean pressure, the second term represents the viscous stress from the momentum transfer and the last term −ρuiuj, is the ﬂuctuating velocity. This term is called Reynolds stresses. The Reynolds stresses are components of symmetric second order tensor, where the diagonal components represents normal stresses while non-diagonal components repres- ents shear stresses. Half the trace of the Reynolds stresses give the turbulent kinetic energy, k, given by: k = 1 2 ρuiui (2.21) Since, six more unknowns are introduced because of the six independent elements due to symmetry of the Reynolds stress tensor hence, in order to close the system, i.e. number of unknowns equal to the number of equations, we need to model the Reynolds stresses in one of the ways given in literatures [32, 33] Turbulence consists of different size eddies, the largest eddies which are highly un- stable in a ﬂow, break up and hence transfer their energy to smaller eddies which are also unstable and break up again to transfer their energy to yet smaller eddies. This is know as energy cascading and continues until the Reynolds number Re(l) ≡ u(l)l/ν is sufﬁciently small so that eddy motion is stable and molecular viscosity is effective in dissipating the kinetic energy [34]. 12
- 2. Physics and Modelling 2.2.2 LES principle Smagorinsky [35], gives the idea and basic theory of LES in 1963. The largest scale eddies, according to theory of Kolmogorov are the eddies which contain most of the energy and do most of the transportation hence these eddies are one of the most important one in turbulence and are calculated directly. While the smallest scale eddies can be easily modelled since they are assumed to behave uniformly. This is the concise basic principle of Large Eddy Simulation (LES). Generally expressed, this implies the smaller scales contributes a small amount of the total energy while the larger scale contain the dominant part of the energy. This can be outline by the turbulent energy cascade or energy spectrum, Figure 2.1. The straight dotted line is also deﬁned in ﬁgure which represents the Kolmogorov’s law and is deﬁned as: E(k) = Ckε2/3 k−5/3 (2.22) Where Ck = 1.5, ε is the energy dissipation rate, and k is the wavenumber which is in- versely proportional to the length scale. Figure 2.1: Energy spectrum of length scales. a) High energy region, b) transfer of energy region c) dissipation region [36] In above Figure 2.1, energy spectrum is divided into three sub-regions: 13
- 2. Physics and Modelling 1. Integral length scale: This is the ﬁrst region and is characterized by largest eddies which contain the dominate part of energy, denoted by ki. 2. Inertial subrange: The second region in which eddies follows the Kolmogrov’s law. In this region mostly the transfer of energy from large to small scale is happing hence it is dominated by transitive scale. 3. Dissipative range: The last and third region contains the smallest scale eddies who’s behaviour is dominated by the viscosity and energy transfer from the larger scale eddies. Like in Reynolds-Averaged Navier-Stokes equations (RANS), 2.2.1; we do some aver- aging to model the large scale, in Large Eddy Simulation (LES) we apply ﬁltering. The scale separation is performed using this ﬁltering, which is the locally derived weighted average of the ﬂow properties over a volume of a ﬂuid. The ﬁlter width ∆ is one of the important feature in ﬁltering operation. ∆ is selected in such a way that, turbulent length scale larger then it are held in the ﬂow while the Sub-Grid Scales (SGS) or the smaller scales then ∆ should be modelled. In this way we can write any turbulent ﬂow variable, like ﬂow velocity, as a sum of large and small scale. ¯u = u−u (2.23) The resolved larger scale is represented by overbar while smaller scale are represented by prime. The ﬁlter process for large scale is obtain by: ¯u = u(x )G(x,x ;∆)dx (2.24) Where (x,x ;∆) is know as ﬁlter function and it should satisfy the condition: G(x,x ;∆)dx = 1 (2.25) The schematic representation of one-dimensional ﬁltering operation for one of the ﬂow variable is shown in Figure 2.2. The implicit top-hat ﬁlter is a standard ﬁlter applied in OpenFOAM (standard ﬁlter for Finite Volume methods), which takes an average over a rectangular region (Some other ﬁlters are also exist such as, Gaussian ﬁlter or sharp hat ﬁlter [37]). The local and averaged value of ¯u will be equal if we choose ﬁter width equal to the grid spacing. It is given by: G(x,∆) = 1 ∆, if | x |≤ ∆ 2 0, otherwise (2.26) 14
- 2. Physics and Modelling Figure 2.2: Filtering operation for a ﬂow variable [38] 2.2.3 Filtered Navier-Stokes equation Equation of motion is obtained for resolved large scales by applying ﬁlter to the incom- pressible Navier-Stokes equation (2.8), the ﬁltered equations are denoted by overbar: ∂ ¯ui ∂xi = 0 (2.27) ∂ ¯ui ∂t + ∂ ∂xj ( ¯ui ¯uj) = − 1 ρ ∂ ¯p ∂xi + 1 ρ ∂τR ij ∂xj +ν∇2 ¯ui (2.28) A dependency is caused between unresolved and resolved scales due to the non-linear convective term of Navier-Stokes equation. The impact of the unresolved scales are con- solidated in the subgrid-stress tensor, which includes the residual stresses and it is char- acterized by: τR ij = ρ(uiuj − ¯ui ¯uj) (2.29) 15
- 2. Physics and Modelling To deﬁne the unresolved scales, an Eddy viscosity model is utilized in LES. Hence stress tensor becomes: τR i j = 2ρνt ¯Sij + 1 3 δijτR kk (2.30) Where νt represents turbulent or eddy viscosity. Which gives us: ∂ ¯ui ∂t + ∂ ∂xj ( ¯ui ¯uj) = − 1 ρ ∂ ¯p ∂xi +2 ∂ ∂xj [(ν +νt) ¯Sij] (2.31) Above equation (2.31) represents the ﬁnal Filtered Navier-Stokes equation, now the last step is to give the deﬁnition of turbulent-viscosity (νt). 2.3 Turbulence closure model In the thesis we used Spalart-Allmaras (S-A) turbulence model to determine the turbulent viscosity (νt). Since S-A model use only one additional equation hence it is relatively simple. The modiﬁed turbulent kinematic viscosity (˜ν) is introduced as the only addi- tional unknown in the equation. Modiﬁed turbulent viscosity is deﬁned by [39]: νt = ˜ν fv1 (2.32) where, fv1 = χ3 χ3 +c3 v1 χ = ˜ν ν Here, ν is the molecular viscosity, cv1 is a contant and ˜ν represents the modiﬁed turbulent viscosity or the working variable, giving the transport equation: D˜ν Dt = cb1 ˜S˜ν + 1 cσ [∇.((ν + ˜ν)∇˜ν)+cb2(∇˜ν)2 ]−cw1 fw ˜ν ˜d 2 (2.33) ˜S = ω + ˜ν κ2 ˜d fv2 (2.34) 16
- 2. Physics and Modelling fv2 = 1− χ 1+ χ fv1 (2.35) Where ω represents magnitude of vorticity while function fw is given by: fw = g 1+c6 w3 g6 +c6 w3 1/6 (2.36) g = r +cw2(r6 −r) (2.37) r = ˜ν ˜Sκ2 ˜d2 (2.38) The values of constants deﬁned above is tabulated in Table 2.1 Constant Value cb1 0.135 cb2 0.622 cw2 0.3 cv1 7.1 cσ 2/3 κ 0.41 cw3 2 cw1 cb1/κ2 +(1+cb2)/cσ Table 2.1: Values of constants in Spalart-Allmaras model 2.4 RANS-LES Hybrid approach In Hybrid methods, for region near the wall they typically utilises the solution of another set of model equations. The region where turbulent boundary layer is solved in a zonal hybrid methods is deﬁned for a region in the vicinity of the wall. While explicit boundary condition is prescribed for communication to the outer LES region. Where as a smooth transition between different regions is made in a blended hybrid methods. Spalart and Allmaras [40] was the ﬁrst to propose the most widely recognized type of a hybrid RANS-LES method in 1992, name as, Detached Eddy Simulation (DES). It combines the advantages of both Reynolds-Averaged Navier-Stokes (RANS) and Large Eddy Simulation (LES) together, which is the basic thought behind this approach. In 17
- 2. Physics and Modelling a more explanatory way, this hybrid RANS-LES method acts as only RANS mode in attached boundary layer and transform into LES mode only for detached ﬂow regions. From the region of unsteady RANS equations to the region where standard LES is solved, a smooth transition is produced for these blended hybrid methods, while this kind of switching between RANS and LES relies on the local-grid resolution. Piomelli et al. [41] had shown that due to the interface treatment resulting form transition layers in DES, results in decrease of skin friction for these blended approaches. This section give the overview of the kind of errors in Detached Eddy Simulation (DES) and Delayed Detached Eddy Simulation (DDES) while dealing with these models and next section 2.5 provide the solution to overcome these kinds of errors. 2.4.1 Detached Eddy Simulation (DES) In a classic Detached Eddy Simulation (DES), a limiter combines the standard Spalart- Allmaras RANS model with its Sub-Grid Scale (SGS), deﬁned by: lDES = min{dw,CDES∆} (2.39) where lDES represents the model length scale, dw is the distance to the wall(given by destructive term of Spalart-Allmaras model), CDES is the derived constant whose value is 0.65 and ∆ is the largest local-grid spacing: ∆ = max{∆x,∆y,∆z} (2.40) In Detached Eddy Simulation (DES), near the wall (dw < CDES∆) in a attached boundary layer, a classic S-A RANS is acting, while away from the wall (dw > CDES∆) in a separa- tion region, a SGS model is acting with a ﬁlter CDES∆. Despite the fact that this turbulence model is most common and utilized for several years, regardless it experiences a few dis- advantages. Issues emerges when separation region is smaller then the thick boundary layer in a wall bounded ﬂows. For this situation, often the boundary layer thickness is larger then the grid spacing parallel to the wall ∆|| or in other words, it grid become ﬁne enough in for DES length-scales, parallel to the wall such that the LES branch follow through it in accordance to equation 2.39. Due to this a phenomena is developed which is called Grid Induced Separation (GIS) [42, 40] according to it, as a consequence of ﬁner grid, the eddy viscosity reduces below the RANS level but the velocity ﬂuctuations which are driving the LES content (or resolved Reynolds stresses) have not replaced the modeled Reynolds Stresses. Hence, these ’missing stresses’ causes the reduction in skin friction. Figure 2.3 represents the basic grid examples to give the overview of grid importance. The Figure 2.3a shows the grid in which wall-parallel spacing ∆|| is larger then the 18
- 2. Physics and Modelling (a) Grid spacing larger then the boundary layer (b) Grid spacing smaller then the boundary layer,too coarse for LES (c) Grid spacing to support LES content Figure 2.3: Examples of three mesh design during grid reﬁnments [38] boundary layer thickness δ, due to it, in entire the boundary, the DES length-scale is equal to the RANS type (lDES = dw). Figure 2.3c shows the grid wall-parallel grid spacing less than to boundary layer thought the domain, traditionally this represents the pure LES type grid, therefore in most of the boundary layer the SGS model is activated (lDES = CDES∆) while only in vicinity of wall a RANS model is activated (lDES = dw). In Figure 2.3b, the wall-parallel grid spacing is not as small as for pure LES grid therefore deep in the bound- ary layer, a SGS model of DES is originated. It can not able to capture all the velocity ﬂuctuations since the grid is not ﬁne enough at this point. Besides, without the acquaint- ance of resolved stresses to re-established the balance the modeled Reynolds stresses and eddy viscosity will be reduced. In literature this phenomena is called Modeled Stress Depletion (MSD). 2.4.2 Delayed Detached Eddy Simulation (DDES) The equivocal grid like Figure 2.3b give rise to the problem like Modeled Stress Depletion (MSD), hence the method is formulated to avoid these error, called Delayed Detached Eddy Simulation (DDES) which is just a simple modiﬁcation of classic Detached Eddy Simulation (DES) and similar to the shear-stress transport model proposed by Menter et 19
- 2. Physics and Modelling al. [43]. The noticeable feature of DDES is that, to deﬁne length-scales it utilises some blending functions. Even if due to the grid spacing the DES limiter is activated even though DDES maintains the full RANS mode by detecting the boundary layer which is dependent on the eddy viscosity and therefore on solution as well. As explained by the Haase et al. [44], even if blending function showing that point of interest is inside the boundary layer, it declines to change into LES mode. As an outcome, the transition between LES-RANS is more abrupt. Hence, the DDES is degigned in such a way that it wipe out the errors caused by DES to a grid reﬁnement like MSD or GIS. Menter et al. [43] has given the blending functions F1 and F2 which utilises the RANS model internal length scale and the wall distance. At the boundary layer, these function are 1 and at the edge of the boundary layer they reduces rapidly to 0. A para- meter ”r” is utilized in one equation models (S-A model) since internal length scale is not present, this parameter is deﬁned as the ratio of model length-scale to the wall distance and is given for S-A model as: rd = νt +ν max[ Ui,jUi,j,10−10].κ2d2 w (2.41) Where Ui,j represents velocity, κ is Von Karman constant and dw represents the wall distance. ”fd” in log layer is equal to 1 while it reduces to 0 at the edges and is given by: fd = 1−tanh(8rd)3 (2.42) It is 0 in whole domain except in LES region (rd << 1) where it reduces to 0. In contrast to the old deﬁnition of DES length-scale given by equation 2.39, a new deﬁnition given by equation 2.43 also consider the modiﬁed length scale which depends on turbulent or eddy viscosity in comparison to to old deﬁnition where only grid dependency is considered. lDES = dw − fdmax(0,dw −CDES∆) (2.43) Now with the new deﬁnition of lDES, based on value of rd even if fd shows point is well inside the boundary layer, it is possible to reject the LES mode. 2.5 Improved Delayed Detached Eddy Simulation (IDDES) Another Improved turbulence method is the Improved Delayed Detached Eddy Simula- tion (IDDES) which overcomes the errors of previous two Classic Detached Eddy Simu- lation (DES) and Delayed Detached Eddy Simulation (DDES). This method consolidate the advantages of Delayed Detached Eddy Simulation (DDES) and Wall Modeled Large 20
- 2. Physics and Modelling Eddy Simulation (WMLES), which is the main objective of IDDES model. An alternate approach is applied to overcome the larger grid resolution requirement which is the basic demand of classic LES, is known as Wall Modeled LES. Taking example, Schumann [45] has given a wall-stress model in 1975, has utilized the empirical derived wall functions along with velocities by considering the ﬁrst off-wall point in log-layer to calculate an approximation for wall stresses at the boundary. Then again, it is likewise conceivable to utilize the DES for these WMLES as was successfully attempted by Nikitin et al. [46]. The log-layer mismatch (LLM) error is encountered mostly with WMLES, between the LES and RANS regime. Actually sim- ulation gives two log layers: outer most layer when distance to the wall is greater then the local grid size while the RANS model give the inner layer. Due to the mismatch error LLM, an error of under-prediction of 15 to 20% was noticed in inner and outer layer. Even though, in comparison to LES, WMLES still save lot of computing time. The IDDES is developed in such a way that it gives one formula set for both WMLES and DES applic- ations and also avoid the LLM so that it can be used for complex geometry for different ﬂows inside a single simulation. The IDDES method can be sub-divided into four parts to demonstrate how it works [40, 44, 47, 48]. 2.5.1 Modiﬁcation of the Sub-grid length-scale Common deﬁnition of sub-grid scale for classic LES in most of the literature is give as the cube root of a cell volume, deﬁned as: ∆ = (∆x)2 +(∆y)2 +(∆z)2 (2.44) Moreover, for the classic DES (section 2.4.1) the decision of the sub-grid length scale is dependent on maximum of three cell dimensions 2.40. Both deﬁnitions give rises to a problem more precisely with the constants of SGS, which ought to have different con- stant values for various ﬂow regimes such as free/pure turbulent ﬂow (Decaying Isotropic Homogeneous Turbulence) or for wall-bounded ﬂows. Hence another deﬁnition was set up to avoid the requirement of different values for different ﬂow regimes. In this new deﬁnition the main idea is to include some wall-distance dependency which gives the a new deﬁnition of sub-grid length scale: ∆ = f(∆x,∆y,∆z,dw) (2.45) Where dw represents the wall distance hence new formula depends on both, the local cell size and the wall distance. Therefore three equations can be given by dividing compu- tational domain into three sub-domains. First one is given by the maximum local-grid 21
- 2. Physics and Modelling spacing just like for classic DES since grid is mostly isotropic away from the wall and hence it is set as a classic DES case, given by: ∆free = ∆max ≡ max(∆x,∆y,∆z) (2.46) Second one is given by equation 2.47, the sub-grid length scale in the region close to the wall should not follow the drop of the wall-normal step. The sub-grid length scale in this region is deﬁned by wall parallel grid only: ∆wall = const(dw) = f(∆x,∆z) (2.47) Third and the last one is deﬁned as, region between the away from the wall and the region close to the wall is assumed to follow as a linear function of dw for the sub-grid length scale. Furthermore an assumption is made for ∆ that it varies in the range ∆min ≤ ∆ ≤ ∆max. Combining all the above statements yields one single equation: ∆ = min{max[Cwdw,Cw∆max,∆wn],∆max} (2.48) Where Cw = 0.15 is a constant based on developed channel ﬂow for LES and ∆wn is the grid spacing in wall-normal direction. Figure 2.4 is a typical representation of sub-grid Figure 2.4: Sub-Grid length scale [38] length scale for a channel ﬂow, where solid line is valid when ∆ ≤ Cwdw. Furthermore as long as dw ≤ ∆max is valid the value of ∆ remains constant, at this point ∆ =Cw∆max. When the maximum cell size dimension becomes less then the distance to the wall, dw > ∆max 22
- 2. Physics and Modelling the SGS grows explicitly with ∆ =Cwdw. As the maximum value is reached ∆max, the SGS remains constant afterwards. The dashed line represents basically a strong wall-normal stretching. The value of SGS remain constant near to the wall, Cw∆max. Once ∆wn > Cw∆max, the value of SGS grows explicitly until maximum cell size is reached. It is well understood that rate is smaller comparatively in the second case since it is unacceptable for simulations. In contrast to the different SGS models, the IDDES approach utilizes a very complex method of assessing the grid ﬁlter. Other then the wall normal distance, cell dimensions and height of the cell in wall normal direction have their impact in the formulation of the grid ﬁlter. 2.5.2 DDES branch of IDDES When inﬂow conditions are not turbulent then the ﬁrst branch corresponds to DDES is activated. The DDES length scale is given by: lDDES = lRANS − fdmax(0,lRANS −lLES) (2.49) with lLES = CDESΨ∆ and lRANS = dw The delaying function is given by equation 2.42. Compared to the classic DES length scale,there is one more factor ψ. The purpose behind the addition of ψ is on the ground that ﬂow Reynolds number decreases due to decrease in the sub-grid eddy viscosity with grid reﬁnement. Sooner or later, the DES will miss- translate and behave like in the vicinity of a wall. As a result, the turbulent viscosity will drop with respect to the surrounding velocity and length scales through fv and ft functions. The functions for Spalart-Allamars model relies on the ratio of the turbulent viscosity to the molecular viscosity, can be deﬁnes according to S-A model: νt/ν or χ ≡ ˜ν/ν. Moreover, CDES value increased effectively due to the Ψ factor. For Spalart-Allamars model this shield function Ψ(νt/ν) is deﬁned as: Ψ2 = min 102 , 1− cb1 cw1κ2 f∗ w [ft2 +(1− ft2)fv2] fv1max(10−10,1− ft2 (2.50) Where constant κ is equal to 0.424. If the sub-grid turbulent viscosity is larger than 10ν, then the correction become inactive (ψ = 1) and for lower values it becomes stronger. 2.5.3 WMLES branch of IDDES In WMLES branch, as opposed to the DDES branch, it will be activated only when ﬂow is turbulent and unsteady and have an adequate grid ﬁneness to resolve eddies in boundary 23
- 2. Physics and Modelling layer. The coupled RANS-LES length scale is utilised to accomplished coupling amongst them, it is given by: lWMLES = fB(1+ fe)lRANS +(1− fB)lLES (2.51) Where fB, blending function is given by: fB = min{2exp(−9α2 0,1.0} (2.52) Where α is equal to 0.25− dw hmax The blending function fB is determine by the fast switch- ing mechanism profound inside the boundary layer, between pure RANS and LES modes, this transition is found in the range of 0.5hmax < dw < hmax wall distance as shown in Fig- ure 2.5. The main idea behind this function is to provide rapid transition between modes, for pure RANS mode it is equal to 1 while 0 for LES mode. Another function is deﬁned as Figure 2.5: Blending function proﬁles [38] in equation 2.53 is called an "elevating" function. It is formulated to balance the excessive decrease in modeled Reynolds stress (RANS), which is encountered in the region of inter- action between RANS and LES interface and thus treats the logarithmic-layer mismatch. fe = max{(fe1 −1,0}Ψfe2 (2.53) 24
- 2. Physics and Modelling While the function fe1 is deﬁned as: fe1 dw hmax = 2exp(−11.09α2), if α ≥ 0 2exp(−9.0α2), if α < 0 (2.54) Since α = 0.25, hence clearly fe1 does not depends the solution but only depends on grid. Therefore this function works for RANS component as an elevating for blended length- scale given by equation 2.51 for RANS-LES. In transition zone when fB < 1, the function fe = fB. While function fe2 is given by fe2 = 1.0−max{ ft, fl} (2.55) In equation 2.51, for RANS component the intensity of elevating is control by the function fe2 by utilizing function ft and fl, deﬁned as: ft = tanh (c2 t rdt)3 (2.56) fl = tanh (c2 l rdl)10 (2.57) Here turbulent νt and laminar ν viscosities are represented by subscript t and l respect- ively, while rdt and rdl are functions which are analogue to function rd and is expressed by equation 2.41. The parameters rdl and rdt will be around one laminar layer and in log region of turbulent boundary layer, respectively. Where as ct and cl are constant para- meters deﬁned for different models. The function fe2 depends on the solution since both functions ft and fl are analogue to function rd and hence also depends on the solution while in boundary layer both functions are around one and enforce functions fe1 and fe2 to become 0. 2.5.4 Hybrid branch of DDES and WMLES For different kind of grid and simulations, the idea is to develop a method which will automatically switch and select WMLES or DDES mode. A reformulation of length scale of DDES is necessary since with the current deﬁnitions of length scales for DDES or of WMLES this was not possible. The new deﬁnition is given by: ˜lDDES = ˜fdlRANS +(1− ˜fd)lLES (2.58) 25
- 2. Physics and Modelling While modiﬁed blending function is given by: ˜fd = max{(1− fdt, fb} (2.59) Where fdt is given as: fdt = 1−tanh[(8rdt)3 ] (2.60) The coupled hybrid length scale for both branches DDES and WMLES is given now as: lhyb = ˜fd(1+ fe)lRANS +(1− ˜fd)lLES (2.61) It is pointed out that when ﬂow is turbulent, the function fdt is around 1 since rdt << 1. Furthermore, ˜fd = fB in order to lhyb approaches to lWMLES. While if the ﬂow is laminar, then the function fe becomes 0 and lhyb approaches to ˜lDDES. 26
- Chapter 3 Software and Methodology This section gives the overview of softer utilized in this thesis and the computational meth- odology used to achieve the objective. Since there are already much literature available to use such methodologies hence this chapter provide a more general overview to perform LES simulations. Moreover, general structure and solver used are also addressed. 3.1 OpenFOAM OpenFOAM is an object-oriented free open source software which refers to Open Field Operation and Manipulation. It has basically a collection of libraries, OpenFOAM has functionality to connect these libraries to solve CFD problems. OpenFOAM is written in ﬁnite volume code, hence equation are discretised in ﬁnite volume approach and the solu- tion is re-written to conform the approach[49]. The main philosophy behind OpenFOAM is to make it available for every user to modify and re-write any functionality in it (under General Public License). Under GNU license, OpenFOAM Foundation ensures that it remain free for all and anyone can contribute to its development, this philosophy leads to its rapid development and hence it become most widely utilized open source CFD solver. Even though every year OpenFOAM foundation aims to provide new and improved ver- sion of OpenFOAM (till now version 3.0.1), still version 2.2 and 2.4 are widely used in academic and industrial applications. This thesis address OpenFOAM version 2.4, it has solvers for compressible and incompressible ﬂows to simulate laminar or turbulent ﬂows (RANS, LES, DES) and heat transfer problems. Another attraction with OpenFOAM is that it the development team provides range of webinars, consultancy and training support for industrial users, however for academic enthusiast users it is no cost widely available open source solver which has a functionality to perform as the user desire. The key feature of OpenFOAM is that its ﬁnite volume code is written in C++ lan- guage which is widely used among industry and academics. It also has a precompiled 27
- 3. Software and Methodology utilities and solvers and also equipped with pre- and post-processing utilities which en- able users to perform complete simulation free of cost. Hence, the beneﬁts mentioned above has a potential to ﬁnd users since it provides both technical and economical bene- ﬁts. 3.1.1 Utilities and Solvers OpenFOAM provides many utilities which helps in mesh generation, pre-precessing and post-processing applications which are available to users in entire work ﬂow. This sec- tion provides some of the utilities which aids in thesis, since the meshing is done with another software hence it will be address in later part of the thesis. It is essential to bring out the fact for new users that OpenFOAM doesn’t provide GUI even though there are various GUI available for OpenFOAM but mostly are not endorsed by OpenFOAM de- velopers, the convenient way interact and communicate with it is via written commands in a terminal window. In terminal the prospective user give the name of solver or utility to perform tasks and information for a particular utility can be found via entering a commant ’-help’ in a terminal window. Some of the utilities are given in table 3.1. Utility Task blockMesh Ofﬁcial block mesher in OpenFOAM snappyHexMesh Automatic mesh reﬁner for complex geometries checkMesh Check mesh quality and report statistics DESModelRegions Gives the volume percentage over which RANS and LES is working forceCoeffs Lift, Drag and Moment coefﬁcients probes Specify the probe for sampling probeLocations Show the probes locations yPlus Report and calculate the y plus for wall patches wallShearStress Report and calculate shear stress for wall patches decomposePar Automatically decompose the domain for parallel processing reconstructPar Automatically reconstruct the decomposed domain data Table 3.1: Utilities in OpenFOAM The solver utilised in thesis is the incompressible transient solver "pimpleFoam", which combines the PISO and SIMPLE algorithm together while maintaining the nu- merical stability even with higher time steps, this solver is used in cojuction with both 28
- 3. Software and Methodology RANS and LES turbulence models hence for IDDES simulation it would be a perfect choice. Besides the pimpleFoam solver there are many incompressible as well as com- pressible solver present in OpenFOAM 2.4, some of the common incompressible solver based on case structure and set up are explained in table 3.2. For speciﬁc problem these solvers (computer executable) provide ﬁnd the solution using the algorithms of a particu- lar solver. Utility Task icoFoam A incompressible solver for transient ﬂows that can be applicable to low Reynolds number applic- ations like; small MAVs or UAVs, internal ﬂuid system. simpleFoam A incompressible solver for steady state ﬂows util- ises SIMPLE algorithm and can be used for both laminar and turbulent ﬂow by using RANS in background. pisoFoam A incompressible transient solver utilising PISO algorithm and can be used in conjunction with both turbulence models RANS and LES. pimpleFoam A incompressible transient solver utilising both PISO and SIMPLE algorithms in conjunction. This solver can be used for larger time steps while provide the numerical stability during simulation. It can be used in conjunction with both turbulence models RANS and LES. Table 3.2: Incompressible solvers in OpenFOAM 3.1.2 Case structure in OpenFOAM Domain region (liquid or solid) or the system of equations are speciﬁcally connected to the set up, case structure and design of an OpenFOAM simulation. This sub-section il- lustrate the case structure and conﬁguration of incompressible IDDES simulation (shown in Figure 3.1). Inside case folder, there are three sub-directories which require to set up simulation, in particular 0, constant and system. The user deﬁnes the boundary conditions in 0 directory for simulation which contains one ﬁle each for IDDES variables, namely, pressure, velocity, Sub-grid scale viscosity and S-A turbulent variable. While the simu- lations requirements which remain same through out the simulation are deﬁned in con- stant directory, it has sub-directories like polyMesh which contains the mesh information, 29
- 3. Software and Methodology transportProperties ﬁle contains the ﬂuid type, RASProperties contains the S-A closure model while LESProperties contains the LES model constants and turbulenceProperties contains the information of type turbulence model (LES). The last and most important folder which decide stable or diverging simulation is the system folder, it contains atleast three important ﬁles, i.e., controlDict ﬁle which contains the information of start and end time as well as the time step size, fvSchemes ﬁle which contains the equation discret- ization schemes and last one is fvSolution which contains the information of numerical algorithms to be used for solving system of equations. Figure 3.1: Case Structure of incompressible IDDES simulation 3.2 OpenFOAM Discretization As mentioned in previous section 3.1, OpenFOAM utilises Finite volume method for LES simulations. This section provides the overview of how equations are discretized in OpenFOAM and which numerical schemes are used in thesis. Even though there are 30
- 3. Software and Methodology some schemes which provide much better and accurate results but this is beyond the topic of research right now in this thesis. Some of the default simulation schemes are also used in this research work. The basic idea behind the Finite Volume Method (FVM) is to sub-divide or discretize the domain in space. Since due to the need of solving the equation in time for unsteady simulation, time-marching method is needed which makes the equations semi-dicretize to solve the problem. Figure 3.2: Finite Volume Method A set of arbitrary shaped Control Volumes (CV’s) are needed for spatial discretization, and for each control volume a computational point P is deﬁned (example, Figure 3.2). From the adjacent cell (N) to the current cell (P), a vector d connect the cell centres of the two, while A represents the normal area vector between the cells for common face. OpenFOAM deﬁnes it variables in this way which results in collocated grid. As mentioned earlier, for unsteady simulation a temporal discretization is necessary, or in other words the time interval or time steps (∆t) are required time marching from the initial conditions. The task is to discretized the ﬁltered Navier-Stokes equation (2.28) of incompressible, Newtonian ﬂuid for LES simulation. After integration of control volume and time using Finite Volume Method (FVM, yields: V ∇. ¯udV = ∂V dA. ¯u = 0 (3.1) 31
- 3. Software and Methodology t+∆t t d dt V ¯udv+ V ∇.( ¯u ¯u)dV − V ∇.νef f (∇ ¯u+∇ ¯uT )dv dt = − t+∆t t V ∆ ¯p ρ dV dt (3.2) The above equation is in second-order due to the presence of the diffusion term which introduced the second derivative. Since we now that in order to get accurate results, the order of discretization of equations need to be higher than or equal to the second-order. Moreover, due to the second order spatial discretization, higher or second-order temporal discretization would results in much better and time accurate solution. Now by applying Tylor series to the transport quantities we wold get: φ(x) = φP +(X −XP).(∇φ)P +ϕ |X −XP|2 (3.3) ∂φ(t) ∂t = φ(t +∆t)−φ(t) ∆t +ϕ(∆t) (3.4) Sub-sections below provides the discretization for each term in governing equation, ﬁrstly spatial discretization is discussed followed by temporal. 3.2.1 Spatial discretization The general discretization integrals utilized for evaluation on control volumes are dis- cussed here, for more through knowledge one can refer to Jasak [50]. Volume Integral : Vp φ(x)dV ≈ φPVP (3.5) Sur face Integral : f φdA = φf Af (3.6) Divergence Integral : VP ∇.φdV ≈ ∑ f Af .φf (3.7) 32
- 3. Software and Methodology Gradient Integral : VP ∇φdV ≈ ∑ f Af φf (3.8) Convective term discretization The Divergence integral (equation 3.7) is applied to the convective term for discretization. It gives: VP ∇.( ¯uφ)dV = ∑ f A.( ¯uφ)f = ∑ f (A.( ¯u)φf = ∑ f Fφf (3.9) Where the volume ﬂux through face is given by F = A. ¯Uf . To get values at faces, second order interpolation is required between the two neighbouring cell values P. Diffusive term discretization Discretization for diffusive term is given by: VP ∇.(ν∇φ)dv = ∑ f A.(ν∇φ)f = ∑ f νf A.(∇φ)f (3.10) By using an interpolation, the scalar term νf can be easily found out. While the term A.(∇φ)f is highly depended on the mesh, like in equation 3.10, the face gradient φ for orthogonal mesh can be deﬁned while the vectors A and d are parallel to each other for such kind of meshes. A.(∇φ)f = |A| φN −φP |d| (3.11) Here P and N are neighbour cells. For non-orthogonal meshes, the equation 3.11 is not valid any more for second order accurate equations. An additional term is introduces which represents the non-orthogonality. A.(∇φ)f = |Ad| φN −φP |d| orthogonal + A∆. ∇φ non−orthogonal (3.12) The instability can be arise if mesh non-orthogonality is very high since it will create negative coefﬁcients, which results in reduced accuracy due to limited correction. That is why a user should always aim for limited non-orthogonality while generating a mesh. 33
- 3. Software and Methodology 3.2.2 Time discretization Temporal discretization also have various ways for discretizing time just like the spatial discretization. The transport equations need to be second-order accurate which is the most critical thing to remember here. One example of the temporal discretization is the Cranck- Nickolson scheme which is the expensive and undesired in this research but provide most accurate result, another option is the second order backward differencing scheme. Backward Differencing The temporal discretized equation is given by 3.13, which provides second order accuracy by utilising three time steps to achieve it. ∂φ ∂t = 3 2φn+1 −φn + 1 2φn−1 ∆t (3.13) While perfoming the simulation, one try to minimize the turncation errors, still there are time’s when some errors are introduced due to small variations in face ﬂuxes. These kind or errors has some serious effects in LES simulation since they cause an additional diffusion. The main problem arises when these errors go beyound the sub-grid diffusion. Due to this reason, the cell face Courant number is always try to set below 1 in order to maintain stability. CFL = ¯uf .n |d| (3.14) This is the reason behind using very small time step in this research work since it results in very small temporal diffusion error. 3.2.3 Momentum-Pressure Coupling Since the thesis consider the PIMPLE algorithm which utilises the merger PISO-SIMPLE algorithm and hence it uses the idea of SIMPLE mode (relaxation), since we run sev- eral simulations to obtain the best inner-outer corrector loops (explained in section 3.3) therefore current simulation doesn’t utilises the relaxation factor idea instead we set the tolerance of 10−6 by observation of test simulation results which should be enough for transient simulations. In PIMPLE algorithm, the momentum equation is calculated ﬁrst after that the pres- sure equation is calculated and this new pressure is used to re-calculate the momentum equation which in turns give new pressure by using this new momentum (explained in schematic overview of OpenFOAM in Figure 3.4). 34
- 3. Software and Methodology Thi ﬁnal Navier-Stokes equation is given below: (full derivation is not presented here) ap ¯up = H −∑ f A ¯pf (3.15) ∑ f A 1 ap f (∇ ¯p)f = ∑ f A. H ap f (3.16) One can refer to literatures [36] and [50] for full derivation of above equations. Here ap represents the set of coefﬁcients depending on ¯up. While H vector consist all the terms like source and convection part except the pressure term. Pressure Implicit with Splitting of Operators (PISO) algorithm coupled with SIMPLE advantage is preferred for transient simulations, like in this research work. 3.2.4 Implementation of Turbulence Model Since we are dealing with Spalart-Allmaras turbulence model in this research work which was already discussed in section 2.3, it equations follow the classic disctretization method similar to the one which are discussed so far, hence recalling Spalart-Allmaras equation once again: ∂ ˜ν ∂t +∇.(˜ν ¯u)− 1 σ ∇.((ν + ˜ν)+∇˜ν) = cb1 ˜S˜ν production + 1 σ cb2(∇˜ν)2 transport −cw1 fw ˜ν ˜d 2 dissipation (3.17) where table 2.1 already represents the constant values and expression for functions. In order to increase stability of solution, we drive the production term as an explicit function of ˜νn−1. Given by: ˜νproduction = cb1 |∇× ¯u|+ ˜νn−1 κ2 ¯d2 fv2 ˜νn−1 (3.18) Discretizing transport term as: ˜νtransport = cb2 σ ∇˜nun−1 .∑ f A˜νf (3.19) 35
- 3. Software and Methodology Discretizing destructive term as: ˜νdissipation = − cw1 fw ˜νn−1 ¯d2 (3.20) Where n−1 refers to previous time step. 3.3 Simulation Overview This section emphasis the procedure of solving equation for LES simulation using discret- ized Navier-Stokes equations which are already discussed. Figure 3.3 gives the general overview of simulation, where Final Residual is the tolerance. Steps involved in PIMPLE algorithm are brieﬂy discussed below: 1. For initializing the ﬂow ﬁeld and to start LES simulation, a RANS solution having velocity, pressure, eddy viscosity and face ﬂuxes is utilized. 2. The next step is to use previous time step for updating turbulence properties. 3. The momentum and pressure coupling is solved thrice using PIMPLE algorithm since nOuterCorrectors or nCorrPIMPLE is set to three (external loop correctors, which are set to 3). 4. The pressure within the PIMPLE loop is corrected twice using PISO algorithm since nCorrectors or nCorrPISO is set to two (internal loop corrector, which is set to 2). 5. The velocities are solved using previous ﬂow ﬁeld equation. A solver that re- quire a smoother smoothSolver applicable to symmetric matrices is applied. While symGaussSeidel "Symmetric Gauss-Seidel" is used as a choice of smoother. 6. The pressure equation are solved using PCG "Preconditioned Conjugate Gradient" solver which is applicable to symmetric matrices. While for a symmetric precon- ditioner "Diagonal Incomplete-Cholesky" DIC is used to improve computational efforts of simulation. 7. To sustain the convergence for pressure equation, the non-orthogonal corrector nNonOrthogonalCorrector which means the pressure ﬁeld is solved more often with new calculated value is set to 1. Due to it we can see the pressure equation 36
- 3. Software and Methodology is solved one more time in PISO loop. It is generally set to either 1 or 0 for LES simulations. ∇2 p = f(U,∇p) → pnew → ∇2 pnew = f(U,∇pnew) → till nNonOrthogonalCorr is reached 8. The number of outer and inner correctors are chosen in such a way that a certain tolerance (in this case it is 10−6) on the quantities is achieved. For this research case the outer corrector 3 and inner corrector 2 with non-orthogonal correctors 1 is found sufﬁcient to achieve certain tolerance in each iteration. Figure 3.3: General overview of log ﬁle 3.4 Solvers, Smoothers and Preconditioners Solvers, Smoothers and Preconditioners can save a lot of computational efforts when used properly. Figure 3.1 represent sub-directory fvSolution under system directory which contains these settings and conditioners. In Appendix B, applied setting for PIMPLE algorithm is provided. Generally considered most computational demanding equation is the pressure equation among others. The Diagonal Incomplete-Cholesky (DIC) was selec- ted as a preconditioner for pressure equation. According to CFDdirect [51], Geometric- algebric multi-grid solver (GAMC) would provide much accurate solution and increase the speed by corsen/reﬁne mesh in stages but during this research work it is found out that DIC is give more accurate results while GAMC is diverging (reason behind this is 37
- 3. Software and Methodology Figure 3.4: Schematic overview of OpenFOAM simulation beyond the scope of this thesis). Moreover it is realised that DIC speed up the solution and the tolerance limit is achieved in much earlier than GAMC. The Preconditioner Con- jugate Gradient (PCG) solver is utilized for solving pressure equation. The other terms are solved using smoothSolver in conjunction with Symmetric Gauss-Seidel (symGauss- Seidel) as a smoother for symmetric matrices. 38
- Chapter 4 Computational Methodology In previous section we have presented the physics and modelling approach (chapter 2) used in this thesis which is very small in comparison to the functionality of DES solution method; fortunately this part is widely explained in various literatures, text books and publications, hence only the important portion of DES simulation needed (e.g., ﬁltered Navier-Stokes equations, momentum-pressure coupling and solver used for resultant matrices) in thesis is presented in previous sections. However this section focus entirely on simula- tion set-up by ﬁrstly introduction of domain selection (including boundary and initial con- ditions) then time-step selection followed by mesh generation strategy and ﬁnally mesh dependent study. 4.1 Computational domain The unsteady simulations were performed in OpenFOAM with a sphere diameter D = 1, whose centre is located at coordinate (0, 0, 0). The computational domain (Figure 4.1) extends 4.5 diameters in upstream direction as well as in radial outward direction from the centre of sphere which corresponds to a blockage (area) ratio of approximately 1.2%. The blockage ratio here is deﬁned as the ratio of sphere frontal (Asphere = 0.785398163) area to the test section area (Adomain = 63.62). This is proportional to the sphere is hanging inside the circular pipe with a diameter of D = 9D (here D always represent the diameter of sphere). Here, the rate of decay of perturbation away from the body determines the extent of the upstream and radial computational domain. Since it is well known [52] that rate of decay of perturbation due to the presence of sphere is 1/r3, here r represents the distance from centre of the sphere. For two-dimensional bluff bodies (i.e. cylinder) the rate of decay of perturbations is 1/r2, for three-dimensional sphere case this factor is r times smaller than the corresponding one. Accordingly, the velocity at x = −4.5 is just 0.1% different form the initial velocity or the free-stream velocity, as per potential hypothesis. 39
- 4. Computational Methodology The same contention additionally holds in the radial direction. Moreover, the blockage factor of the order of 1% are viewed as insigniﬁcant when performing simulations or experiments as already mentioned in few literatures [2, 14]. While computational domain in downstream direction extends 25 diameter form the centre of sphere. As reported by Tomboulides and Orszag [4], simulation by performing domain length of 20 diameter in downstream direction (with same outﬂow boundary condition) didn’t have any effect in upstream direction. Still 25D is chosen due to the reason to have atleast 3 to 4 vortical structures shedding behind the sphere within the domain, it will increase the grid elements drastically which indeed increase the computational efforts. Figure 4.1: Schematic of computational domain for simulation Some mesh were generated with ICEM CFD during initial investigation represented in Figure 4.2 with more then 1 million cells for both structured and unstructured mesh but the simulation diverges every time after converting mesh in OpenFOAM format by using ﬂuent3DMeshToFoam. It is observe that after conversion the domain size increased in all three direction which can lead to the divergence due to no element present in the increased length. Further investigation is beyound the scope of current thesis work (remember that OpenFOAM is an open source code which can have bugs moreover the version used for this research is 2.4 which is older then the 2016 version 3.0.1). Further details about mesh is presented in section 4.4. 4.2 Initial and Boundary conditions The boundary conditions in OpenFOAM are provided in ﬁles for initial velocity, pres- sure and turbulent ﬁelds in 0 directory (Figure 3.1). Four patches are generated during meshing procedure namely; sphere patch, inlet patch, outlet patch and sides (represents the radial side of the computational domain). Numerous boundary conditions are imple- ment on ﬁnal set-up mesh according to simulations and experiments performed earlier, since OpenFOAM uses different names for deﬁning boundary conditions and due to lack 40
- 4. Computational Methodology (a) Structure mesh with 1.4 million elements (b) Unstructured mesh with 1.8 million elements Figure 4.2: ICEM CFD mesh of detailed documentation on it, the best and the most suitable boundary conditions are implemented. They are described in detailed below: 1. Sphere patch: The velocity ﬁeld is set as ﬁxedValue with value of (0,0,0) which as the name implies, the velocity over sphere patch is kept ﬁxed at 0 m/s in all directions. The pressure ﬁeld is set as zerogradient, which represents the normal gradient of pressure is zero or Neumann boundary condition. while ﬁxedValue of 0 for turbulent ﬁelds or Dirichlet boundary condition. 2. Inlet patch: The Dirichlet boundary condition or ﬁxedValue with a uniform value of free-stream in x-direction onlyU∞ = (68.058,0,0)m/s is speciﬁed. The free-stream velocity is calculated by using the Mach number of M∞ = 0.2, while dynamic and kinematic viscosity is calculated by using the Reynolds number formula (equation 4.1), taking free-stream conditions for density (ρ∞ = 1.225kg/m3), pressure p∞ = 101325 pascal, Reynolds number Re∞ = 10,000 and diameter of sphere D = 1m. Re∞ = ρ∞U∞D µ∞ (4.1) While for initializing pressure ﬁeld the Neumann type boundary condition is pre- 41
- 4. Computational Methodology scribed hence zeroGradient is used. Furthermore, turbulent ﬁeld is calculated using turbulent intensity of 0.1% which gives the value 0.071444734, a ﬁxedValue is set using this. 3. Outlet patch: Neumann and Dirichlet boundary condition for velocity and pressure ﬁeld respectively, is prescribed in literature [53]. While in OpenFOAM is found that Neumann type boundary condition for both ﬁelds (pressure and velocity) generates numerically induced oscillations which can easily be avoided by using inletOutlet boundary condition for velocity and turbulent ﬁeld (using same values as for inlet patch). Hence for a daring experiment this boundary condition is used and found suitable in current research work, while the pressure ﬁeld is set as ﬁxedValue with a value of 0 . 4. Sides patch: It represents the cylindrical domain around the sphere at it is set as symmetry boundary condition for every ﬁeld which is according to OpenFOAM guide represents the slip wall for non-planer patches. Initial Condition Value Re∞ 10,000 M∞ 0.2 ρ∞ 1.225kg/m3 p∞ 101325 pascal µ∞ 8.336×10−3 kg/ms ν∞ 6.805×10−3 m2/s nuTilda 0.071444734 D 1m Table 4.1: Initial values for simulation 4.3 Time step selection Since this research work used PIMPLE algorithm whose main attraction is stability of simulation for higher time steps, which can be used to advance in time much faster for unsteady simulation without compromising the stability of solution but some important physics can be skip if we use higher time step. Considering the total time required for running the simulation it would be expected to use higher time steps but in this thesis we are using much smaller time step to capture the effect of low-frequency ﬂuctuation which is the main task of thesis. Hence a time step is selected using the convection time which 42
- 4. Computational Methodology 50 times less then it. The convection time is given by time required by the ﬂow to pass the sphere which is equal to tconvection = D/U∞, calculated as 0.01469. Therefore the time step selected to carry out simulation is 0.00029, ∆t = 0.00029. Moreover the maximum Courant Number, CFL is set to 0.5 for whole simulation, if the mean Courant number value exceed 0.5 any time in simulation, the OpenFOAM reports divergence. Considering the low frequency ﬂuctuation, the time required to run entire simula- tion should be long enough to capture such low frequencies (more explanation is re- fchap:results), hence the current simulations are run for 9.048 seconds (see A) which corresponds to 120 vortex shedding cycles. According to the knowledge of literatures, this is the longest simulation for ﬂow over sphere at this Reynolds number). For calcu- lating the vortex shedding, the experimental value of vortex shedding Strouhal number fvs = 0.195 is used, which gives the frequency of one vortex shedding equals to 13.2713 therefore, corresponding time for one vortex shedding is equal to 0.07535. Using these calculations it is found out that for one vortex shedding almost 260 time steps are required which should allow enough time to capture the low-frequency content accurately. Mesh Number of CPUs Clock time RANS volume% LES volume% Coarse mesh, M1 32 34 : 47 : 30 ∼ 1.4Days 37.2 62.8 Medium mesh, M2 32 121 : 04 : 00 ∼ 5Days 30.7 69.3 Fine mesh, M3 32 195 : 13 : 01 ∼ 8Days 35.1 64.9 Table 4.2: Summary of simulation time and DESModelRegions for all three mesh 4.4 Mesh Generation The most challenging part faced during this process is the post-processing, since it not only require a complete understanding of how OpenFOAM work but also a requires a solid understanding of ﬂow physics (which is already discussed in 1) work for ﬂow over sphere case. Therefore the most crucial part of pre-processing is to generate a suitable mesh which represents the ﬂow physics as close as to the nature. Since a mesh generation is a time consuming process for complex geometries even with commercial software’s like ICEM CFD. Some initial meshes were generated using this software package which generate very good results in Ansys FLUENT but diverges in OpenFOAM after convert- ing mesh in it’s format. The potential reason behind it is already mentioned in section 4.1. Hence ICEM meshes are neglected for current research work. OpenFOAM has its own mesher snappyHexMesh which is considered very powerful meshing tool among OpenFOAM users. Even though it generates high quality mesh automatically, still it is not very popular among community due to two reasons, ﬁrstly 43
- 4. Computational Methodology it requires signiﬁcant amount of RAM memory for implementation and secondly, from usability viewpoint it is consider very cumbersome for generating inﬂation layers for high quality boundary layer grids. Therefore another open source software is consider in this thesis work which is explained in next section. 4.4.1 Procedure Due to the problem faced with commercial meshing package, ICEM CFD and due to the cumbersome nature of OpenFOAM own mesher snappyHexMesh, another open source software cfMesh is used to generate grid for simulations,it is a mesher for OpenFOAM provided by Creative Field company. It is a cross-platform library for automatic mesh generation that is built on top of OpenFOAM and it is compatible with all versions of OpenFOAM [54]. The Cartesian Mesh is generated using cfMesh, which offers structured mesh as well as Unstructured Tetrahedral mesh, since Tetrahedral meshes are well-known to not be optimal for OpenFOAM simulations among users (this statement wasn’t investigated due to time constrain). Hence a premilary test with Structured as well as Cartesian mesh was investigated to make the decision for ﬁnal type of mesh to be run. Since purely Structured mesh are better, at the condition that cells have a low skewness and/or are aligned with the ﬂow. While, Cartesian meshes ensures an optimized mesh quality (zero skewness, aspect ratio equalling one) in the quasi-totality of the domain. Structured mesh are known to converge better than tetrahedral meshes. It was shown that OpenFOAM could give bad results when cells are skewed or not well aligned with the mesh. The best illustration in our case is that the potentialFoam solver, used to initialized the velocity ﬁeld, failed to give physical results on a Structured mesh, when it worked ﬁne on the Cartesian mesh. The main problem to create a high quality structured mesh in our case is the presence of the sphere, which prevent cells to be aligned with the ﬂow close to it. Here, an illustration of this after few iterations on the structured mesh Figure 4.3a. For all these reasons, Cartesian mesh type is better than structured in our case. The Cartesian mesh generated using cfMesh generated a 3D mesh which containd mostly hexahedral elements while in transition region, polyhedral elements are present between the elements of different sizes. The procedure is detailed below, it worth mentioning here that Carterian mesh generated, introduced automatically one boundary layer which can be reﬁned further. 1. Geometry: The tool used to prepare the domain’s geometry (Figure 4.1) was Sa- lome, which provides a CAD module. 2. Patch Creation: Using Salome all patches were created separately namely; sphere, inlet, outlet and sides. Figure 4.4 shows the patch names. 44
- 4. Computational Methodology (a) Global view (b) Zoomed view Figure 4.3: Velocity magnitude contour for structured mesh generated using cfMesh Figure 4.4: Computational domain geometry 45
- 4. Computational Methodology 3. STL ﬁle preparation: Each patch was then exported in STL format. The name of the patch was manually added into each STL ﬁle (Figure 4.5 shows the example of sphere patch ﬁle). Finally, all STL ﬁles were concatenated (copy-pasted) into a single one. Figure 4.5: Patch ﬁle example 4. File conversion: The STL input ﬁle was converted into FMS format using command surfaceToFMS, which is recommended in the cfMesh documentation and allows the user to deﬁne OpenFOAM patch types (like patch, wall, symmetry, empty, etc.) before meshing instead of modifying them in the constant/polyMesh/boundary ﬁle after each mesh generation. Figure 4.6 shows the heading of the FMS ﬁle which was used: Figure 4.6: File format conversion from STL to FMS format using command surfa- ceToFMS 5. meshDict ﬁle: Finally two mandatory ﬁeld are edited in meshDict ﬁle (see, Ap- pendix D) to start the meshing process using cfMesh: 46

Publicidad