MSc Thesis - Jaguar Land Rover

MSc Thesis - Jaguar Land Rover
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 presented 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 simulations are carried out based on free-stream Mach number M∞ = 0.2 and sphere diameter 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, turbulence statistics are compared with previous experimental and numerical results available in literature for sub-critical Reynolds number. Specific consideration is dedicated to computing 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 shedding 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 coefficient 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 experimental 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 various 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 entire 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 distribution 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 regime 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 different 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 numerical 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 expectations 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 mechanism 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 configuration 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 components 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 structure 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 turbulent. 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 critical 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 number 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 methods 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 related 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 laminar 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 fluctuations 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 energy 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 number 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 unstructured 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 characteristics 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 recirculation 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 recirculation 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, unsteady 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 experimental 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 experimental and numerical background of flow over sphere case and provides the overall introduction to the shedding mechanism. Chapter-2 discuss the hybrid numerical method utilised 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 constant 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 typical 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 represents 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 unstable 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 averaging 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 incompressible 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 characterized 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 additional 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 separation 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 boundary 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 parameter ”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 simulation 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 applications 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 constant 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 computational 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 switching 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 interaction 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 respectively, 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 parameters 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 methodology 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 solution 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 version 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 benefits. 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 section 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 numerical 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 compressible 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 particular solver. Utility Task icoFoam A incompressible solver for transient flows that can be applicable to low Reynolds number applications like; small MAVs or UAVs, internal fluid system. simpleFoam A incompressible solver for steady state flows utilises 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 simulations requirements which remain same through out the simulation are defined in constant 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 discretization 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 discussed 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 several 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 pressure 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 ∇ñun−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 discretized 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 require 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 preconditioner "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 selected 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 simulation set-up by firstly introduction of domain selection (including boundary and initial conditions) 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, pressure 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 simulation 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 converting 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

MSc Thesis - Jaguar Land Rover

Recomendados

Más contenido relacionado

Presentaciones para ti(20)

Similar a MSc Thesis - Jaguar Land Rover(20)

Último(20)

MSc Thesis - Jaguar Land Rover