Good Practice in CFD. A rough guide.

Transcription

1 Good Practice in CFD. A rough guide. Prof. Neil W. Bressloff March 2018

2 Material covered Introduction External and internal flow The CFD process Geometry, meshing, simulation, post-processing The issues Test case 1 Test case 2 Test case 3 Test cases 4 & 5 Checklist Other resources For each of the steps in the CFD process The Reynold s number Verification and validation Simulation of flow over a 2D backstep Model selection Order of accuracy Mesh verification Simulation of flow over an airplane y + : the non-dimensional distance from the wall Turbulence model selection The drag prediction workshops (variation in CFD results) Pulsatile (unsteady) blood flow Verification of number of pulses, spatial and temporal spacing Verification in CFX (tank sloshing) and in OpenFOAM (rim-driven thruster) The things to consider for setting-up, running and post-processing a CFD simulation 2

3 Introduction external flow 3

4 Introduction external flow 2018

5 Introduction external flow 5

6 Introduction TOTALSIM 6

7 Introduction internal flow 7

8 Introduction internal flow 2018

9 Introduction biomedical flow 2018

10 Introduction the process Geometry > mesh > simulation Geometry > post-process Mesh Simulation The fourth sixth drag prediction workshop D1-9_DPW4-ANSYS-Marco-Oswald-new.pdf 10

11 Introduction Geometry > mesh > simulation flow rate m3/s non-dimensional time Bressloff, N. W., 2007, Parametric geometry exploration in the carotid artery bifurcation, J. Biomech., 40,

12 The issues - geometry Construct from scratch? OR Supplied geometry? Feature definition wrapping Outer domain (for external flow) Parameterisation 12

13 The issues geometry software Rhino CATIA DesignModeler Solidworks NX4 13

14 The issues - mesh Mesh tool? AND Mesh strategy? Boundary layer mesh? Mesh dependence? Computational cost? 14

15 The issues mesh software Harpoon Starccm+ ANSYS mesher ICEM CFD Solidworks 15

16 The issues - simulation Model definition? AND Solution strategy? Boundary conditions? Initial conditions? Monitoring? Convergence? 16

17 The issues simulation software Fluent Starccm+ CFX OpenFOAM 17

18 Reynold s number Why is Re important? Laminar > Transition > Turbulent Increasing Re Boundary layer behaviour/representation 18

19 Simulation accuracy? Which of the above Cp variations is correct? Is either of them correct? If so, how accurate are they? Do the associated solutions yield physically meaningful results? 19

20 The issues post-process Need to show quantitative results Explain the results Verification Validation Has this flow separated? Errors Significance 20

21 Verification & Validation Verification Check for correct setup Validation Check accuracy of results (preferably against experimental data) 21

22 Test case 1. 2D flow over a backward facing step

23 2D flow over a backward facing step validation 23

24 2D flow over a backward facing step the experiment 24

25 2D flow over a backward facing step flow settings 25

26 2D flow over a backward facing step - results 26

27 2D flow over a backward facing step 2D versus 3D 27

28 2D flow over a backward facing step simulation 28

29 2D flow over a backward facing step simulation Model definition? AND Solution strategy? Boundary conditions? Initial conditions? Monitoring? Convergence? Solver settings Mesh dependence Resolution Type Boundary layer mesh Memory Convergence Simulation time Hardware Parallel simulation 29

30 Solver setup: default settings Mesh spacing = 1mm 30

31 Solver setup: change to 1 st order Mesh spacing = 1mm 31

32 Solver setup: pressure algorithm set to 2nd order Mesh spacing = 1mm 32

33 Solver setup: pressure based; SIMPLE; 2nd order (finer mesh) Mesh spacing = 0.5mm 33

34 Solver setup: switch to SIMPLEC and use higher under-relaxation factors Mesh spacing = 0.5mm Higher under-relaxation factors Default values Note: 0.8 for momentum didn t converge 34

35 So SIMPLEC converges well with high under-relaxation factors. BUT.do we trust the solution? Mesh spacing = 0.5mm 35

36 Solver setup: pressure based; Coupled; 2nd order (switch from SIMPLEC for finer mesh) Mesh spacing = 0.25mm Test under-relaxation Switch to 1 st order Switch to 2 nd order Switch to coupled solver SIMPLEC Coupled Coupled Selecting Coupled from the Pressure-Velocity Coupling drop-down list indicates that you are using the pressure-based coupled algorithm, described in this section in the separate Theory Guide. This solver offers some advantages over the pressure-based segregated algorithm. The pressure-based coupled algorithm obtains a more robust and efficient single phase implementation for steady-state flows. It is not available for cases using the Eulerian multiphase, NITA, and periodic mass-flow boundary conditions. 36

37 Solver setup: The coupled solver 37

38 Solver setup: The coupled solver Mesh spacing = 0.5mm 38

39 Solver setup for mesh dependence Coupled solver is more robust and is recommended for steady-state solutions N.B. only incompressible flow considered here Use at least 2 nd order discretisation schemes Check convergence N.B. aim for at least three orders of magnitude Mesh dependence Consider at least four mesh resolutions Halve the mesh spacing each time 39

40 Mesh dependence: spacing of 1mm to 0.125mm 40

41 Mesh dependence x-component of shear stress on bottom wall. 41

42 2D flow over a backward facing step - results 42

43 Boundary (layer) mesh or inflation layer 1mm spacing 1mm spacing 5 layers 0.1mm first layer Growth rate = 2.0 Cell count increased from 6,000 to 10,069 43

44 Boundary (layer) mesh or inflation layer 0.5mm spacing 0.5mm spacing 5 layers 0.1mm first layer Growth rate = 1.5 Cell count increased from 24,353 to 31,366 44

45 Boundary (layer) mesh or inflation layer 0.25mm spacing 0.25mm spacing 5 layers 0.1mm first layer Growth rate = 1.2 Cell count increased from 99,844 to 105,407 45

46 Triangular cells spacing = 0.25mm Cell count increased from 99,844 to 211,589 46

47 The Lyceum cluster

48 Logging into the Lyceum cluster Normally, your supervisor will need to request access to the Lyceum cluster for you through serviceline Read the web-pages (including the wiki pages) Use secure shell to remotely login 48

49 Three scripts! First script requests a job to be run on the cluster Second script is the actual file that is run when the job is allocated to a compute node This will contain a command to run a simulation The third script will contain the commands needed by the simulation For example, read a particular mesh file and setup the solver, BCs etc 49

50 200 iterations of the 1mm mesh on the Lyceum cluster 50

51 Test case 2. 3D flow around a transonic aeroplane Fluent

52 Drag prediction workshop D1-9_DPW4-ANSYS-Marco-Oswald-new.pdf 52

53 DPW-4 - grid guidelines Grid Convergence Case NASA Common Research Model: Coarse (3.5M), Medium (10M), and Fine (35M) grids are required; The Extra-fine (100M) grid is optional Total grid size to grow ~3X between each grid level for grid convergence cases Initial spacing normal to all viscous walls (RE=5e+6 Based on C REF =275.80): coarse: y + ~ 1.0 dy = medium: y + ~ 2/3 dy = fine: y + ~ 4/9 dy = extra-fine: y + ~ 8/27 dy = ~ 0.04mm Recommended: generate grids with 2 cell layers of constant spacing normal to viscous walls Grid convergence cases must maintain the same grid family between grid levels, i.e. maintain the same stretching factors, same topology, etc. Growth rate of cell sizes in the viscous layer should be < Farfield located at ~100 C REF s for all grid levels. 53

54 DPW-5 - overview 54

55 Grid guidelines coarse grid..\articles\dpw4-ansys-marco-oswald-new_2009.pdf 55

56 Solver setup 56

57 Turbulence model selection ALSO consider how to model the near wall behaviour Is y + in the correct range? 57

58 RANS models descriptions 58

59 RANS models behaviour and usage 59

60 Near-wall treatment (y + ) y y p 60

61 Harpoon first mesh Mesh settings Surface cell size = 138mm BL settings Initial cell height = 20mm No. of layers = 3 Expansion rate = 1.3 Volume mesh: 389,585 cells Including BL mesh: 553,566 cells 39 seconds to create mesh 61

62 Harpoon-Fluent - first mesh y + 62

63 Harpoon second mesh Mesh settings Surface cell size = 69mm BL settings Initial cell height = 2mm No. of layers = 4 Expansion rate = 1.5 Volume mesh: 1,363,903 cells Including BL mesh: 2,238,970 cells 112 seconds to create mesh 63

64 Harpoon-Fluent second mesh y + 64

65 Harpoon third mesh Mesh settings Surface cell size = 69mm BL settings Initial cell height = 0.5mm No. of layers = 10 Expansion rate = 2.0 Volume mesh: 1,363,903 cells Including BL mesh: 3,521,225 cells 148 seconds to create mesh 65

66 Harpoon-Fluent third mesh y + 66

67 DPW- 5 summary - drag 67

68 DPW- 5 drag (turbulence models) Scatter is still large for coarser grids Best results for hex-based grids (even if unstructured) Discretisation and turbulence modelling major contributors to scatter 68

69 DPW4 summary - separation 69

70 DPW4 summary no separation 70

71 Test case 3. Coronary artery stent design (pulsatile flow) Starccm+

72 Coronary artery disease Coronary Artery Disease (CAD) is a condition caused by the accumulation of plaque (usually atheromatous or fibrous plaque) on the inner walls of the artery. (1) GNU Free Documentation License - (2) Creative Commons License - (3) Antonio Colombo and Goran Stankovic. Colombo s Tips & Tricks with Drug-Eluting Stents. Taylor and Francis Group,

73 Stents (1) National heart lung and blood institute (nlhbi). All.html. 73

74 Geometry construction Representative models of the ART stent and Bx VELOCITY are constructed using Rhinoceros 4.0 ART stent Flat model Bx VELOCITY Flat model 74

75 Problem formulation Blood flow in coronary arteries Flow type Dynamic Viscosity(μ) Inlet velocity profile Unsteady, Newtonian, Incompressible and laminar 3.7x10-3 Pa-s Density (ρ) 1.06 x 10 3 kg/m 3 Peak and mean blood velocities Peak and mean Reynolds number 77 & cm/s & 5.04 cm/s - Unsteady due to the pulsatile nature of blood flow -Blood behaves as a Newtonian fluid for shear rates higher than 100 s -1 (1) - Incompressible laminar flow for Reynolds numbers lower than 200 Inlet velocity profile (2) 1. Fung Y C 1993 Biomechanics: Mechanical Properties of Living Tissues vol 18 2nd edn (New York: Springer) 2. K. Perktold,M. Hofer, G. Rappitsch,M. Loew, B.D. Kuban, and M.H. Friedman. Validated computation of physiologic flow in a realistic coronary artery artery branch. Journal of Biomechanics, 31:217 28,

76 Simulation setup Governing Equations.(v) = 0 (1) ρ( v/ t) + ρ(v. v ) = - P + μ 2 v (2) Boundary conditions Numerical simulations are performed over a quarter stent to exploit symmetry Outlet: zero pressure Plane2: Periodic/cyclic boundary condition Stent & artery wall: No slip wall Inlet: velocity specified as a fourier series representing pulsatile blood flow Plane1: Periodic/cyclic boundary condition 76

77 Mesh, time-step and pulse Various time-step, mesh, and blood-pulse dependence tests help to determine the final parameters for CFD simulations. Mesh dependence test Time step independence Time step 10-3 s Mesh size ~ 1 million cells Blood pulses 2 Final parameters Pulse dependence test 77

78 Meshing Tool used for meshing and CFD runs: Star CCM Cells 1,097,951 Interior faces 6,023,874 Vertices 4,850,151 Cells 1,076,793 Interior faces 6,177,303 Vertices 5,010,556 78

79 Results wall shear stress Axial WSS patterns at point 3 of the cardiac pulse areas of low WSS are localised around the struts and the connectors. In earlier studies low WSS areas are reported to correlate with sites of more intimal thickening 79

80 Flow differences: ART vs Bx-VELOCITY 80

81 Test case 4. Sloshing in a LNG tank (oscillatory free surface flow) CFX

82 Sloshing of LNG 82

83 Sloshing verification & validation 83

84 Test case 5. Rim driven thruster OpenFOAM

85 Mesh verification of open propeller flow 85

86 Validation of open propeller flow Validation Against Experimental Data for the Wageningen B4-70 Propeller Using k-omega SST Turbulence Model 86

87 Validation of rim driven thruster Validation Against Experimental Data for the 70mm Rim Driven Thruster 87

88 Checklist (1) Grid design Geometry (check/fix CAD model) Boundary conditions Boundary layer (Turbulence model) y+ of first layer of grid points how many points in the boundary layer? structured BL or size functions or refinement? Avoid skew cells Local resolution (adaption) Check/improve the grid Check units, scaling, reference values 88

89 Checklist (2) Validation Compare to experimental data Compare with other simulations Grid dependence At least 3 (preferably 4) different grid resolutions Select a sensible range of grids 8 times 8? Time dependence At least 3 significantly different time step sizes Use engineering judgement and a sensible Courant number. 89

90 Checklist (3) Solution scheme Pressure based (segregated) or density based (coupled) solver? Implicit or explicit? At least 2nd order accuracy (in space and time) Set high under-relaxation parameters Monitor residuals, derived variables, point data Flow physics Post-process (Fluent, Fieldview, TecPlot, Ensight) How meaningful? Discuss results using graphical evidence Label all axes and figures 90

91 Checklist (4) Convergence problems Mesh quality (errors) Boundary conditions Under-relaxation First order and then switch to second order Slowness due to problem size Check memory and CPU power Consider running in parallel o speed-up from multiple processors o avoid paging through distributed memory 91

92 Checklist (5) Research the literature Journal and conference papers, reports etc Read the software manuals Casey, M. & Wintergerste, T., 2000, Special Interest Group on Quality and Trust in Industrial CFD, Best Practice Guidelines, Version 1, ERCOFTAC. 92

93 93

94 Resources GoodPracticeCFD_2018.pdf Applications of CFD (FEEG6005) Computational Modelling Group: CFD Online help with ANSYS 94

95 Summary learning outcomes Good Practice in CFD Understand the key steps in setting-up, running and post-processing a CFD simulation. Knowledge about the issues relating to each of these steps. Appreciate the importance of verification (particularly with respect to mesh resolution and the effect this has on results). Understand the significance of the Reynold s number. Knowledge about turbulence model selection and the impact of mesh resolution close to solid boundaries. Appreciation of the critical need to read the CFD manuals (theory and user guides) and other supporting literature. 95

96 And finally! 96