CFD Best Practices and Troubleshooting - with speaker notes
- 1. 1 DAY CFD PRESENTATION Hashan Mendis 1
- 2. 2 AGENDA 1. Introduction to CFD 2. Modelling Process 3. Pre-Processing - Geometry 4. Pre-Processing - Meshing 5. Pre-Processing – Solver Condition 6. Post-Processing 7. Simulation Review 8. Troubleshooting 9. LEAP Academic Portal 2
- 4. 4 INTRODUCTION LEARNING OUTCOMES • Understand ANSYS Computational Fluid Dynamics (CFD) workflow • Understand best practises 4
- 5. 5 CFD is used to predict fluid flow, heat and mass transfer, chemical reactions, and related phenomena. Solves physics equations to characterise fluid flow – Conservation of mass – Conservation of energy – Newton's second Law INTRODUCTION TO CFD PURPOSE OF CFD • Computational Fluid Dynamics is the science of predicting fluid flow, heat and mass transfer, chemical reactions, and related phenomena. • To predict these phenomena, CFD solves equations for conservation of mass, Newton’s second law (F=ma), conservation of energy and additional equations 5
- 6. 6 Provide detailed information : – Distribution of pressure, velocity, temperature, – Forces like lift, drag – Distribution of multiple phases – Species composition Used throughout the engineering process • Conceptual studies of new designs • Detailed product development • Optimization • Troubleshooting • Redesign INTRODUCTION TO CFD PURPOSE OF CFD It can be used to provide detailed information about: Distribution of pressure, velocity, temperature, Forces like Lift, Drag Distribution of multiple phases Species composition And Much more... CFD is used in all stages of the engineering process: Conceptual studies of new designs Detailed product development Optimization Troubleshooting Redesign Its important to keep in mind CFD complements testing and experimentation by reducing effort and cost required for experimentation and data acquisition 6
- 7. 7 Technical Support after training : support@leapaust.com.au INTRODUCTION TO CFD PURPOSE OF CFD 7
- 8. 8 INTRODUCTION TO CFD HOW IT WORKS Control Volume ሶ𝑚𝑖𝑛 ሶ𝑚 𝑜𝑢𝑡 ሶ𝑚 = 𝐴 × 𝑣 × 𝜌 ANSYS CFD solvers are based on the finite volume method Domain is cut up into a finite set of volumes Physics equations are then solved on this set of volumes These equations are then arranged into a system of algebraic equations and then solved 8
- 9. 9 INTRODUCTION TO CFD NAVIER-STOKES EQUATIONS 𝑇𝑟𝑎𝑛𝑠𝑖𝑒𝑛𝑡 + 𝐶𝑜𝑛𝑣𝑒𝑐𝑡𝑖𝑜𝑛 = 𝐷𝑖𝑓𝑓𝑢𝑠𝑖𝑜𝑛 + 𝐺𝑒𝑛𝑒𝑟𝑎𝑡𝑖𝑜𝑛 Variable Description p Continuity u, v, w Momentum in x, y, z k Turbulence production ε Turbulence dissipation h Enthalpy (energy) CFX – Flux value at nodeFLUENT – Flux value at cell In reality instead of just solving your actually solving a set of equations called Navier- stokes Its looks like a complicated but in reality each of those terms can be broken down and simplified for you to understand In this equation we have Transient term capturing the unsteady nature of flow Convection term – captures the bulk fluid motion, ie flow dominated by velocity Diffusion term – capturing viscous flow, ie through diffusion, like buoyant flows, natural convection and the generation or removal of material, ie particles being injected into the domain With this equation you can substitute different variables to capture different flow physics Partial differential equations are discretized into a system of algebraic equations and all algebraic equations are then solved numerically Different solvers can solve the equations in different points of the mesh. As an example fluent is a cell based solver where as CFX is node based, but we wont go too deep into the benefits. Its just important to understand different solver can solve the same equations in different ways. 9
- 11. 11 Problem Identification Pre- Processing Solve Post- Processing Review Results Update Model MODELLING PROCESS For the next few slides I will be going over the modelling process. We will start with problem identification, then preparing the geometry through pre-processing, we would then solve the simulations and post process the results. Its important to keep in mind that cfd is an iterative process, requiring you to go back to previous steps, make changes and re-evaluate your simulation. 11
- 12. 12 Before you starting – Project Timeline – Current Literature – Component Constraints – Manufacturing Constraints – Testing Constraints PROBLEM IDENTIFICATION GOAL IDENTIFICATION Before you start your simulations its important to consider, The project timeline – time allocated for design, manufacturing, testing and refinement The Current Literature – its important to understand what others have done, and how you can improve the design. Component Constraints – understand the whole system, how your sub system slots in and how your part integrates. You should establish goals for your simulation. Manufacturing constraints - How can you manufacture the part And Testing – how are you going to test and validate your simulations. 12
- 13. 13 Create Testing Matrix : Goal maximise downforce created at 15m/s PROBLEM IDENTIFICATION GOAL IDENTIFICATION Case Input Parameter 1 – Inlet Velocity Input Parameter 1 – Angle of Attack of the Front Wing Output Parameter 1 – Downforce Force 1 15 m/s 10 deg 2 15 m/s 15 deg 3 15 m/s 20 deg 4 15 m/s 25 deg 13
- 15. 15 PRE-PROCESSING RELEVANT GEOMETRY Symmetry? Fully Featured? Now identify the geometry that is relevant. What geometry is relevant? Is there existing manufacturing or simulation CAD? Do I have to create my own CAD? If I want to understand the interaction between the front wing, nose and wheels Do I need my whole car? Can I utilize geometry symmetry to reduce computation resources? And also look into removing features around areas that aren’t of interest. 15
- 16. 16 PRE-PROCESSING GEOMETRY REPAIR AND PREPARATION SPLIT EDGES EXTRA EDGES MISSING FACES SMALL FACES After identifying your geometry it is advised to repair and prepare it for simulation. We can remove unnecessary features, edges and then create a watertight body to create our enclosure. There is a repair tab within SpaceClaim that allows you Fill in missing faces, which can happen if the model is saved as an intermediately file format. Remove Small faces – cleaning these faces will result in a reduced mesh count and better quality which reduces computational resources and helps convergence Split edges – which merges edges that don’t make a boundary Extra edge – removing unnecessary edges 16
- 17. 17 PRE-PROCESSING GEOMETRY REPAIR AND PREPARATION INTERFERENCE SMALL EDGES ROUNDS FACES Within the prepare tab you can Removing fillets Resolving interference Remove faces And remove short edges Short edges are really import to resolve in order to reduced mesh count, increase quality which helps convergence 17
- 18. 18 PRE-PROCESSING FLUID DOMAIN The domain can then be created using the enclosure function in SpaceClaim. This will create the fluid domain and Boolean out the solid bodies. 18
- 19. 19 PRE-PROCESSING FLUID DOMAIN L 3L L Dimensionless Length – L (Length of the car) Inlet - L Height – L Width - L Outlet - 3L When it comes to creating the domain, around the geometry, its important to place your boundary away from your car. This ensures the flow around the car is not effected by the wall. Make sure the inlet profile, isn’t effected by the stagnation region, your capturing the shape of your wake and the outlet is placed away from any recirculation regions. For reference the inlet, width and height is one car width in front, outlet 3 The outlet is far enough behind to resolve the wake, this also makes convergence easier 19
- 20. 20 PRE-PROCESSING FLUID DOMAIN The wheel was cut off by 5 mm. this results I a sharp angle so it was filleted, this will increase the mesh quality around that area 20
- 21. 21 PRE-PROCESSING FLUID DOMAIN We will need to refine around areas of interest, so extra boxes were added to be used as bodies of influence later on. There is one to pick up the front wing and wheel wake 21
- 22. 22 • Understand your time, manufacturing and testing constraints before starting CFD • Identify geometry needed to achieve your simulation goal • Make simplifications to the model if possible • Use the repair and prepare functions • Clean geometry, clean mesh, clean convergence PRE-PROCESSING GEOMETRY - KEY POINTS 22
- 23. 23 Use the repair and prepare functions • Remove sharp feature • Reduce number of fillets if possible • Remove small gaps, small faces and small edges • Defeature where possible • Make changes to the initial CAD • Add bodies of influence for meshing • Make sure the domain doesn’t effect the flow field PRE-PROCESSING GEOMETRY - KEY POINTS 23
- 24. 24 1. Core Skills 2. Creating Geometry 3. Repairing Geometry 4. FEA and CFD Modelling 1. Pick up the CFD tutorials RECOMMENDED TUTORIALS 24
- 26. 26 Mesh Strategy Accuracy Efficiency Ease of Generation PRE-PROCESSING MESH GOALS Choosing your mesh strategy depends on Accuracy - mesh quality to achieve convergence Efficiency in cell count, and element type, to ensure the flow pattern has been captured, at low computational cost And easiness of generate – time taken to generate the mesh The goal is to find the best compromise between accuracy, efficiency and easiness to generate 26
- 27. 27 PRE-PROCESSING MESHING ELEMENTS • In ANSYS there are 2 meshing tools, ANSYS meshing and Fluent meshing. For simple geometry and in order to learn we will use ANSYS meshing, but with larger and complicated geometry you should use Fluent Meshing. • When it comes to generating a mesh, we start with a course mesh, refine around areas of interest like the wake region and import pressure gradients. • Using fluent meshing there are different element types that can be created each with their own benefits, with prism layer used to capture the boundary layer 27
- 28. 28 PRE-PROCESSING MESHING ELEMENTS • Tetrahedral grids provide high resolution of complex geometry but can take longer to solve • Polyhedral elements have a lower cell count compared to a tet grid, by 3-5 times, this will reduce CPU resources with the expense of more RAM needed. • Due to the larger size a finer sizing may be needed though • Hex core uses tets on the surface and then are hex elements around the volume mesh. Hex elements are more efficient so its computationally more efficient than straight-tets • In the latest version of ANSYS 19.2, we can also generate poly hexcore grids with poly elements on the surface with hexcore in the volume. • So you probably asking yourself whats type should you use? There isn’t an easy answer because it depends on the physics your using and computational requirements. We recommend a mesh study which we will talk about in the future 28
- 29. 29 Poly-Hexcore Hexcore Polyhedral Tetahedral Time (hr) 0.52 0.62 0.69 1.64 0.00 0.20 0.40 0.60 0.80 1.00 1.20 1.40 1.60 1.80 Time(hr) Case vs Time Poly-Hexcore Hexcore Polyhedral Tetahedral RAM 8.6 10.7 12.8 25.5 0.0 5.0 10.0 15.0 20.0 25.0 30.0 RAM(GB) Case vs RAM Poly-Hexcore Hexcore Polyhedral Tetahedral Elements (x 1e6) 1.3 2.4 1.4 7 0 1 2 3 4 5 6 7 8 Elements(x1e6) Case vs Elements This is an example, you should tested out different mesh elements types on your model. Model had the same sizing function and geometry. Computer used: I7 – 7920HQ 32 GB RAM Windows 10 Here is an example of a test I ran showing the different in element count, RAM and Time for each element type. These results are case dependent, so its important to test on your model and reference up to date research 29
- 30. 30 MESH QUALITY Orthogonal Quality mesh metrics spectrum • It important to check the quality of the mesh. • If the quality is low, you can encounter issues with convergence and inaccurate results. • Using the meshing tools there are ways to improve the surface and volume mesh by identifying poor quality cells. • The orthogonal quality is a range of orthogonal quality is 0-1, where a value of 0 is worst and a value of 1 is best. • The orthogonal quality for cells is computed using the face normal vector, for each face; the vector from the cell centroid to the centroid of the adjacent cells, and the vector from the cell centroid to each of the faces 30
- 31. 31 PRE-PROCESSING MESHING QUALITY In ANSYS meshing we can analyse the mesh and pull out important data points 31
- 32. 32 PRE-PROCESSING MESHING QUALITY We can chart the elements and highlight areas of low quality. With this information you can improve the quality if they are around areas of interest. 32
- 33. 33 PRE-PROCESSING MESHING QUALITY EXAMPLE Good Bad We can chart the elements and highlight areas of low quality. With this information you can improve the quality if they are around areas of interest. 33
- 34. 34 PRE-PROCESSING MESHING QUALITY EXAMPLE Mesh Quality at a sharp edge Mesh Quality at a flat face with 1 element across the thickness At a sharp edge the quality close to the wall is low With 1 element the prims around the face has poor quality 34
- 35. 35 PRE-PROCESSING MESHING QUALITY EXAMPLE Mesh Quality at a flat face with 3 element across the thickness Mesh Quality at a flat face with 6 element across the thickness 3 elements has a better quality 6 elements has an equivalent quality, inflation region is more uniform as well 35
- 36. 36 PRE-PROCESSING MESHING QUALITY EXAMPLE Mesh Quality at a flat face with 3 element across the thickness Mesh Quality at a flat face with 6 element across the thickness 3 elements has a better quality 6 elements has an equivalent quality, inflation region is more uniform as well 36
- 37. 37 PRE-PROCESSING MESHING QUALITY EXAMPLE Mesh Quality with a radius, 6 element around the radius Mesh Quality with a radius, 9 element around the radius 6 elements around has good quality but it defeatures the radius, 9 elements resolves the radius, more elements than a flat edge 37
- 38. 38 Turbulent boundary layer consists of distinct regions – viscous sublayer – log-layer – Outer-layer PRE-PROCESSING MESHING BOUNDARY LAYERS viscous A turbulent boundary layer consists of distinct regions A laminar - viscous sublayer next to the wall, this then transitions into the fully turbulent – log layer, outer layer and then free stream Resolving closer to the wall accurately predicts skin friction drag and adverse pressure gradients which induced separation. Adverse pressure gradients are important on a race car as they characterise flow around the wings and diffuser. 38
- 39. 39 PRE-PROCESSING MESHING BOUNDARY LAYERS Boundary layer u y Viscous sublayer unresolved u y Viscous sublayer resolved So if we were to resolve the laminar layer, we would need to ensure our first cell height is small, with enough prism layers to capture the boundary layer, as is the example on the left. Where as the example on the right has large first cell height. As you need more elements in the first case it will have more elements than the right increasing computational resources. Now in order to estimate the first cell height we will use a dimensionless value called y plus. It’s a equation proportional to the flow velocity, density and shear stress at the wall. 39
- 40. 40 PRE-PROCESSING MESHING INDEPENDENCE STUDIES MonitorPoint # of Elements A mesh study should also be performed. When meshing, a coarse mesh may be quick, but unable to capture the flow characteristics, a fine mesh may be accurate but encompass high computational resources. A mesh study is performed by refining the surface and domain mesh until the deviation between monitor points stabilise. 40
- 41. 41 PRE-PROCESSING MESHING INDEPENDENCE STUDIES GRID NUSSELT NUMBER ERROR 1st order 2nd order 1st order 2nd order 50 50 190.175 176.981 22.1 % 13.6 % 100 100 170.230 163.793 9.3 % 5.1 % 200 200 162.664 159.761 4.4 % 2.6 % 400 400 159.646 158.296 2.3 % 1.4 % 800 800 157.808 157.168 1.1% 0.7 % 155.751 155.777 41
- 42. 42 PRE-PROCESSING EXAMPLE MESH Name Selection Sizing BOI - Near 10 mm BOI - Far 50 mm Curvature Sizing – Front Wing Min – 1 mm Max – 10 mm Proximity Sizing – Front Wing 3 elements across gap Scoped Prism - Front Wing First Cell Height – 0.02 mm Number of Layers – 18 Last Percent Ratio – 20% Curvature Sizing – Rod Min – 4 mm Max – 10 mm Curvature Sizing – Wheel Min – 15 mm Max – 20 mm Curvature Sizing – Chassis Min – 10 mm Max – 20 mm 42
- 50. 50 • Identify the correct mesh type to use depending on simulation goal and computational resources • Identify boundary layer resolution for simulation goal • DO A MESH STUDY! How to perform a mesh study • 80% OF MY SUPPORT CALLS WOULDN’T EXIST IF SOMEONE CHECKED THEIR MESH AND DID A MESH STUDY. CHECK YOUR MESH AND DO A MESH STUDY FOR MY SAKE!! • Clean mesh, clean convergence PRE-PROCESSING MESHING KEY POINTS 50
- 51. 51 • Make sure surface mesh quality is > 0.6 orthogonal quality • Make sure volume mesh quality is > 0.95 orthogonal quality • Keep in mind, the majority of the mesh is close the surface. If you need to reduce element count, start with the surface mesh and inflation elements. • Ensure there are 3-4 elements across small features to maintain quality • Double check surface with high curvature to ensure they are resolved • Use bodies of influence to reduce element count • Make sure flow features of interest are captured PRE-PROCESSING MESHING KEY POINTS 51
- 52. 52 PRE-PROCESSING EXAMPLE MESH REFINEMENT TEST Case Input Parameter 1 – BOI – Near Output Parameter 1 – Cl % Error to Successive Case 1 20 mm Cl(1) 2 15 mm Cl(2) (Cl(n+1)- Cl(n))/(Cl(n+1) 3 10 mm Cl(3) … 4 5 mm Cl(4) … Example mesh study to understand how fine the BOI – Near needs to be in order to capture vortex structure. Measure Cl until the difference between the successive cases are within your margin of error 52
- 53. 53 • Basic Workflow • Surface Mesh Preparation • Wrapping a Dirty Geometry • Volume Fill Methods RECOMMENDED TUTORIALS 53
- 55. 55 SOLVER CONDITIONS Setting Up Physics •Solver •Models •Zones Solving •Solutions •Controls •Reports 55
- 56. 56 SOLVING SOLVER No Set the solution parameters Initialize the solution Enable the solution monitors of interest Modify solution parameters or grid Calculate a solution Check for convergence Check for accuracy Stop Yes Yes No As CFD is an iterative solver. It initializes a solution with a velocity field, solves the navier stokes equations checking against convergence criteria, when it achieves its result it and returns the result for analysis. 56
- 57. 57 SOLVER CONDITIONS SOLVER Type • Pressure-Based is the default and should be used for most problems • Handles the range of Mach numbers from 0 to ~2-3 • Density-Based is normally only used for higher Mach numbers, or for specialized cases such as capturing interacting shock waves 57
- 58. 58 Segregated Coupled Implicit Solve Continuity; Update Velocity Solve U-Momentum Solve V-Momentum Solve W-Momentum Coupled Solve Turbulence Equation(s) Solve Species Solve Energy Solve Other Transport Equations as required Solve Mass & Momentum Solve Mass, Momentum, Energy, Species Coupled-Explicit Solve Mass, Momentum, Energy, Species Pressure-Based Density-Based 58
- 59. 59 SOLVER CONDITIONS MODELS Commonly used models include • Energy (heat transfer) • Radiation • Viscous (turbulence) • Multiphase • Species and combustion • Discrete Phase 59
- 60. 60 PRE-PROCESSING TURBULENCE MODELLING Laminar (Low Reynolds Number) Transitional (Increasing Reynolds Number) Turbulent (Higher Reynolds Number) . . ReL U L = The Reynolds number is the criterion used to determine whether the flow is laminar or turbulent Transition to turbulence varies depending on the type of flow: External flow along a surface : ReX > 500 000 around on obstacle : ReL > 20 000 Internal flow : ReD > 2 300
- 61. 61 PRE-PROCESSING TURBULENCE MODELLING Small structures Large structures This is an example of turbulent flow. You can see small and large turbulent structures being created and dissipated. A Turbulent flow can have : Unsteady and irregular structure Unpredictability in detail Turbulent flows contain a wide range of eddy sizes that can be resolved
- 62. 62 DNS (Direct Numerical Simulation) LES (Large Eddy Simulation) RANS (Reynolds Averaged Navier-Stokes Simulation) PRE-PROCESSING TURBULENCE MODELLING Three basic approaches can be used to calculate a turbulent flow DNS-Numerically solving the full unsteady Navier-Stokes equations Resolves the whole spectrum of scales High computational demand LES-The large eddies are fully resolved with the small eddies modelled Less expensive than DNS, but the efforts and computational resources needed are still too large for most practical applications RANS-Solve time-averaged N-S equations Many different models are available This is the most widely used approach for industrial flows
- 63. 63 PRE-PROCESSING RANS TURBULENCE MODELS One-Equation Model Spalart-Allmaras Two-Equation Models k–ε family (Standard, RNG, Realizable) k–ω family (Standard, BSL, SST) Reynolds Stress Model Transition Models k–kl–ω, Transition SST and Intermittency Models There are different RANS models used for different applications. They can be classed by how many equations are added to the NS equations with computational resources increases down the page. These include the Spalart-Allmaras model, the k-epsilon family of models and the k- omega family of models. There are also more advanced models such as the Reynolds Stress and transition models with computational resources increasing down the table
- 64. 64 PRE-PROCESSING TURBULENT BOUNDARY LAYER PROFILE
- 65. 65 PRE-PROCESSING TURBULENT BOUNDARY LAYER PROFILE
- 66. 66 PRE-PROCESSING TURBULENT BOUNDARY LAYER PROFILE
- 67. 67 PRE-PROCESSING MESHING BOUNDARY LAYERS Boundary layer u y Viscous sublayer unresolved u y Viscous sublayer resolved So if we were to resolve the laminar layer, we would need to ensure our first cell height is small, with enough prism layers to capture the boundary layer, as is the example on the left. Where as the example on the right has large first cell height. As you need more elements in the first case it will have more elements than the right increasing computational resources. Need to capture because of Boundary layers Heat transfer Wakes, shock Flow gradients 67
- 68. 68 68 “Bad” “Good” PRE-PROCESSING VELOCITY PROFILES AT AIRFOIL
- 69. 69 Turbulent flow past a blunt flat plate was simulated using four different turbulence models. 8,700 cell quad mesh, graded near leading edge and reattachment location. Non-equilibrium boundary layer treatment N. Djilali and I. S. Gartshore (1991), “Turbulent Flow Around a Bluff Rectangular Plate, Part I: Experimental Investigation,” JFE, Vol. 113, pp. 51–59. D 000,50Re =D Rx Recirculation zone Reattachment point 0U PRE-PROCESSING TURBULENT FLOW PAST A BLUNT FLAT PLATE Expect enhanced heat transfer at separation bubble reattachment (impingement flow).
- 70. 70 RNG k–εStandard k–ε Reynolds StressRealizable k–ε Contours of Turbulent Kinetic Energy (m2/s2) 0.00 0.07 0.14 0.21 0.28 0.35 0.42 0.49 0.56 0.63 0.70 The standard k-e model greatly overpredicts the production of turbulence at stagnation points, which can lead to qualitatively inaccurate predictions, as seen on the next slide. PRE-PROCESSING TURBULENT FLOW PAST A BLUNT FLAT PLATE 70
- 71. 71 Experimentally observed reattachment point is at x / D = 4.7 Predicted separation bubble: Standard k–ε (SKE) Skin Friction Coefficient Cf × 1000 SKE severely underpredicts the size of the separation bubble, while RKE predicts the size exactly. Realizable k–ε (RKE) Distance Along Plate, x / D PRE-PROCESSING TURBULENT FLOW PAST A BLUNT FLAT PLATE Ske is compared with rke and rng in skin friction figure. Note the peak cf at the leading edge for the ske and the considerably smaller re-circulation region (where cf returns to zero around x/d=2 under ske (experiment is 4.7). Rke appears to be slightly better at predicting this flow than rng.
- 72. 72 • K-w SST, RKE with Enhanced Wall Function recommended for FSAE with Curvature Correction • Able to accurately resolution in the boundary layer PRE-PROCESSING TURBULENCE MODELLING For fsae its recommended to use the k-w sst model. Out of the box this can be used to accurately predict the boundary layer and hence separation. 72
- 74. 74 PRE-PROCESSING ZONES External Boundaries Any flow Pressure Inlet Pressure Outlet Incompressible flow Velocity Inlet Compressible flow Mass Flow Inlet (can also use for incompressible) Pressure Far Field Other Wall Symmetry Axis Periodic Special flow boundaries Inlet / Outlet Vent Intake / Exhaust Fan Internal Boundaries Fan Interior Porous Jump Radiator Wall orifice outlet inlet plate plate-shadow wall There are many different boundary conditions for different simulations. Poorly defined boundary conditions can have a significant impact on your solution Most Robust: Velocity at inlet with static pressure at outlet (Velocity Inlet : Pressure Outlet) 74
- 75. 75 SOLVER CONDITIONS ZONES Make sure static pressure at the nose doesn’t effect inlet profile, and outlet isn’t in the recirculation region Make sure b/c are in the correct place to capture all flow features If flow features aren’t fully developed it will also effect monitor points 75
- 76. 76 PRE-PROCESSING BOUNDARY CONDITIONS Named Selection Boundary Condition All Car Faces No-Slip Wall Ground and Boundary Walls Moving Wall at 11 m/s Inlet 11 m/s Outlet 0 Gauge Pressure Average Pressure Specification Symmetry Symmetry Condition Wheel Rotating Wall Speed – 55 rad (w=v/r) Axis Origin Rotation Axis - + x We would make use of symmetry plan being able to half our model. No-slip walls around the car, where a b/l will be created and slip walls around the far boundaries were we aren’t concerned. We can also use porosity to model the radiator. 76
- 78. 78 Segregated Solve Continuity; Update Velocity Solve U-Momentum Solve V-Momentum Solve W-Momentum Coupled Solve Turbulence Equation(s) Solve Species Solve Energy Solve Other Transport Equations as required Solve Mass & Momentum Pressure-Based SOLVER CONDITIONS SOLUTION For our simulations its advised to use the pressure based solver with a coupled solver. For compressible flow the coupled solver can be used. Instead of solving the variables separately and then correcting they are solved simultaneously leading to faster convergence with the compromise of require more memory. 78
- 79. 79 Coupled: ~120 iterationsSIMPLE: ~2250 iterationsRotating propeller 1500 rpm Pressure based coupled solver with default settings Approximately 2250 iterations of SIMPLE (default) in 3.5 hours Approximately 120 iterations of coupled 13 minutes SOLVER CONDITIONS SOLUTION Basic example showing how the solution can be spead up using a coupled solver
- 80. 80 SOLVER CONDITIONS SOLUTION First-order upwind scheme example ii -1i -2 Time = n 𝑢𝑖 𝑛𝑢𝑖−1 𝑛 𝑢𝑖−2 𝑛 Second-order upwind scheme example 1-D Mesh example Use of the default settings for spatial discretization is recommended for most cases They are a way of calculating physics terms. If we take velocity as an example. In the first example we have a first order scheme. In order to determined velocity in a cell, its use the cell to the right and averaging it. A second order scheme will take the last 2 velocity elements. As the order increases more elements are taken into account, this increases accuracy at the cost of computational resources.
- 81. 81 SOLVER CONDITIONS SOLUTION 1st-Order Scheme Flow is misaligned with mesh Theory 0 1 2nd-Order Scheme Example on the screen, more diffusion when first order and for is unaligned with mesh.
- 82. 82 SOLVER CONDITIONS CONTROLS Courant Number Within the solver an artificial time step called the Courant number is used to calculate the averaged flow characteristic. The default is 200 and can be reduced to 10-50 for problems that are difficult to converge. In general, lower Courant number values make the solution more stable, while higher values allow the solution to converge faster. 82
- 83. 83 SOLVER CONDITIONS CONTROLS Control Volume Time-average of velocity Velocity Instantaneous velocity Time In order to understand what the timestep value is doing lets take this example Lets take our volume from our pipe. If were to give it an inlet velocity we can expect real velocity to be fluctuating with time. By trying to solve steady state we are looking for the time averaged velocity. The timestamping value allows us to take enough data points to calculate the averaged velocity. 83
- 85. 85 SOLVER CONDITIONS REPORTS The solver must perform enough iterations to achieve a converged solution, at convergence, the following should be satisfied: • All discrete conservation equations are obeyed in all cells to a specified tolerance (Residual). • The residual measures the imbalance of the current numerical solution and is related to but NOT EQUAL to the numerical error. • Overall mass, momentum, energy, and scalar balances are achieved • Target quantities reach constant values • Integral: e.g. Pressure drop • Local: e.g. Velocity at specified position 85
- 86. 86 SOLVER CONDITIONS REPORTS Monitoring convergence using residual history • Generally, a decrease in residuals by three orders of magnitude can be a sign of convergence • Scaled energy residual should decrease to 10−6 (for the pressure-based solver) • Scaled species residual may need to decrease to 10−5 to achieve species balance Best practice is to also monitor quantitative variables to decide convergence • Ensure that overall mass/heat/species conservation is satisfied • Monitor other relevant key variables/physical quantities for confirmation • Report Definitions are used for this purpose • It is strongly recommended to use one or more report definitions for all simulations 86
- 87. 87 SOLVER CONDITIONS CALCULATION Initial mesh before solving Standard Initialization: All cells have the same value Hybrid Initialization: Slightly more realistic non-uniform initial guess FMG Initialization: Much more realistic non-uniform initial guess, however takes longer to generate Final converged solution 87
- 88. 88 • What turbulence model is appropriate for my case? What does the literature say? What has been tested before? – General recommendation – 𝑘 − 𝜔 SST or Realizable 𝑘 − 𝜀 with the Enhanced Wall Function • Am I capturing my boundary layer? Check the Turbulence Viscosity Ratio • Are my boundary conditions correct? Do they need to be calibrated? • Which scheme should I be using? A SIMPLE or Coupled Scheme? If your not sure check the ANSYS Help. – General recommendation – Coupled solver • What Spatial Discretisation Scheme do I need? First order or second order? If your not sure test it. – General recommendation – 2nd order terms may be more accurate, but may be unstable depending on the mesh • Make sure your ALWAYS using solution monitor points around areas of interest. Have the monitor points stabilised? SOLVING CONDITION KEY POINTS 88
- 89. 89 • Mixing Elbow • Solving • Airfoil • Backward Facing Step • Using the Discrete Phase Model • Multispecies Flow • Multiphase Flow • Vortex Shedding RECOMMENDED TUTORIALS 89
- 91. 91 There are several different factors that combine to affect the overall solution accuracy. In order of magnitude: – Round-off errors • Computer is working to a certain numerical precision – Iteration errors • Difference between ‘converged’ solution and solution at iteration ‘n’ – Solution errors • Difference between converged solution on current grid and ‘exact’ solution of model equations • ‘Exact’ solution → Solution on infinitely fine grid – Model errors • Difference between ‘exact’ solution of model equations and reality (data or analytic solution) – Systematic Error SOURCES OF ERROR DIFFERENT SOURCES OF ERROR 91
- 92. 92 SOURCES OF ERROR ROUND OFF ERROR 92
- 93. 93 SOURCES OF ERROR ITERATION ERROR 93
- 94. 94 SOURCES OF ERROR ITERATION ERROR EXAMPLE: 2D COMPRESSOR CASCADE 94
- 95. 95 SOURCES OF ERROR DISCRETIZATION ERROR All discrete methods have solution errors: Finite volume methods Finite element methods Finite difference methods ... The difference between the solution on a given grid and “exact” solution on an infinitely fine grid is called “discretization error” Exact solution not available → Discretization error estimation 95
- 96. 96 SOURCES OF ERROR DISCRETIZATION ERROR ESTIMATION 96
- 97. 97 SOURCES OF ERROR DISCRETIZATION ERROR ESTIMATION 97
- 98. 98 SOURCES OF ERROR MODEL ERRORS Inadequacies of (empirical) mathematical models: – Base equations (Euler vs. RANS, steady-state vs. unsteady-state, …) – Turbulence models – Combustion models – Multiphase flow models – … Due to model errors, discrepancies between data and calculations can remain, even after all numerical errors have become insignificant! 98
- 99. 99 SOURCES OF ERROR MODEL ERROR: IMPINGING JET 99
- 100. 100 SOURCES OF ERROR SYSTEMATIC ERRORS 100
- 102. 102 POST-PROCESSING RESULTS Then after the simulation has been finished you will be checking out the results. Personally I would recommend plotting contours of static pressure and then a total pressure sweep to understand the flow structure. 102
- 104. 104 Cut planes showing mesh 104
- 105. 105 POST-PROCESSING RESULTS Overlaying mesh and contour 105
- 106. 106 Total Pressure Sweep Video – Click Me Creating animations 106
- 108. 108 Question that is sometimes asked – how does case comparison work when geometry is not the same. A - Difference variables are computed as the values from case 1 minus values from case 2. Case 2 variables are interpolated onto the case 1 mesh before the subtraction, thus difference variables are located on the mesh from case1 z
- 109. 109 Creating isosurfaces or vortex cores
- 111. 111 ESULTS Plots Reports Xy plots can be created an exported to compare to experiments Reports created showing contour plots and numerical values to document the simulations
- 112. 112 • What are my output parameters? • Can I use quantitative and qualitative methods? • What reports do I need? • What contour/vectors/streamlines are need? • Can I make animations? • Double check your assumptions? • Check resolution of the wake and boundary. POST PROCESSING KEY POINTS 112
- 114. 119 Are the physical models appropriate? – Is the flow turbulent? – Is the flow unsteady? – Are there compressibility effects? – Are there 3D effects? Are the boundary conditions correct? – Is the computational domain large enough? – Are boundary conditions appropriate? – Are boundary values reasonable? Is the mesh adequate? – Can the mesh be refined to improve results? – Does the solution change significantly with a refined mesh, or is the solution mesh independent? – Does the mesh resolution of the geometry need to be improved? SIMULATION REVIEW 119
- 115. 120 CFD is an iterative process 1. Create Testing Matrix of input and output parameters 2. Build domain 3. Create simplified mesh 4. Set up boundary conditions and post processing 5. Refine mesh 6. Design iterations 7. Physical testing 8. Validate design or check modelling assumptions, mesh and boundary conditions SIMULATION REVIEW 120
- 117. 122 Typically used for finding optimal shape for given operating conditions Derive optimal shape from initial calculation ADJOINT SOLVER 122
- 118. 123 • Adjoint solver tutorials RECOMMENDED TUTORIALS 123
- 119. 124 Refine the mesh after a solution has been run depending on the results MESH ADAPTION Initial Mesh Refined Mesh 124
- 120. 125 Wrap dirty geometry that may not be capped, more info here SURFACE WRAPPING STL file given Able to create high quality cells 125
- 121. 126 • Wrapping Dirty Geometry RECOMMENDED TUTORIALS 126
- 122. 127 Create a script that can automate the meshing and solving process. JOURNALING Tutorial series about how to create a script : Intro to scripting ANSYS Fluent Meshing and Fluent Solver 127
- 123. 128 Able to overlay different meshes on top of each other, Link to video OVERSET MESHING 128
- 124. 129 Able to change the mesh as geometry changes, Link to video DYNAMIC MESHING 129
- 125. 130 • Dynamic Meshing Tutorials RECOMMENDED TUTORIALS 130
- 128. 133 • The ANSYS Help guide has access to User Guides, Theory Guides and best practises. More information here: User Guides • Boundary condition Help – Fluent User Guide > Solution Mode > Cell Zone and Boundary Conditions > Boundary Condition > Different boundary condition information • Turbulence Help – Fluent User Guide > Solution Mode > Modelling Turbulence – Fluent User Guide > Solution Mode > Modelling Turbulence > Setting Up the k-e model – Fluent User Guide > Solution Mode > Modelling Turbulence > Setting Up the k-w model – Fluent User Guide > Solution Mode > Modelling Turbulence > Setup Options for All Turbulence Modelling TROUBLESHOOTING ANSYS HELP 133
- 129. 134 Solver Help – Fluent User Guide > Solution Mode > Using the Solver – Fluent User Guide > Solution Mode > Using the Solver > Choosing the Spatial Discretization Scheme – Fluent User Guide > Solution Mode > Using the Solver > Choosing the Spatial Discretization Scheme > First Order Accuracy vs Second Order Accuracy – Fluent User Guide > Solution Mode > Using the Solver > Pressure Based Solver Settings – Fluent User Guide > Solution Mode > Using the Solver > Full Multigrid Initialization (FMG) – Fluent User Guide > Solution Mode > Using the Solver > Performing Pseudo-Transient Calculation TROUBLESHOOTING ANSYS HELP 134
- 130. 135 Adaption Help – Fluent User Guide > Solution Mode > Adapting the Mesh Adjoint Help – Fluent User Guide > Solution Mode > Design Analysis and Optimisation > The Adjoint Solver TROUBLESHOOTING ANSYS HELP 135
- 131. 136 • Solve on a local drive, network drives solve slower • Make sure there is enough space on your hard disk to solve on • Make sure your don’t have special characters in your file name or file location • Features that kill meshing and can contribute to convergence issues: - small face, thin slivers, sharp angles • Check and double check mesh quality – you can create iso-surfaces of bad mesh elements in post • Triple check of boundary conditions, scale and units! • There is no one size fits all turbulence model, different models work for different cases. • Start simple, add complexity - Reducing the number of variables that could go wrong will help isolate problems with your model • In the real world, computational resources and time are your biggest constraints. • Check out basic training before stating your simulation. - I know it's boring, I hate it too. I want my simulation finished yesterday with no errors or effort. But there is a learning curve, be patient. TROUBLESHOOTING FAQ 136
- 132. 137 • Reduce your Courant Number, untill you hit 5. if that doesn’t work activate Pseudo-transient time step • Don’t rely on residuals, always monitor areas of interest • If 2nd order schemes aren’t converging, try first order. If you can’t converge first order there is something else going wrong • A finer mesh may pick up transient features and cause issues with convergence • Have a clear testing plan • Know what to expect from CFD. Before attempting complicated 3D simulations make sure you do your research and have numbers locked down from 1-D or 2-D fundamentals • Always try to validate your CFD data with reality, compare with wind tunnel data, testing data or peer reviewed research papers TROUBLESHOOTING FAQ 137
- 134. 139 ANSYS Student Community Portal • Pre and Post Processing • Physics Simulation • Tutorials, Articles and Textbooks • Student Competition Teams – ANSYS Formula SAE/BAJA SAE Tutorials ANSYS STUDENT COMMUNITY 139
- 135. 140 LEAP CFD Blog : Top posts – Turbulence Part 1 - Introduction to Turbulence Modelling – Turbulence Part 2 - Wall Functions and Y+ requirements – Turbulence Part 3 - Selection of wall functions and Y+ to best capture the Turbulent Boundary Layer – Turbulence Part 4 - Reviewing how well you have resolved the Boundary Layer – Estimating the First Cell Height for correct Y+ – Shape Optimisation without constraints - How to use the Adjoint Solver Part 1 – Convergence and Mesh Independence Study – How to Shrink Wrap a biomedical STL file in Fluent Meshing ADDITIONAL RESOURCES 140
- 136. 141 LEAP YouTube : Top Playlists – Introduction to HFSS Playlist – Information about the Internet of Things – Introduction to CFD for FSAE Teams – Introduction to Composites for FSAE Teams – Introduction to FEA for FSAE Teams – Information about Augmented Reality – Information about Discovery Live ADDITIONAL RESOURCES 141
- 138. 144 1200 students on the LEAP Academic Portal With access to the free student download 144
- 139. 145 Learn about how ANSYS can be used for your application 145
- 140. 146 Additional short courses to get you started 146
- 141. 147 Academic Portal Website 1. Create a Portal Account 2. ANSYS Student Download • Geometry Pre-processing using SpaceClaim • Introduction to FEA Course • Introduction to CFD Course • Introduction to Composites Need more technical help? support@leapaust.com.au LEAP ACADEMIC PORTAL 147
- 142. 148 Follow LEAP on social media for more videos, tips & tutorials on @LEAPAust@LEAP Australia @LEAP_Australia @leap_australia STAY CONNECTED TO LEAP CLICK ON THE ICONS BELOW LEAP Australia 148