Best Practices for Aerospace Aerodynamics. Peter Ewing
|
|
- Claude Berry
- 5 years ago
- Views:
Transcription
1 Best Practices for Aerospace Aerodynamics Peter Ewing
2 Agenda Pre-processing Geometry Origin/Import Geometry Prep Surface Mesh Volume Mesh Solver Settings Defining Flight Physics Setting Up Solvers Post-processing Automated Data Extraction Plotting Scenes Automated Reporting
3 Agenda Pre-processing Geometry Origin/Import
4 STAR-CCM+ Parts Geometries ultimately conglomerate in Parts Laser scans, extracted mesh topology External CAD modelers, e.g. CATIA, NX STAR-CCM+ 3D-CAD Mesh Operation Parts Common Denominator: tessellated surfaces STL or surface meshes dummy or flattened surface meshes Discrete Mesh Operations Detached mesh operations are green 3D-CAD/CAD Parts Analytic representation, blue or solid grey User should be aware of geometry quality Especially for flattened Parts! STAR-CCM+ requires clean, closed geometry: To use Boolean operations To generate a volume mesh Import Prep Surface Volume
5 CAD is Preferred Aero surfaces & leading edges are complex swept geometries These features matter! Hierarchy of geometry fidelity : STAR-CCM+ 3D-CAD CAD-Clients CAD Exchange X_B /X_T then STP/STEP DBS, STL, IGES Direct Link SolidWorks Parameter Transfer CAD geometry allows several benefits over flattened parts Project to CAD CAD-based Mesh Operations Feature aligned meshing Parametric design changes 3D-CAD and CAD-Clients Persistent Part naming STAR-CCM+ Bi-directional link Import Prep Surface Volume
6 Agenda Pre-processing Geometry Origin/Import Geometry Prep
7 External Aerodynamics Geometry Preparation Split the body into multiple Part Surfaces: Inflow/Outflow/Freestream definitions Allows tracking of physical convergence Trailing Edge for custom controls Rounded edges DPW4 Geometry (upper) Naming conventions enable filtering and efficient identification, e.g.: 00 Inlet, 00 Outlet, 00 Freestream, etc. 01 Wing, 01 Body, 01 Tail, etc. 02 Symmetry Plane 3D RAE2822 Airfoil for 2D simulation 03 Interface (Sliding or Overset) DPW4 Geometry (lower) Filter selection box Import Prep Surface Volume
8 Low-Speed Far-field Boundary Preparation Velocity Inlet Atmospheric flight: Upstream boundary: Typically velocity inlet in a round/bullet shape Distance is characteristic lengths Outflow boundary: Typically a outflow flat plane cut Distance is characteristic lengths Pressure Outflow Example bullet domain Wind tunnel configurations should be matched: Duplicate the geometry Inlet distances typically set as free stream * Outlet distance should follow free stream distance Side walls typically set to symmetry * * If inlet conditions are well measured, duplicate Import Prep Surface Volume
9 Transonic Far-field Boundary Preparation Freestream settings: Circular domain will use Freestream boundary condition Upstream position characteristic length scales Downstream position characteristic length scales Freestream Boundary Body Sample transonic circular domain Wind tunnel sections can be difficult to reproduce Transonic wind tunnels typically have slatted configurations Simulations may contain shock reflections to disrupt upstream flow Unless specific configuration is well documented, run in Freestream Import Prep Surface Volume
10 Supersonic and Hypersonic Far-field Boundary Preparation Upstream placed fairly close and aligned with shocks generated by the body The shock should not interact with the freestream boundary Outlet boundaries can either be Pressure Outlet or Freestream Hypersonic cases Outlet can be set to Pressure field function to extrapolate Pressure Outlet Freestream Axis or Symmetry Body Example of hypersonic domain for Mach 12 sphere Import Prep Surface Volume
11 Wrapping What does it do? Enables fast turn-around of broken geometry Standard use case is for unification of assemblies of broken (i.e. not clean and closed) Parts How do I know if I should wrap? Inefficient control over the CAD or Parts are flattened Extensive* Surface Repair work is required: Inefficient (or no) control of CAD workflow Many CAD based-errors (e.g. too many pieces) to fix efficiently in CAD Too many tessellation errors to efficiently fix in Surface Repair Simulation fidelity is independent of intricate details affected by Wrapper Features worth investigating: Works well in the PBM structure Maintains Part Surface naming convention Operation can be Detached to create new Part Partial Wrapping Speeds up the wrapping process Project to CAD Used by permission: Sikorsky / American Helicopter Society Import Prep Surface Volume
12 STAR-CCM+ Surface Repair Comments What does it do? Checks triangulations for valid clean/closed geometry Manipulate underlying triangulations (tessellations) How do I know if I should Surface Repair? The underlying Part is not clean/closed manifold There is no control of the CAD to fix within CAD If a Part Requires Repair: Don t panic! Undo/Forward-do buttons Surface Repair can repair the parts: Up-to-date guide flags remaining fixes Create new Part Surfaces where needed Create new Part Curves where needed Keep in Mind: It s like sewing up a bundle of triangles: Connect dots, zip edges Goal is to create a manifold, air-tight surface Import Prep Surface Volume
13 Agenda Pre-processing Geometry Origin/Import Geometry Prep Surface Mesh
14 Automated Surface Mesher Settings Automatic Surface Repair Model: Off Default settings Surface Remesher Settings: Increase minimum face quality to 0.20 Curvature=76 Surface mesher settings: Base Size to Characteristic Length/10, e.g.: Chord length/10 Characteristic Body length/10 Surface Curvature: Surface Growth Rate: Custom Surface Controls: Edge proximity on bodies to 3 Lifting Surfaces: Basic Curvature to 76 Growth rate to Target Size: Chord/100 Trailing Edges: Minimum Target Size to ¼ of t.e. thickness Inlet/Outlet/Freestream/Symmetry Boundaries: Target Surface Size to be at least characteristic length Chord/100 Proximity NACA0010 Growth = 1.05 Import Prep Surface Volume
15 Agenda Pre-processing Geometry Origin/Import Geometry Prep Surface Mesh Volume Mesh
16 Quasi-2D Core Volume Mesh Models 2D Automated Meshing (PBM): Requires an initial 3D body 2D section lies on z-axis Does not need to be CAD Applications: Airfoil analyses Test mesh settings Testing of physics settings Supersonic 2D/Axisymmetric NLF-0416 Directed Mesher (PBM): Ordered style grids High quality grids for supersonic flows Best practice topology for hypersonic cases Requires an initial 3D CAD body Workflow tip: Split patches in the CAD-Client or in 3D-CAD On Geometry transfer, choose All CAD Edges option Choose to Initialize Patches by CAD Edge Allows for macro automation 2D Axisymmetric Hypersonic bi-conic Import Prep Surface Volume
17 Core Volume Mesh Models Trimmer or Polyhedral are both acceptable topologies Refinement in flow regions of interest are key to capturing flow features in the simulation Polyhedral mesh: Aerospace cases mesh in serial Pseudo-random orientation of faces reduces numerical dissipation Smooth growth away from bodies Optimizer can increase mesh quality Prefer to control mesh based solely on remeshed surface Volume controls to catch the hard spots Trimmer mesh model: Massively parallel Faster, requires less memory Aligning the trimmer mesh model to the main flow directions can reduce numerical dissipation Mesh refinement/coarsening in factors of 2 Use of volume control to control location of transitions Lockheed Martin Public Release: ORL Import Prep Surface Volume
18 Polyhedral meshing for Aerospace Polyhedral Mesher Settings Growth Rate: Can be off or on Reduces cell count between geometry gaps Optimization Cycles Increase Optimization cycles to 1-4 Effective in aiding Adjoint case convergence Polyhedral Controls If Volume Growth Rate On Volume Growth Rate to 1.2 Maximum cell size to characteristic length Mesh Density Leave at defaults If a volume control exists in the mesh Volumetric Control Blending to 0.5 Growth Rate On Off Import Prep Surface Volume
19 Trimmer Mesher Settings Trimmer Mesh Model Settings Typically left at defaults Mesh in parallel Typical control settings Volume Growth Rate Slow to Very Slow Maximum Cell Size to characteristic length Maximum Core/Prism Transition Ratio Anywhere between 2-5 Import Prep Surface Volume
20 Prism Layer Mesher Model Settings: Stretching function: Hyperbolic Tangent Stretching Mode: Wall Thickness Minimum Thickness Percentage: 0.01 Layer Reduction Percentage: 0.0 Make conformal prisms in all layers Near Core Layer Aspect Ratio: =<1.0 Typically set to 1.0 or 0.75 Requires two inputs: Wall Thickness Prism Layer Total Height Translation: Wall Thickness = a low y+ mesh or high y+ mesh Prism Layer Total Height = Boundary Layer Thickness RAE2822 Airfoil HLPW4 Import Prep Surface Volume
21 High y+ mesh vs. Low y+ mesh High y+ mesh notes: Sub layer and buffer region is modelled by one grid cell Wall y+ value should be > 30 Wall y+ value < Typically has 8-14 prism layers Implicitly assumes that the boundary layer is turbulent and will try to reproduce the log layer behavior Low y+ mesh notes: Attempt to integrate/resolve entire boundary layer Wall y+ value should be ~< 1 Values << 1.0 will not improve results Should not be > 5.0 Has at least 10 prisms in y+ < 30 region Typically prism layers Flows that are not modelled with a transition model should not be taken as predictive transition modelling Explicitly model the trip on tripped boundary layers U Viscous sublayer Buffer-layer Log-layer Defect-layer Y+ Low y+: First grid point High y+: First grid point Import Prep Surface Volume
22 Prism Layer Techniques for Trailing Edges (or Hypersonic Leading Edges) Knife-edges lead to cells with high skewness angles High skewness angles create numerical instabilities Counter is to create refinements on the edge O-Grid, Retract O-Grid, No Retract Custom Surface Settings on Trailing Edges Create models with finite trailing edges Use Prism Layer Thickness Reduction Avoids prism layer collapse on trailing edges Avoids oddly shaped cells in the rear TE Custom Settings Import Prep Surface Volume
23 Automated Mesh Refinement STAR-CCM+ can perform automated mesh refinement : Table based refinement Custom Field Function metric for refinement Tabulate cell size refinement metric Solution based refinement Initial JAVA macro-driven volumetric control Conceptually, flow field contains arbitrary cells that contain refinement metrics Threshold Derived Parts are exported as STL files STL files can be wrapped to create volumetric control Remesh 1 New Feature in Adjoint based mesh refinement JAVA macro can drive adjoint-based mesh refinement Original Remesh 2 Refined Blunt Nose*; Mach 6.8; AoA 20 *Courtesy Lockheed Martin Missiles & Fire Control AGARD RAE 2822 Adjoint Refinement Physics Solvers
24 Agenda Pre-processing Geometry Origin/Import Geometry Prep Surface Mesh Volume Mesh Solver Settings Defining Flight Physics
25 Turbulence: RANS RANS Reynolds Averaged Navier Stokes Most common choice for external aerodynamics Robust, well studied Steady state simulations: 2D, Axisymmetric, 3D Obtains the average of all resolved flow features Extra equations add a turbulent viscosity to the dynamic viscosity in the Navier-Stokes Equations HLPW4 is the turbulence model of choice Enables use of, transition model Does not preclude the use of and its variants All y+ wall model is the preferred choice Boundary conditions: Typically left as default, but can use measured values Decay of inflow turbulent quantities can be mitigated by activating the Ambient Source Term (ASM) Do not use with the transition model Solver settings: Not uncommon to increase Turbulent Viscosity Limiter, e.g.: 1e8 Physics NLF-0416 Solvers
26 Unsteady Turbulence: URANS vs DES vs LES URANS Unsteady Reynolds Averaged Navier Stokes Run in 2D, Axisymmetric, 3D Adds unsteady term to the RANS equations Common choice for rotor performance Sliding mesh setup About 2 degrees per time step If nothing dynamically changes about the geometric configuration during the simulation, risks reverting to RANS Rotor wake from a ROBIN body DES Detached Eddy Simulation Legitimate in 3D simulations, always unsteady Popular choice for performance simulations Not prohibitively more expensive than 3D URANS IDDES = Improved Delayed DES default mode modern method Blend of RANS and Large Eddy Simulation RANS near-wall, LES everywhere else Far less turbulent viscosity in the LES regions TLG: DES Buffeting analysis 2012 STAR Global Conference Talk Physics Solvers
27 Turbulence: LES and Laminar LES Large Eddy Simulation Legitimate in 3D simulations, always unsteady Not particularly popular choice in external aero More expensive than RANS and DES High mesh counts required near walls Needed to properly resolve structures of transitioning flows Laminar Navier Stokes Equations solved directly without any turbulence model Low-speed to supersonic simulations will not likely use this Hypersonic simulations that are not interested in boundary layer will choose in conjunction with a high y+ (>100) mesh 2012 STAR Korean Conference: Satish Kumar B. et al. Transition flow and aero-acoustic analysis of NACA0018 ALM: Bow shocks on re-entry of the Crew Exploration Vehicle Physics Solvers
28 What can you get in a 2D vs. 3D simulation? 2D Simulation Enables: Fast testing for unknown physics phenomena Shock position for grid refinement Solver settings Simulations for 3D axisymmetric shapes RANS/URANS turbulence modelling Transition location using, _ Onset of trailing edge stall 3D Simulation Enables: RANS, URANS, DES, LES Complex geometry interactions Stall Prediction Physics Solvers
29 Unsteady Time Stepping Key Idea: Simulating a continuously transient behavior in a discrete fashion U(t) Time (t) T/20 is a good start 2015: STAR Global : Overset with Zero Gap Demo Physics Solvers
30 Agenda Pre-processing Geometry Origin/Import Geometry Prep Surface Mesh Volume Mesh Solver Settings Defining Flight Physics Setting Up Solvers
31 Physics Continuum Solver Choice Low Speed: P weak function of ρ, T High Speed: P strong function of ρ, T Segregated Solver SIMPLE Continuity and momentum yield a pressure-correction equation Mildly compressible flows, but not appropriate for shock capturing Flow regimes: Incompressible Low speed High speed, subsonic; Mach < ~0.5 Consider local flow Mach numbers! Lower memory requirements, faster than Coupled solver Coupled Solver Continuity, momentum, energy are solved simultaneously Equation of state yields pressure Flow regimes: Incompressible Low speed High speed, subsonic; Mach < ~0.5 All other flow speeds for Mach > ~0.5 Designed for hyperbolic nature of equations and shocks Higher memory requirements Physics Solvers
32 Solver Settings: Incompressible to Ma<0.5 If Using the Segregated Solver Simulations that use this solver should start with good initial conditions Constant velocity in the direction of the flow Smoothly ramping velocity from wall using field function Constant temperature set to flow conditions Turbulent quantities are typically default URFs are typically not ramped Rotor cases typically ramp or step RPM Unsteady simulation initialization Begin from steady state RANS solution Turn on Unsteady Solver If Using the Coupled Solver Roe FDS Initial condition: Constant velocity in direction of flow Constant temperature set to flow conditions CFL: Grid Sequencing Initialization On Expert Driver On Physics Solvers
33 Solver Settings: Transonic to Supersonic Coupled Solver Suggested Settings: Transonic (0.5 < Ma < 1.0): Roe FDS if no local Ma > 1.0 CFL from 5.0 to 50.0 Supersonic (1.0 < Ma < 4.0): AUSM+ CFL from 5.0 to 20.0, 20/Ma Grid Sequencing Initialization Turn on Expert Driver to On If no Expert Driver: Ramp CFL from 1 to 1000 Ratio of CFL Number : Explicit relaxation factor = 3:1 Physics Solvers
34 Solver Settings: Hypersonic (Ma > 4) Implicit Coupled Solver Suggested Settings: Typical CFL ~ Grid Sequencing Initialization Expert Driver Ramp CFL from 1 to 1000 CCA Turned On If no Expert Driver: Ramp CFL from 1 to 1000 Ratio of CFL Number : Explicit relaxation factor = 3:1 Mach 6.77 blunt cone: NASA TN-D1606 Physics Continuum Settings: AUSM+ May choose gradient reconstruction value between 1.0 and 2.0 Sometimes an almost 2 nd order will converge Mach 11.3 Blunt Biconic Mach 16 Shock-shock interaction on a cylinder Physics Solvers
35 Grid Sequencing Initialization (GSI) GSI Input: Physics Continuum Initial Conditions How it Works: Runs the Euler equations on successively refined series of grids, from coarse grid to finest (real) grid Wrapped Rocket GSI Initial After Condition GSI 1000 Iterations Result: Field starts at near-flight conditions Recommended Settings: Sweeps per grid level = 200 Tolerance = Notes No reason for special velocity initial conditions Develops preliminary shock locations Physics Solvers
36 Continuity Convergence Accelerator When: High Mach number aerodynamic cases CCA Input: Updated Coupled Solver flow field How it works: Solves an elliptic equation for pressure corrections Updates the cell pressures (w/underrelaxation) Corrects the face mass fluxes and cell velocities Updates density, total enthalpy, etc. appropriately Continuity Convergence Acceleration of a Density-Based Coupled Algorithm, Caraeni et al., AIAA Fluid Dynamics Conference, June 2013, San Diego, CA With CCA Without CCA Results: Can result in faster convergence for stiff problems Mixed high Mach and low Mach numbers Internal compressible flows Temperature dependent properties Settings: URF typically set Physics Solvers
37 Agenda Pre-processing Geometry Origin/Import Geometry Prep Surface Mesh Volume Mesh Solver Settings Defining Flight Physics Setting Up Solvers Post-processing Automated Data Extraction Plotting Scenes Automated Reporting
38 Interpreting the Residuals Mission statement: Simulations should be as accurate as possible. Residual values are a global metric of convergence Local convergence may get lost when only using residual values Residuals are used as a metric to judge overall quality of the simulation Used in both steady and unsteady simulations Example Residual Plots: Steady Unsteady Post
39 Checking Convergence with Engineering Criteria Both Steady and Unsteady Simulations Create Plots of Quantitative Data Skin Friction Coefficient Mass imbalance (especially for high speed flows) Lift Drag Moments Plot versus inner iteration, make sure metrics asymptotically converge onto a value For steady simulations, asymptotic behavior For unsteady simulations, asymptotic behavior within the prescribed time step s iterations Post
40 Optimate & External Aero Requires additional planning up front Testing CAD robustness Post-processing change in data sets Use JAVA to drive changes Benefits: Automated sweeps 3D-CAD parameterization CAD-client bi-directional capability Fire-and-forget Reduces burden on heavy scripting Small pieces of JAVA can be inserted into process Rotating the coordinate systems Visualization of large data sets Post-processing is collected in single tool Visualize multi-variable interactions Post
41 Post-Process Interactively on a Cluster Common practice to post-/troubleshoot on special big-memory machines External aerodynamics cases can be more than 20M cells Difficult to run multiple iterations for troubleshooting purposes Download, identify mesh issues, remesh, re-submit to queue, crash, re-download, make rhetorical statement: There s got to be another way. STAR-CCM+ client-server architecture Data is post-processed by parallel cores Visualization on workstation graphics Benefits: Increased framerates Volume rendering Line Integral Convolutions 28.8M cell DPW4 model on 4 64 cores Client location: Los Angeles, CA Server location: Detroit, MI Post
42 Agenda Pre-processing Geometry Origin/Import Geometry Prep Surface Mesh Volume Mesh Solver Settings Defining Flight Physics Setting Up Solvers Post-processing Automated Data Extraction Plotting Scenes Automated Reporting
43 Thank You Time for any questions
Introduction to ANSYS CFX
Workshop 03 Fluid flow around the NACA0012 Airfoil 16.0 Release Introduction to ANSYS CFX 2015 ANSYS, Inc. March 13, 2015 1 Release 16.0 Workshop Description: The flow simulated is an external aerodynamics
More informationRecent & Upcoming Features in STAR-CCM+ for Aerospace Applications Deryl Snyder, Ph.D.
Recent & Upcoming Features in STAR-CCM+ for Aerospace Applications Deryl Snyder, Ph.D. Outline Introduction Aerospace Applications Summary New Capabilities for Aerospace Continuity Convergence Accelerator
More informationMissile External Aerodynamics Using Star-CCM+ Star European Conference 03/22-23/2011
Missile External Aerodynamics Using Star-CCM+ Star European Conference 03/22-23/2011 StarCCM_StarEurope_2011 4/6/11 1 Overview 2 Role of CFD in Aerodynamic Analyses Classical aerodynamics / Semi-Empirical
More informationCAD-BASED WORKFLOWS. VSP Workshop 2017
CAD-BASED WORKFLOWS VSP Workshop 2017 RESEARCH IN FLIGHT COMPANY Established 2012 Primary functions are the development, marketing and support of FlightStream and the development of aerodynamic solutions
More informationHigh-Lift Aerodynamics: STAR-CCM+ Applied to AIAA HiLiftWS1 D. Snyder
High-Lift Aerodynamics: STAR-CCM+ Applied to AIAA HiLiftWS1 D. Snyder Aerospace Application Areas Aerodynamics Subsonic through Hypersonic Aeroacoustics Store release & weapons bay analysis High lift devices
More informationSTAR-CCM+: Wind loading on buildings SPRING 2018
STAR-CCM+: Wind loading on buildings SPRING 2018 1. Notes on the software 2. Assigned exercise (submission via Blackboard; deadline: Thursday Week 3, 11 pm) 1. NOTES ON THE SOFTWARE STAR-CCM+ generates
More informationIntroduction to CFX. Workshop 2. Transonic Flow Over a NACA 0012 Airfoil. WS2-1. ANSYS, Inc. Proprietary 2009 ANSYS, Inc. All rights reserved.
Workshop 2 Transonic Flow Over a NACA 0012 Airfoil. Introduction to CFX WS2-1 Goals The purpose of this tutorial is to introduce the user to modelling flow in high speed external aerodynamic applications.
More informationTransition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon Kim, Hogeon Kim
Transition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon Kim, Hogeon Kim Transition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon
More informationDebojyoti Ghosh. Adviser: Dr. James Baeder Alfred Gessow Rotorcraft Center Department of Aerospace Engineering
Debojyoti Ghosh Adviser: Dr. James Baeder Alfred Gessow Rotorcraft Center Department of Aerospace Engineering To study the Dynamic Stalling of rotor blade cross-sections Unsteady Aerodynamics: Time varying
More informationNUMERICAL 3D TRANSONIC FLOW SIMULATION OVER A WING
Review of the Air Force Academy No.3 (35)/2017 NUMERICAL 3D TRANSONIC FLOW SIMULATION OVER A WING Cvetelina VELKOVA Department of Technical Mechanics, Naval Academy Nikola Vaptsarov,Varna, Bulgaria (cvetelina.velkova1985@gmail.com)
More informationExpress Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil
Express Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 -
More informationSTAR-CCM+ User Guide 6922
STAR-CCM+ User Guide 6922 Introduction Welcome to the STAR-CCM+ introductory tutorial. In this tutorial, you explore the important concepts and workflow. Complete this tutorial before attempting any others.
More informationModeling External Compressible Flow
Tutorial 3. Modeling External Compressible Flow Introduction The purpose of this tutorial is to compute the turbulent flow past a transonic airfoil at a nonzero angle of attack. You will use the Spalart-Allmaras
More informationCoupling of STAR-CCM+ to Other Theoretical or Numerical Solutions. Milovan Perić
Coupling of STAR-CCM+ to Other Theoretical or Numerical Solutions Milovan Perić Contents The need to couple STAR-CCM+ with other theoretical or numerical solutions Coupling approaches: surface and volume
More informationCompressible Flow Modeling in STAR-CCM+
Compressible Flow Modeling in STAR-CCM+ Version 01/11 Content Day 1 Compressible Flow WORKSHOP: High-speed flow around a missile WORKSHOP: Supersonic flow in a nozzle WORKSHOP: Airfoil 3 27 73 97 2 Compressible
More informationDetached Eddy Simulation Analysis of a Transonic Rocket Booster for Steady & Unsteady Buffet Loads
Detached Eddy Simulation Analysis of a Transonic Rocket Booster for Steady & Unsteady Buffet Loads Matt Knapp Chief Aerodynamicist TLG Aerospace, LLC Presentation Overview Introduction to TLG Aerospace
More informationEstimation of Flow Field & Drag for Aerofoil Wing
Estimation of Flow Field & Drag for Aerofoil Wing Mahantesh. HM 1, Prof. Anand. SN 2 P.G. Student, Dept. of Mechanical Engineering, East Point College of Engineering, Bangalore, Karnataka, India 1 Associate
More informationAIR LOAD CALCULATION FOR ISTANBUL TECHNICAL UNIVERSITY (ITU), LIGHT COMMERCIAL HELICOPTER (LCH) DESIGN ABSTRACT
AIR LOAD CALCULATION FOR ISTANBUL TECHNICAL UNIVERSITY (ITU), LIGHT COMMERCIAL HELICOPTER (LCH) DESIGN Adeel Khalid *, Daniel P. Schrage + School of Aerospace Engineering, Georgia Institute of Technology
More informationApplication of STAR-CCM+ to Helicopter Rotors in Hover
Application of STAR-CCM+ to Helicopter Rotors in Hover Lakshmi N. Sankar and Chong Zhou School of Aerospace Engineering, Georgia Institute of Technology, Atlanta, GA Ritu Marpu Eschol CD-Adapco, Inc.,
More informationTHE EFFECTS OF THE PLANFORM SHAPE ON DRAG POLAR CURVES OF WINGS: FLUID-STRUCTURE INTERACTION ANALYSES RESULTS
March 18-20, 2013 THE EFFECTS OF THE PLANFORM SHAPE ON DRAG POLAR CURVES OF WINGS: FLUID-STRUCTURE INTERACTION ANALYSES RESULTS Authors: M.R. Chiarelli, M. Ciabattari, M. Cagnoni, G. Lombardi Speaker:
More informationStudies of the Continuous and Discrete Adjoint Approaches to Viscous Automatic Aerodynamic Shape Optimization
Studies of the Continuous and Discrete Adjoint Approaches to Viscous Automatic Aerodynamic Shape Optimization Siva Nadarajah Antony Jameson Stanford University 15th AIAA Computational Fluid Dynamics Conference
More informationContribution to GMGW-1
Contribution to GMGW-1 Vivek Ahuja, Shaunak Pai, John Wilson, Rajesh Kumar, Michael Stubert Inc. (003) Restricted Siemens AG 2017 Realize innovation. Summary of meshes generated Star-CCM+ Geometry Core
More informationBest Practices: Volume Meshing Kynan Maley
Best Practices: Volume Meshing Kynan Maley Volume Meshing Volume meshing is the basic tool that allows the creation of the space discretization needed to solve most of the CAE equations for: CFD Stress
More informationANSYS FLUENT. Airfoil Analysis and Tutorial
ANSYS FLUENT Airfoil Analysis and Tutorial ENGR083: Fluid Mechanics II Terry Yu 5/11/2017 Abstract The NACA 0012 airfoil was one of the earliest airfoils created. Its mathematically simple shape and age
More informationBest Practices Workshop: Parts & Mesh-Based Operations
Best Practices Workshop: Parts & Mesh-Based Operations Overview What are Parts and Mesh Based Operations? Transition from Region Based Meshing Why move to Parts Based Meshing How to use Parts Based Mesh
More informationAerodynamic Analysis of Forward Swept Wing Using Prandtl-D Wing Concept
Aerodynamic Analysis of Forward Swept Wing Using Prandtl-D Wing Concept Srinath R 1, Sahana D S 2 1 Assistant Professor, Mangalore Institute of Technology and Engineering, Moodabidri-574225, India 2 Assistant
More informationFluent User Services Center
Solver Settings 5-1 Using the Solver Setting Solver Parameters Convergence Definition Monitoring Stability Accelerating Convergence Accuracy Grid Independence Adaption Appendix: Background Finite Volume
More informationValidation of an Unstructured Overset Mesh Method for CFD Analysis of Store Separation D. Snyder presented by R. Fitzsimmons
Validation of an Unstructured Overset Mesh Method for CFD Analysis of Store Separation D. Snyder presented by R. Fitzsimmons Stores Separation Introduction Flight Test Expensive, high-risk, sometimes catastrophic
More informationModeling Unsteady Compressible Flow
Tutorial 4. Modeling Unsteady Compressible Flow Introduction In this tutorial, FLUENT s density-based implicit solver is used to predict the timedependent flow through a two-dimensional nozzle. As an initial
More informationAccurate and Efficient Turbomachinery Simulation. Chad Custer, PhD Turbomachinery Technical Specialist
Accurate and Efficient Turbomachinery Simulation Chad Custer, PhD Turbomachinery Technical Specialist Outline Turbomachinery simulation advantages Axial fan optimization Description of design objectives
More informationRBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent
RBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent Gilles Eggenspieler Senior Product Manager 1 Morphing & Smoothing A mesh morpher is a tool capable of performing mesh modifications in order
More informationµ = Pa s m 3 The Reynolds number based on hydraulic diameter, D h = 2W h/(w + h) = 3.2 mm for the main inlet duct is = 359
Laminar Mixer Tutorial for STAR-CCM+ ME 448/548 March 30, 2014 Gerald Recktenwald gerry@pdx.edu 1 Overview Imagine that you are part of a team developing a medical diagnostic device. The device has a millimeter
More informationAutomated calculation report (example) Date 05/01/2018 Simulation type
Automated calculation report (example) Project name Tesla Semi Date 05/01/2018 Simulation type Moving Table of content Contents Table of content... 2 Introduction... 3 Project details... 3 Disclaimer...
More informationSolution Recording and Playback: Vortex Shedding
STAR-CCM+ User Guide 6663 Solution Recording and Playback: Vortex Shedding This tutorial demonstrates how to use the solution recording and playback module for capturing the results of transient phenomena.
More informationComputational Fluid Dynamics for Engineers
Tuncer Cebeci Jian P. Shao Fassi Kafyeke Eric Laurendeau Computational Fluid Dynamics for Engineers From Panel to Navier-Stokes Methods with Computer Programs With 152 Figures, 19 Tables, 84 Problems and
More informationThe Spalart Allmaras turbulence model
The Spalart Allmaras turbulence model The main equation The Spallart Allmaras turbulence model is a one equation model designed especially for aerospace applications; it solves a modelled transport equation
More informationAil implicit finite volume nodal point scheme for the solution of two-dimensional compressible Navier-Stokes equations
Ail implicit finite volume nodal point scheme for the solution of two-dimensional compressible Navier-Stokes equations Vimala Dutta Computational and Theoretical Fluid Dynamics Division National Aerospace
More informationIntroduction to C omputational F luid Dynamics. D. Murrin
Introduction to C omputational F luid Dynamics D. Murrin Computational fluid dynamics (CFD) is the science of predicting fluid flow, heat transfer, mass transfer, chemical reactions, and related phenomena
More informationImpact of STAR-CCM+ v7.0 in the Automotive Industry Frederick J. Ross, CD-adapco Director, Ground Transportation
Impact of STAR-CCM+ v7.0 in the Automotive Industry Frederick J. Ross, CD-adapco Director, Ground Transportation Vehicle Simulation Components Vehicle Aerodynamics Design Studies Aeroacoustics Water/Dirt
More informationLES Applications in Aerodynamics
LES Applications in Aerodynamics Kyle D. Squires Arizona State University Tempe, Arizona, USA 2010 Tutorial School on Fluid Dynamics: Topics in Turbulence Center for Scientific Computation and Mathematical
More informationS-ducts and Nozzles: STAR-CCM+ at the Propulsion Aerodynamics Workshop. Peter Burns, CD-adapco
S-ducts and Nozzles: STAR-CCM+ at the Propulsion Aerodynamics Workshop Peter Burns, CD-adapco Background The Propulsion Aerodynamics Workshop (PAW) has been held twice PAW01: 2012 at the 48 th AIAA JPC
More informationNumerical Investigation of Transonic Shock Oscillations on Stationary Aerofoils
Numerical Investigation of Transonic Shock Oscillations on Stationary Aerofoils A. Soda, T. Knopp, K. Weinman German Aerospace Center DLR, Göttingen/Germany Symposium on Hybrid RANS-LES Methods Stockholm/Sweden,
More informationAn efficient method for predicting zero-lift or boundary-layer drag including aeroelastic effects for the design environment
The Aeronautical Journal November 2015 Volume 119 No 1221 1451 An efficient method for predicting zero-lift or boundary-layer drag including aeroelastic effects for the design environment J. A. Camberos
More informationCOMPUTATIONAL AND EXPERIMENTAL INTERFEROMETRIC ANALYSIS OF A CONE-CYLINDER-FLARE BODY. Abstract. I. Introduction
COMPUTATIONAL AND EXPERIMENTAL INTERFEROMETRIC ANALYSIS OF A CONE-CYLINDER-FLARE BODY John R. Cipolla 709 West Homeway Loop, Citrus Springs FL 34434 Abstract A series of computational fluid dynamic (CFD)
More informationEstimating Vertical Drag on Helicopter Fuselage during Hovering
Estimating Vertical Drag on Helicopter Fuselage during Hovering A. A. Wahab * and M.Hafiz Ismail ** Aeronautical & Automotive Dept., Faculty of Mechanical Engineering, Universiti Teknologi Malaysia, 81310
More informationGerman Aerospace Center, Institute of Aerodynamics and Flow Technology, Numerical Methods
Automatische Transitionsvorhersage im DLR TAU Code Status der Entwicklung und Validierung Automatic Transition Prediction in the DLR TAU Code - Current Status of Development and Validation Andreas Krumbein
More informationResearch and Design working characteristics of orthogonal turbine Nguyen Quoc Tuan (1), Chu Dinh Do (2), Quach Thi Son (2)
GSJ: VOLUME 6, ISSUE 6, JUNE 018 116 Research and Design working characteristics of orthogonal turbine Nguyen Quoc Tuan (1), Chu Dinh Do (), Quach Thi Son () (1) Institute for hydro power and renewable
More informationSteady Flow: Lid-Driven Cavity Flow
STAR-CCM+ User Guide Steady Flow: Lid-Driven Cavity Flow 2 Steady Flow: Lid-Driven Cavity Flow This tutorial demonstrates the performance of STAR-CCM+ in solving a traditional square lid-driven cavity
More informationVerification and Validation of Turbulent Flow around a Clark-Y Airfoil
Verification and Validation of Turbulent Flow around a Clark-Y Airfoil 1. Purpose 58:160 Intermediate Mechanics of Fluids CFD LAB 2 By Tao Xing and Fred Stern IIHR-Hydroscience & Engineering The University
More informationCase C3.1: Turbulent Flow over a Multi-Element MDA Airfoil
Case C3.1: Turbulent Flow over a Multi-Element MDA Airfoil Masayuki Yano and David L. Darmofal Aerospace Computational Design Laboratory, Massachusetts Institute of Technology I. Code Description ProjectX
More informationRecent Advances in Modelling Wind Parks in STAR CCM+ Steve Evans
Recent Advances in Modelling Wind Parks in STAR CCM+ Steve Evans Introduction Company STAR-CCM+ Agenda Wind engineering at CD-adapco STAR-CCM+ & EnviroWizard Developments for Offshore Simulation CD-adapco:
More informationSupersonic Flow Over a Wedge
SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 2 Supersonic Flow Over a Wedge Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification A uniform supersonic stream encounters a wedge
More informationOptimization of under-relaxation factors. and Courant numbers for the simulation of. sloshing in the oil pan of an automobile
Optimization of under-relaxation factors and Courant numbers for the simulation of sloshing in the oil pan of an automobile Swathi Satish*, Mani Prithiviraj and Sridhar Hari⁰ *National Institute of Technology,
More informationApplication of Wray-Agarwal Turbulence Model for Accurate Numerical Simulation of Flow Past a Three-Dimensional Wing-body
Washington University in St. Louis Washington University Open Scholarship Mechanical Engineering and Materials Science Independent Study Mechanical Engineering & Materials Science 4-28-2016 Application
More information(c)2002 American Institute of Aeronautics & Astronautics or Published with Permission of Author(s) and/or Author(s)' Sponsoring Organization.
VIIA Adaptive Aerodynamic Optimization of Regional Introduction The starting point of any detailed aircraft design is (c)2002 American Institute For example, some variations of the wing planform may become
More informationAxisymmetric Viscous Flow Modeling for Meridional Flow Calculation in Aerodynamic Design of Half-Ducted Blade Rows
Memoirs of the Faculty of Engineering, Kyushu University, Vol.67, No.4, December 2007 Axisymmetric Viscous Flow Modeling for Meridional Flow alculation in Aerodynamic Design of Half-Ducted Blade Rows by
More informationIntroduction to Computational Fluid Dynamics Mech 122 D. Fabris, K. Lynch, D. Rich
Introduction to Computational Fluid Dynamics Mech 122 D. Fabris, K. Lynch, D. Rich 1 Computational Fluid dynamics Computational fluid dynamics (CFD) is the analysis of systems involving fluid flow, heat
More informationRecent developments for the multigrid scheme of the DLR TAU-Code
www.dlr.de Chart 1 > 21st NIA CFD Seminar > Axel Schwöppe Recent development s for the multigrid scheme of the DLR TAU-Code > Apr 11, 2013 Recent developments for the multigrid scheme of the DLR TAU-Code
More informationAnalysis of an airfoil
UNDERGRADUATE RESEARCH FALL 2010 Analysis of an airfoil using Computational Fluid Dynamics Tanveer Chandok 12/17/2010 Independent research thesis at the Georgia Institute of Technology under the supervision
More informationShape optimisation using breakthrough technologies
Shape optimisation using breakthrough technologies Compiled by Mike Slack Ansys Technical Services 2010 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary Introduction Shape optimisation technologies
More informationFLUID DYNAMICS ANALYSIS OF A COUNTER ROTATING DUCTED PROPELLER
FLUID DYNAMICS ANALYSIS OF A COUNTER ROTATING DUCTED PROPELLER Chao Xu, Cees Bil, Sherman CP. Cheung School of Aerospace, Mechanical and Manufacturing Engineering, RMIT University Keywords: Twin counter-rotating
More informationCompressible Flow in a Nozzle
SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 1 Compressible Flow in a Nozzle Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification Consider air flowing at high-speed through a
More informationFlow Field of Truncated Spherical Turrets
Flow Field of Truncated Spherical Turrets Kevin M. Albarado 1 and Amelia Williams 2 Aerospace Engineering, Auburn University, Auburn, AL, 36849 Truncated spherical turrets are used to house cameras and
More informationDirect Numerical Simulation of a Low Pressure Turbine Cascade. Christoph Müller
Low Pressure NOFUN 2015, Braunschweig, Overview PostProcessing Experimental test facility Grid generation Inflow turbulence Conclusion and slide 2 / 16 Project Scale resolving Simulations give insight
More informationGrid. Apr 09, 1998 FLUENT 5.0 (2d, segregated, lam) Grid. Jul 31, 1998 FLUENT 5.0 (2d, segregated, lam)
Tutorial 2. Around an Airfoil Transonic Turbulent Flow Introduction: The purpose of this tutorial is to compute the turbulent flow past a transonic airfoil at a non-zero angle of attack. You will use the
More informationEXPERIMENTAL VALIDATION OF STAR-CCM+ FOR LIQUID CONTAINER SLOSH DYNAMICS
EXPERIMENTAL VALIDATION OF STAR-CCM+ FOR LIQUID CONTAINER SLOSH DYNAMICS Brandon Marsell a.i. solutions, Launch Services Program, Kennedy Space Center, FL 1 Agenda Introduction Problem Background Experiment
More informationAdjoint Solver Workshop
Adjoint Solver Workshop Why is an Adjoint Solver useful? Design and manufacture for better performance: e.g. airfoil, combustor, rotor blade, ducts, body shape, etc. by optimising a certain characteristic
More informationStrömningslära Fluid Dynamics. Computer laboratories using COMSOL v4.4
UMEÅ UNIVERSITY Department of Physics Claude Dion Olexii Iukhymenko May 15, 2015 Strömningslära Fluid Dynamics (5FY144) Computer laboratories using COMSOL v4.4!! Report requirements Computer labs must
More informationIsotropic Porous Media Tutorial
STAR-CCM+ User Guide 3927 Isotropic Porous Media Tutorial This tutorial models flow through the catalyst geometry described in the introductory section. In the porous region, the theoretical pressure drop
More informationSHOCK WAVES IN A CHANNEL WITH A CENTRAL BODY
SHOCK WAVES IN A CHANNEL WITH A CENTRAL BODY A. N. Ryabinin Department of Hydroaeromechanics, Faculty of Mathematics and Mechanics, Saint-Petersburg State University, St. Petersburg, Russia E-Mail: a.ryabinin@spbu.ru
More informationDigital-X. Towards Virtual Aircraft Design and Testing based on High-Fidelity Methods - Recent Developments at DLR -
Digital-X Towards Virtual Aircraft Design and Testing based on High-Fidelity Methods - Recent Developments at DLR - O. Brodersen, C.-C. Rossow, N. Kroll DLR Institute of Aerodynamics and Flow Technology
More informationEffect of Position of Wall Mounted Surface Protrusion in Drag Characteristics At Low Reynolds Number
ISSN (e): 2250 3005 Volume, 07 Issue, 11 November 2017 International Journal of Computational Engineering Research (IJCER) Effect of Position of Wall Mounted Surface Protrusion in Drag Characteristics
More informationCFD Analysis of conceptual Aircraft body
CFD Analysis of conceptual Aircraft body Manikantissar 1, Dr.Ankur geete 2 1 M. Tech scholar in Mechanical Engineering, SD Bansal college of technology, Indore, M.P, India 2 Associate professor in Mechanical
More informationSecond Symposium on Hybrid RANS-LES Methods, 17/18 June 2007
1 Zonal-Detached Eddy Simulation of Transonic Buffet on a Civil Aircraft Type Configuration V.BRUNET and S.DECK Applied Aerodynamics Department The Buffet Phenomenon Aircraft in transonic conditions Self-sustained
More informationA STUDY ON THE UNSTEADY AERODYNAMICS OF PROJECTILES IN OVERTAKING BLAST FLOWFIELDS
HEFAT2012 9 th International Conference on Heat Transfer, Fluid Mechanics and Thermodynamics 16 18 July 2012 Malta A STUDY ON THE UNSTEADY AERODYNAMICS OF PROJECTILES IN OVERTAKING BLAST FLOWFIELDS Muthukumaran.C.K.
More informationCFD VALIDATION FOR SURFACE COMBATANT 5415 STRAIGHT AHEAD AND STATIC DRIFT 20 DEGREE CONDITIONS USING STAR CCM+
CFD VALIDATION FOR SURFACE COMBATANT 5415 STRAIGHT AHEAD AND STATIC DRIFT 20 DEGREE CONDITIONS USING STAR CCM+ by G. J. Grigoropoulos and I..S. Kefallinou 1. Introduction and setup 1. 1 Introduction The
More informationUsing a Single Rotating Reference Frame
Tutorial 9. Using a Single Rotating Reference Frame Introduction This tutorial considers the flow within a 2D, axisymmetric, co-rotating disk cavity system. Understanding the behavior of such flows is
More informationSTAR-CCM+: Ventilation SPRING Notes on the software 2. Assigned exercise (submission via Blackboard; deadline: Thursday Week 9, 11 pm)
STAR-CCM+: Ventilation SPRING 208. Notes on the software 2. Assigned exercise (submission via Blackboard; deadline: Thursday Week 9, pm). Features of the Exercise Natural ventilation driven by localised
More informationAbstract. Introduction
EULER SOLUTIONS AS LIMIT OF INFINITE REYNOLDS NUMBER FOR SEPARATION FLOWS AND FLOWS WITH VORTICES Wolfgang Schmidt and Antony Jameson Dornier GmbH, D-7990 Friedrichshafen, FRG and Princeton University,
More informationUsage of CFX for Aeronautical Simulations
Usage of CFX for Aeronautical Simulations Florian Menter Development Manager Scientific Coordination ANSYS Germany GmbH Overview Elements of CFD Technology for aeronautical simulations: Grid generation
More informationHPC Usage for Aerodynamic Flow Computation with Different Levels of Detail
DLR.de Folie 1 HPCN-Workshop 14./15. Mai 2018 HPC Usage for Aerodynamic Flow Computation with Different Levels of Detail Cornelia Grabe, Marco Burnazzi, Axel Probst, Silvia Probst DLR, Institute of Aerodynamics
More informationNumerical Methods in Aerodynamics. Fluid Structure Interaction. Lecture 4: Fluid Structure Interaction
Fluid Structure Interaction Niels N. Sørensen Professor MSO, Ph.D. Department of Civil Engineering, Alborg University & Wind Energy Department, Risø National Laboratory Technical University of Denmark
More informationAERODYNAMIC DESIGN AND OPTIMIZATION TOOLS ACCELERATED BY PARAMETRIC GEOMETRY PREPROCESSING
1 European Congress on Computational Methods in Applied Sciences and Engineering ECCOMAS 2000 Barcelona, 11-14 September 2000 ECCOMAS AERODYNAMIC DESIGN AND OPTIMIZATION TOOLS ACCELERATED BY PARAMETRIC
More informationThe viscous forces on the cylinder are proportional to the gradient of the velocity field at the
Fluid Dynamics Models : Flow Past a Cylinder Flow Past a Cylinder Introduction The flow of fluid behind a blunt body such as an automobile is difficult to compute due to the unsteady flows. The wake behind
More informationStudy of Swept Angle Effects on Grid Fins Aerodynamics Performance
Journal of Physics: Conference Series PAPER OPEN ACCESS Study of Swept Angle Effects on Grid Fins Aerodynamics Performance To cite this article: G A Faza et al 2018 J. Phys.: Conf. Ser. 1005 012013 View
More informationCFD Study of a Darreous Vertical Axis Wind Turbine
CFD Study of a Darreous Vertical Axis Wind Turbine Md Nahid Pervez a and Wael Mokhtar b a Graduate Assistant b PhD. Assistant Professor Grand Valley State University, Grand Rapids, MI 49504 E-mail:, mokhtarw@gvsu.edu
More informationINSTABILITY OF A SHOCK WAVE OVER A BACKWARD FACING RAMP
INSTABILITY OF A SHOCK WAVE OVER A BACKWARD FACING RAMP Alexander Kuzmin and Konstantin Babarykin Department of Fluid Dynamics, St. Petersburg State University, Russia E-Mail: a.kuzmin@spbu.ru ABSTRACT
More informationMeshing in STAR-CCM+: Recent Advances Aly Khawaja
Meshing in STAR-CCM+: Recent Advances Aly Khawaja Outline STAR-CCM+: a complete simulation workflow Emphasis on pre-processing technology Recent advances in surface preparation and meshing Continue to
More informationSimulation of Turbulent Flow around an Airfoil
1. Purpose Simulation of Turbulent Flow around an Airfoil ENGR:2510 Mechanics of Fluids and Transfer Processes CFD Lab 2 (ANSYS 17.1; Last Updated: Nov. 7, 2016) By Timur Dogan, Michael Conger, Andrew
More informationANSYS AIM Tutorial Compressible Flow in a Nozzle
ANSYS AIM Tutorial Compressible Flow in a Nozzle Author(s): Sebastian Vecchi Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Pre-Analysis Start-Up Geometry Import Geometry Mesh
More informationStreamlining Aircraft Icing Simulations. D. Snyder, M. Elmore
Streamlining Aircraft Icing Simulations D. Snyder, M. Elmore Industry Analysis Needs / Trends Fidelity Aircraft Ice Protection Systems-Level Modeling Optimization Background Ice accretion can critically
More informationCase C2.2: Turbulent, Transonic Flow over an RAE 2822 Airfoil
Case C2.2: Turbulent, Transonic Flow over an RAE 2822 Airfoil Masayuki Yano and David L. Darmofal Aerospace Computational Design Laboratory, Massachusetts Institute of Technology I. Code Description ProjectX
More informationFlow Structures Extracted from Visualization Images: Vector Fields and Topology
Flow Structures Extracted from Visualization Images: Vector Fields and Topology Tianshu Liu Department of Mechanical & Aerospace Engineering Western Michigan University, Kalamazoo, MI 49008, USA We live
More informationSPC 307 Aerodynamics. Lecture 1. February 10, 2018
SPC 307 Aerodynamics Lecture 1 February 10, 2018 Sep. 18, 2016 1 Course Materials drahmednagib.com 2 COURSE OUTLINE Introduction to Aerodynamics Review on the Fundamentals of Fluid Mechanics Euler and
More informationCOMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE METERING SITUATIONS UNDER ABNORMAL CONFIGURATIONS
COMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE METERING SITUATIONS UNDER ABNORMAL CONFIGURATIONS Dr W. Malalasekera Version 3.0 August 2013 1 COMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE
More informationHigh-Order Numerical Algorithms for Steady and Unsteady Simulation of Viscous Compressible Flow with Shocks (Grant FA )
High-Order Numerical Algorithms for Steady and Unsteady Simulation of Viscous Compressible Flow with Shocks (Grant FA9550-07-0195) Sachin Premasuthan, Kui Ou, Patrice Castonguay, Lala Li, Yves Allaneau,
More informationChallenges in Boundary- Layer Stability Analysis Based On Unstructured Grid Solutions
Challenges in Boundary- Layer Stability Analysis Based On Unstructured Grid Solutions Wei Liao National Institute of Aerospace, Hampton, Virginia Collaborators: Mujeeb R. Malik, Elizabeth M. Lee- Rausch,
More informationCalculate a solution using the pressure-based coupled solver.
Tutorial 19. Modeling Cavitation Introduction This tutorial examines the pressure-driven cavitating flow of water through a sharpedged orifice. This is a typical configuration in fuel injectors, and brings
More informationSimulation of Turbulent Flow over the Ahmed Body
Simulation of Turbulent Flow over the Ahmed Body 58:160 Intermediate Mechanics of Fluids CFD LAB 4 By Timur K. Dogan, Michael Conger, Maysam Mousaviraad, and Fred Stern IIHR-Hydroscience & Engineering
More informationCFD Methods for Aerodynamic Design
CFD Methods for Aerodynamic Design Afandi Darlington Optimal Aerodynamics Ltd Why CFD? Datasheet methods are still very relevant today (ESDU, USAF DATCOM) Validated estimates of lift, drag, moments, stability
More information