Introduction To FLUENT. David H. Porter Minnesota Supercomputer Institute University of Minnesota

Transcription

1 Introduction To FLUENT David H. Porter Minnesota Supercomputer Institute University of Minnesota

2 Topics Covered in this Tutorial What you can do with FLUENT FLUENT is feature rich Summary of features and capabilities Using FLUENT at MSI Essentials of working with FLUENT Hosts, X forwarding, environment, startup Basic steps for success User Resources at MSI Web documentation: User Guides & tutorials Help is available: helpline & forums

3 What You Can Do With FLUENT Flow problems in 2D and 3D Compressible & Incompressible Steady state and time dependent Variety of material properties Complex physics & chemsitry Inviscid, viscous, and turbulence models Complex geometries & meshes Multiple and non-inertial reference frames Quantitative analysis & visualization

4 Flow Problems in 2D and 3D 2D Planar Axisymmetric Axisymmetric with swirl 3D Full 3D Complex boundaries

5 Compressible and Incompressible Low subsonic Incompressible or weakly compressible Constant or variable density Equation of state Transonic Strong compressibility Shock waves Supersonic & Hypersonic Inviscid model Euler discontinuities Strong shocks

6 Steady State and Time Dependent Iterative convergence to steady state solutions Follow transient solutions Use steady state solution to initialize transient problems.

7 Material Properties Newtonian & non-newtonian fluids Phase changes Melting and solidification Porous media Non-isotropic permeability Inertial resistance Solid heat conduction Porous-face pressure jump conditions Material properties database Porous media in a catalytic converter

8 Chemistry Chemical Species Mixing Reaction Combustion models Homogeneous Heterogeneous Surface deposition/reaction models

9 Complex Physics MHD Heat transfer solid/fluid conjugate transfer Forced, natural & mixed convection Volume sources of mass, momentum and energy Acoustic models: flow induced noise 000 Natural Convection Velocity field

10 Viscosity & Turbulence Models Models for various flow regimes Laminar (only for smooth flows) Viscous (Navier-Stokes) Turbulence models Large Eddy Simulations (LES) Detached Eddy Simulation Spalart-Allmaras (1 eqn) K-epsilon (standard & RNG) (2 eqn) K-omega (2 eqn) Reynolds Stress (7 eqn)

11 Complex Geometries & Meshes Various and mixed meshes Structured, unstructured, & mixed Sliding meshes Mixing-plane model Time averaged mesh boundaries Dynamic (deforming) meshes Free surfaces GAMBIT: mesh generation T-GRID: merge meshes

12 Reference Frames Inertial Stationary or moving Non-inertial Rotating Accelerating Multiple reference frames Meshes in relative motion

13 Quantitative Analysis XY plots of values along lines Primitive & derived quantities Surface and volume integrals Fluxes Averages Temporal variation Fourier analysis

14 Flow Visualization On surfaces Contours Primitive and derived fields In volumes Particle paths Vector fields Colored with scalar fields Animation Time dependent flows Moving viewpoint

15 Using FLUENT at MSI Hardware to run FLUENT on Computational resources at MSI MSI maintains academic licenses from ANSYS Run locally in MSI labs Running remotely on core hardware SSH & X forwarding Getting Started Environmental settings & modules Tutorial files & run directories GUIs for GAMBIT & FLUENT

16 FLUENT Availability at MSI Core hardware (remote access) Altix (up to 256 processors) Regatta (up to 32 processors) Labs (run locally or remotely) BMSDL SDVL

17 Running Remotely GUI driven GAMBIT & FLUENT From your graphics & X11 enabled desktop X11 is standard with Linux shells On Mac use an xterm shell & ssh -Y... On Windows, need X server & SSH client X server: XMing SSH client: PuTTY Linux: SSH to remote host with X forwarding ssh -X <user_name>@regatta.msi.umn.edu

18 Getting Started Use the fluent module to set your environment module load fluent GAMBIT & FLUENT produce many files Good idea to make a project directory Tutorial resource files available on regatta Meshes & example output Zipped files for each tutorial /usr/local/fluent.inc/fluent6.3.26/help/tutfiles

19 Essentials of Working with FLUENT Dream up a problem Draw a picture with labels for consistency Use GAMBIT to generate mesh Specify geometry & boundaries Specify solver, mesh type & resolution Use FLUENT to generate flow solutions Specify models, boundaries, material properties Specify solver approx, monitors, & iterate... Adapt/refine mesh Examine/compare results

20 Example Problem Channel flow with backward-facing step Classic problem from turbulence Our example: 2D for simplicity & speed Will solve for steady state solution Compare results from different models Re = (2/3)U(2h)/nu = 500 Lambros, Kaiktsis, Karniadakis, & Orszag, 1991 JFM vol. 231, pp Rani, Sheu, & Tsai, 2007, JFM vol. 588, pp. 4358

21 Define Geometry Y vop=(10,1) vip=(-1,1) Wall Inflow Wall vi0=(-1,0) vmm=(0,-1) vm0=(0,0) Wall X Wall 2D problem: Z=0 Walls can be free slip or no slip Use default MKS units Outflow vom=(10,-1)

22 Mesh Generation: Outline Setup & start GAMBIT Specify FLUENT 5/6 solver 0D: Vertices from point coordinates 1D: Edges from pairs of vertexes 2D: Domain from edges Specify 1D meshes on Edges Interior mesh (on face) from 1D meshes Associate boundary types & labels with edges Save work & export mesh

23 Setup GAMBIT Project Directory Make directory: mkdir step Enter directory: cd step Start GAMBIT module load fluent gambit Specify solver menu: solver -> FLUENT 5/6

24 Specify Vertices Vertexes from point coordinates Operation: GEOMETRY button Geometry: VETREX button Vertex: CREATE VERTEX button Enter coordinates with labels & APPLY for each pair vip (-1,1) vmm (0,-1) vim (-1,0) vom (10,-1) vm0 (0,0) vop (10,1) Resize view to see all Global Control: FIT TO WINDOW button

25 Create 1D Edges & 2D Domain Edges from pairs of vertices Geometry: EDGE button Edge: CREATE EDGE button: strait edge (default) Select pairs of vertices, label, & Apply in ibot step {vip, vim} {vim, vm0} {vm0, vmm} bot out top {vmm, vom} {vom, vop} {vop, vip} Face from edges Geometry: FACE button Face: FORM FACE button Select all edges, label domain, & Apply

26 Generate Mesh 1D Mesh on Edges (0.1 m mesh) Operation: MESH button Mesh: EDGE button Mesh Edges dialog: Spacing: 0.1 (interval size) Select all edges & Apply Mesh 2D domain from edges Mesh: FACE button Face: MESH FACES button Mesh faces dialog: Select all edges Retain defaults for quad mesh & Apply

27 Boundary Types Associate boundary types & labels with edges Operation: ZONES button Zones: SPECIFY BOUNDARY TYPES button Specify Boundary Types dialog: Edge, label, boundary type, in out top bot ibot step inlet outlet top bot ibot step VELOCITY_INLET PRESURE_OUTLET WALL WALL WALL WALL Apply

28 Save Work & Export Mesh Good Idea to save GAMBIT session Modify or fix mesh as needed Use as a starting point for another project Menu: File -> Save As... Export mesh Generates a mesh file: step.msh Will import this file into FLUENT Menu: File -> Export -> Mesh... Enable Export 2-D (X-Y) Mesh File name: step.msh Accept

29 Solve for Steady State Solution Use FLUENT Import mesh Models: solver, viscous, source terms,... Material properties Boundary conditions Operating conditions Solution controls & initialization Monitors Iterate...

30 Setup FLUENT Use step project directory Contains file: step.msh Set environment: module load fluent Only need to do once per shell Can put module load... in file:.bashrc Run FLUENT for 2D simulations fluent 2D Import mesh from file step.msh File -> Read -> Case Check mesh: Grid -> Check

31 Choose Model Solver framework Define -> Models -> Solver Retain defaults Energy equation? Define -> Models -> Energy... Simple, low Mach flow: Try energy eqn. off Viscosity model Define -> Models -> Viscous... Try Laminar option.

32 Materials & Boundaries Select fluid Define -> Materials... Can select from Database Can define your own Will keep default: air Dynamic Viscosity: e-05 [kg/m-s] Boundaries: Define -> Bounary Conditions Select Inlet (Velocity Inlet) & Set... Set Velocity Magnitude: m/s (Re ~ 500) Retain default settings for outlet (Pressure Outlet) Retain defaults for all other boundaries (Wall)

33 Operating Conditions & Solver Controls Set operating conditions Define -> Operating Conditions... Retain defaults NOTE: panel entry fields adapt to model chosen. Set solver controls Solve -> Controls -> Solution Discretization: Momentum: 2nd order Upwind Retain other defaults

34 Initialization & Monitors Initialize flow on mesh Solve -> Initialize -> Initialize... Compute From: inlet Init Solution convergence monitors Solve -> Monitors -> Residual... Select Plot under Options Increase Storage & Plotting iterations to Keep Continuity, X-, & Y-velocity monitors

35 Iterative Solution to Steady State Iterate Solver -> Iterate... Set # of iterations to 1000 Iterate Laminar: unrealistic Low res. mesh Numerical Diff. Need Turb. Visc. Save settings & data File -> Write -> Case & Data...

36 Try a Turbulence Model Standard K-epsilon model Define -> Models -> Viscous... Select k-epsilon (2 eqn) Retain standard default settings Solver for SGS fields Solve -> Controls -> Solution... 2nd order Upwind for TKE & TDR Iterate...

37 Examine Flow Vector fields Contours Particle paths XY plots along lines or edges Quantitative reports Compare results from different models Hard copy output File -> Hardcopy... I've used: JPEG & Color

38 Flow Visualization Display -> Vectors In subsets of full domain Colored by... Zoom with middle mouse button Display -> Contours... Select Filled under Options Display -> Pathlines... Steps 200; Path skip 2 Release from default-interior

39 Quantitative Results Pressure along a vertical cut Surface -> Line/Rake X0=X1=0.6; Y0=-1; Y1=1 Name: x=0.6 Plot -> XY Plot... Plot Direction: (X,Y,Z)=(0,1,0) Surfaces: x=0.6 & Plot Quantitative reports Report -> Fluxes... Select: Inlet & Outlet Retain Mass Flow Rate Compute Mass Flow Rate inlet outlet Net (kg/s) e-07

40 Compare Results from Different Models Plot -> XY Plot... Select Write to File Write Switch cases File -> Write -> Case & Date File -> Read -> Case & Data Plot -> XY Plot... Load File... Select file: keps_vx_on_x=0.6.xy Plot

41 Adapt/Refine Mesh Reason: test & improve accuracy Refinement based on your choice of Gradients Residual errors Domain Adapt -> Region X=[-1,10]; y=[-1,1] Adapt doubles mesh Solver -> Iterate...

42 Comparison of Vx from 3 Models

43 User Resources at MSI User Guide & tutorials on the WEB: GAMBIT: FLUENT: MSI User Support Phone: (8:30am 5pm) MSI web portals & Forums Still in planning stages Will be under MSI web site

44 Proposed: MSI Forum on Fluid Dynamics/Continuum Mech. Interdisciplinary & interdepartmental Theory, Experiment, Computation Facilitate access to local resources & opportunities Share knowhow Address questions & concerns with MSI resources Brainstorm projects leveraged by MSI resources Still in planning stages Forums will be user driven Your input is crucial