Introduction To FLUENT by xdu18397

VIEWS: 835 PAGES: 44

									Introduction To FLUENT


           David H. Porter
  Minnesota Supercomputer Institute
       University of Minnesota
        Topics Covered in this Tutorial
●   What you can do with FLUENT
    –   FLUENT is feature rich
    –   Summary of features and capabilities
●   Using FLUENT at MSI
    –   Hosts, X forwarding, environment, startup
●   Essentials of working with FLUENT
    –   Basic steps for success
●   User Resources at MSI
    –   Web documentation: User Guides & tutorials
    –   Help is available: helpline & forums
    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
          Flow Problems in 2D and 3D
●   2D
    –   Planar
    –   Axisymmetric
    –   Axisymmetric with swirl



●   3D
    –   Full 3D
    –   Complex boundaries
    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
    Steady State and Time Dependent
●   Iterative convergence to
    steady state solutions

●   Follow transient solutions

●   Use steady state solution
    to initialize transient
    problems.
                   Material Properties
●   Newtonian & non-Newtonian fluids
●   Phase changes
    –   Melting and solidification

●   Porous media
    –   Non-isotropic permeability
    –   Inertial resistance           Porous media in a catalytic converter
    –   Solid heat conduction
    –   Porous-face pressure jump conditions

●   Material properties database
                      Chemistry
●   Chemical Species
    –   Mixing
    –   Reaction

●   Combustion models
    –   Homogeneous
    –   Heterogeneous

●   Surface deposition/reaction models
     Complex Physics
●   MHD                                       000



●   Heat transfer
    –   solid/fluid “conjugate” transfer     Natural Convection
                                             Velocity field
    –   Forced, natural & mixed convection

●   Volume sources of mass,
    momentum and energy

●   Acoustic models: flow induced
    noise
        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)
        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
                   Reference Frames
●   Inertial
    –   Stationary or moving

●   Non-inertial
    –   Rotating
    –   Accelerating

●   Multiple reference frames
    –   Meshes in relative motion
                 Quantitative Analysis
●   XY plots of values along
    lines
    –   Primitive & derived
        quantities
●   Surface and volume
    integrals
    –   Fluxes
    –   Averages
●   Temporal variation
●   Fourier analysis
    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
               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
          FLUENT Availability at MSI

●   Core hardware (remote access)
    –   Altix (up to 256 processors)
    –   Regatta (up to 32 processors)
         http://www.msi.umn.edu/hardware/


●   Labs (run locally or remotely)
    –   BMSDL
    –   SDVL
         http://www.msi.umn.edu/labs/
                 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
    http://www.cs.caltech.edu/courses/cs11/misc/xwindows.html


●   Linux: SSH to remote host with X forwarding
    ssh -X <user_name>@regatta.msi.umn.edu
                       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
         http://wwwr.msi.umn.edu/fluent/tutfiles/
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
                     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
                                                 Rani, Sheu, & Tsai, 2007,
JFM vol. 231, pp. 501-528
                                                 JFM vol. 588, pp. 43–58
                              Define Geometry
                          Y


    vip=(-1,1)                                  vop=(10,1)
                                 Wall                        Outflow
Inflow
                  Wall    vm0=(0,0)
                                                                 X
     vi0=(-1,0)
                          Wall
                                    Wall
             vmm=(0,-1)                          vom=(10,-1)




         ●2D problem: Z=0
         ●Walls can be free slip or no slip

         ●Use default MKS units
        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
                      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
          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
         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      {vip, vim}     bot   {vmm, vom}
         ibot    {vim, vm0}     out   {vom, vop}
         step    {vm0, vmm}     top   {vop, vip}

●   Face from edges
    –   Geometry: FACE button
    –   Face: FORM FACE button
    –   Select all edges, label “domain”, & Apply
                         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
                              Boundary Types
●   Associate boundary types &
    labels with edges
    –   Operation: ZONES button
    –   Zones: SPECIFY BOUNDARY
        TYPES button
    –   Specify Boundary Types dialog:
         ●   Edge, label , boundary type,      Apply
              in     inlet    VELOCITY_INLET
              out    outlet   PRESURE_OUTLET
              top    top      WALL
              bot    bot      WALL
              ibot   ibot     WALL
              step   step     WALL
            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
     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 ...
                     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
          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.
    Materials & Boundaries
●   Select fluid
     Define -> Materials ...
     –   Can select from Database
     –   Can define your own
     –   Will keep default: air
          ●   Dynamic Viscosity: 1.7894e-05 [kg/m-s]
●   Boundaries: Define -> Bounary Conditions
     –   Select Inlet (Velocity Inlet) & Set...
     –   Set Velocity Magnitude: 0.002435 m/s (Re ~ 500)
     –   Retain default settings for outlet (Pressure Outlet)
     –   Retain defaults for all other boundaries (Wall)
    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
               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 10000
    –   Keep Continuity, X-, & Y-velocity
        monitors
        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 ...
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 ...
                    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
                    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”
                      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 ...
                                               Mass Flow Rate    (kg/s)
    –   Select: Inlet & Outlet                 inlet            0.0029828751
                                               outlet           -0.0029837638
    –   Retain Mass Flow Rate                  Net              -8.887e-07
    –   Compute
    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
                     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 ...
Comparison of Vx from 3 Models
               User Resources at MSI
●   User Guide & tutorials on the WEB:
    –   GAMBIT: http://wwwr.msi.umn.edu/gambit/index.htm
    –   FLUENT: http://wwwr.msi.umn.edu/fluent/index.htm

●   MSI User Support
    –   Email: help@msi.umn.edu
    –   Phone: 612–626–0802 (8:30am – 5pm)

●   MSI web portals & Forums
    –   Still in planning stages
    –   Will be under MSI web site http://www.msi.umn.edu
                  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
    –   Email: porter@msi.umn.edu

								
To top