Transcript Slide 1

Chapter 3
Solver Basics
Introductory FLUENT
Training
Sharif University of Technology
Lecturer: Ehsan Saadati
[email protected]
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-1
April 28, 2009
Inventory #002600
Solver Basics
FLUENT 12 GUI Navigation
Training Manual
• The FLUENT GUI is arranged such that the tasks are generally
arranged from top to bottom in the project setup tree.
• Selecting an item in the tree opens the relevant input items in the
center pane.
–
–
–
–
General
Models
Materials
Boundary
Conditions
– Solver Settings
– Initialization and
Calculation
– Postprocessing
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-2
April 28, 2009
Inventory #002600
Solver Basics
Scaling the Mesh and Selecting Units
Training Manual
• When FLUENT reads a mesh
file (.msh), all physical
dimensions are assumed to be
in units of meters.
– If your model was not built in
meters, then it must be scaled.
– Verify that the Domain Extents
are correct after scaling the
mesh.
• When importing a mesh under
Workbench, the mesh does not
need to be scaled; however, the
units are set to the default MKS
system.
Define
Units…
• Any “mixed” units system can
be used if desired.
– By default, FLUENT uses the SI
system of units (specifically,
MKS system).
– Any units can be specified in
the Set Units panel, accessed
from the top menu.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-3
April 28, 2009
Inventory #002600
Solver Basics
Text User Interface
Training Manual
• Most GUI commands
have a corresponding
TUI command.
– Many advanced
commands are only
available through
the TUI.
– Press the Enter key
to display the
command set at the
current level.
– q moves up one level.
• FLUENT can be run
in batch mode or
scripted using a
journal file (see
Appendix)
• A TUI user guide is available on the FLUENT User Services Center
www.fluentusers.com
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-4
April 28, 2009
Inventory #002600
Solver Basics
Mouse Functionality
Training Manual
• Mouse button functionality depends on the chosen solver (2D / 3D)
and can be configured in the solver.
Display
Mouse Buttons…
• Default settings
– 2D Solver
• Left button translates/pans (dolly)
• Middle button zooms
• Right button selects/probes
– 3D Solver
• Left button rotates about 2 axes
• Middle button zooms
– Middle click on point in screen centers point
in window
• Right button selects/probes
• Retrieve detailed flow field information at point with Probe enabled.
– Right-click on the graphics display.
• Mouse controls can be set to emulate those in Workbench!
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-5
April 28, 2009
Inventory #002600
Solver Basics
Material Properties
Training Manual
• FLUENT provides a standard
database of materials and the
ability to create a custom
user-defined database.
• Your choice of physical models
may require multiple materials
and dictate which material
properties must be defined.
– Multiphase (multiple materials)
– Combustion (multiple species)
– Heat transfer (thermal
conductivity)
– Radiation (emissivity and
absorptivity)
• Material properties can be directly customized as function of
temperature/pressure
– Use of other solution variable(s) requires UDF.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-6
April 28, 2009
Inventory #002600
Solver Basics
Materials Databases
Training Manual
• FLUENT materials database
– Provides access to a number
of pre-defined fluid, solid and
mixture materials.
– Materials can be copied to
the case file and edited if
required.
• Custom material database:
– Create a new custom database
of material properties and
reaction mechanisms from
materials in an existing case
file for reuse in future cases.
– Custom databases can be created,
accessed and modified from the
standard materials panel in FLUENT.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-7
April 28, 2009
Inventory #002600
Solver Basics
Operating Conditions
Training Manual
• The Operating Pressure with a Reference
Pressure Location sets the reference
value that is used in computing gauge
pressures.
• The Operating Temperature sets the
reference temperature
(used when computing
buoyancy forces.
• Specified Operating
Density sets the reference
value for flows with widely
varying density.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-8
April 28, 2009
Inventory #002600
Solver Basics
Parallel Processing
Training Manual
• Parallel processing can be used to run
FLUENT on multiple processors to
decrease turnaround time and increase
simulation efficiency.
– Critical for cases involving large meshes
and/or complex physics.
– FLUENT is fully parallelized and capable of
running across most hardware and
software configurations, such as compute
clusters or multi-processor machines.
• Parallel FLUENT can be launched either
using the system command prompt or
using the FLUENT Launcher panel.
– For example, to launch an n-CPU parallel
session, use the command
fluent 3d –tn
• The mesh can be partitioned either
manually or automatically using a number
of different methods.
– Non-conformal meshes, sliding mesh
interfaces and shell conduction zones
require partitioning in serial.
• A web-based lecture is available on the
FLUENT User Services Center.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-9
April 28, 2009
Inventory #002600
Solver Basics
Summary
Training Manual
• This lecture has presented many basic tasks that are often performed
during a CFD simulation setup.
• Parallel processing can be used to reduce calculation time. This is
advantageous only on large meshes.
• A later lecture contains material related to the setup and solution of
time-dependent problems.
• Other topics not discussed (see Appendix for information).
–
–
–
–
Mesh heirarchy and relationships.
Reordering and modifying the mesh in the solver.
Polyhedral mesh conversion.
Solution-based mesh adaption.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-10
April 28, 2009
Inventory #002600
Appendix
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-11
April 28, 2009
Inventory #002600
Solver Basics
FLUENT Journals
Training Manual
• FLUENT can be run in batch mode using
journal files.
• A journal file is a text file which contains
TUI commands which FLUENT will execute
sequentially.
• The FLUENT TUI accepts abbreviations of
the commands; for example,
–
–
–
–
–
–
ls
rcd
wcd
rc/wc
rd/wd
it
Lists the files in the working folder
Reads case and data files
Writes case and data files
Reads/writes case file
Reads/writes data file
Iterate
• TUI commands in a batch file can be used
to automate operations in a non-interactive
mode.
– The TUI commands file/read-bc and
file/write-bc can be used for reading
and writing the settings for a FLUENT
session to and from a file, respectively.
– A web-based training module is available
which explains this process
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-12
Sample Journal File
; Read case file
rc example.cas.gz
; Initialize the solution
/solve/initialize/initialize-flow
; Calculate 50 iterations
it 50
; Write data file
wd example50.dat.gz
; Calculate another 50 iterations
it 50
; Write another data file
wd example100.dat.gz
; Exit FLUENT
exit
yes
April 28, 2009
Inventory #002600
Solver Basics
Reading the Mesh – Zones
Training Manual
plate
plate-shadow
wall
outlet
Default-interior zone(s)
can always be ignored.
inlet
fluid (cell zone)
• In this example, there are two cell zones (fluid-upstream and fluiddownstream).
• Because of this, FLUENT splits the exterior wall zone into two zones
(wall and wall:001). This is because an external boundary cannot
span multiple cell zones.
• FLUENT also splits the orifice plate into two walls also (plate and
plate-shadow) since the plate zone is an internal wall.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-13
April 28, 2009
Inventory #002600
Solver Basics
Mesh Information and Hierarchy
Training Manual
• All mesh information is stored in the mesh file.
– Node coordinates
– Connectivity
– Zone definition
Node
• Similar to the way geometry is defined, mesh
entities obey a hierarchy:
– Node
– Edge
– Face
– Cell
– Zone
Cell
Center
Edge intersection / grid point
Boundary of a face (defined by
two nodes
The boundaries of cells, defined by
a collection of edges
The control volumes into which the
domain is discretized.
A collection of nodes, edges, faces
or cells.
Cell Face
Boundary
Face
Cell
Simple 2D Mesh
• The computational domain is defined by all
members of the hierarchy
Node
– For fluid flow simulation only, the domain consists
only of the fluid region.
– For conjugate heat transfer or fluid-structure
interaction problems, the domain needs to include
any solid parts that are present.
Boundary
Face
• Boundary data is assigned to face zones.
• Material data and source terms are assigned to
cell zones.
Edge
Cell
Simple 3D mesh
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-14
April 28, 2009
Inventory #002600
Solver Basics
Reordering and Modifying the Grid
Training Manual
• The grid can be reordered so that neighboring cells are near each
other in the zones and in memory
– Improves efficiency of memory access and reduces the bandwidth of the
computation
– Reordering can be performed for the entire domain or specific cell zones.
Grid
Reorder
Grid
Domain
Reorder
Zones
– The bandwidth of each partition in the grid can be printed for reference.
Grid
Reorder
Print Bandwidth
• The face/cell zones can also be modified by the following operations
in the Grid menu:
–
–
–
–
–
–
Separation and merge of zones
Fusing of cell zones with merge of duplicate faces and nodes
Translate, rotate, reflect face or cell zones
Extrusion of face zones to extend the domain
Replace a cell zone with another or delete it
Activate and Deactivate cell zones
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-15
April 28, 2009
Inventory #002600
Solver Basics
Polyhedral Mesh Conversion
Training Manual
• A tetrahedral or hybrid grid can be
converted to polyhedra in the FLUENT GUI
(not in the preprocessor).
Tet/Hybrid Mesh
– Generate a tetrahedral mesh then convert
inside FLUENT.
– Advantages
• Improved mesh quality.
• Can reduce cell count significantly.
• User has control of the conversion process.
– Disadvantages:
• Cannot be adapted or converted again.
• Cannot use tools such as smooth, swap, merge
and extrude to modify the mesh.
• Two conversion options are available in the
Grid menu: Grid Polyhedra Convert Domain
Polyhedral Mesh
– Convert all cells in the domain (except hex
cells) to polyhedra
• Cannot convert meshes with hanging nodes
• HexCore mesh can be converted using the tpoly
standalone utility.
– Convert only highly skewed cells to
polyhedra
Grid
Polyhedra
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
Convert Skewed Cells
3-16
April 28, 2009
Inventory #002600
Solver Basics
Profile Data and Solution Data Interpolation
Training Manual
• FLUENT allows interpolation of selected
variable data on both face zones and cell
zones by using profile files and data
interpolation files, respectively.
– For example, a velocity profile from
experimental data or previous FLUENT run
at an inlet, or a solution interpolated from
a coarse mesh to fine mesh.
File
Write
Profile…
File
Read
Profile…
• Profile files are data files which contain
point data for selected variables on
particular face zones, and can be both
written and read in a FLUENT session.
File
Interpolate…
• Similarly, Interpolation data files contain
discrete data for selected field variables
on particular cell zones to be written and
read into FLUENT.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-17
April 28, 2009
Inventory #002600
Solver Basics
Mesh Adaption
Training Manual
• Mesh adaption refers to refinement
and/or coarsening cells where needed
to resolve the flow field without
returning to the preprocessor.
– Mark cells satisfying the adaption
criteria and store them in a “register.”
– Display and modify the register if
desired.
– Click Adapt to adapt the cells listed in
the
register.
Refine Threshold should
be set to 10% of the value
reported in the Max field.
• Registers can be defined based on:
– Gradients or isovalues of all variables
– All cells on a boundary
– All cells in a region with a defined
shape
– Cell volumes or volume changes
– y+ in cells adjacent to walls
• To assist adaption process, you can:
–
–
–
–
Combine adaption registers
Draw contours of adaption function
Display cells marked for adaption
Limit adaption based on cell size
and number of cells
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-18
April 28, 2009
Inventory #002600
Solver Basics
Adaption Example – Supersonic Projectile
Training Manual
• Adapt grid in regions of large pressure gradient to better resolve the
sudden pressure rise across the shock.
Large pressure gradient
indicating a shock (poor
resolution on coarse
mesh)
Initial Mesh (Generated by Preprocessor)
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
3-19
Pressure Contours on Initial Mesh
April 28, 2009
Inventory #002600
Solver Basics
Adaption Example – Supersonic Projectile
Training Manual
• Solution-based mesh adaption allows better resolution of the bow
shock and expansion wave.
Mesh adaption yields
much better resolution
of the bow shock.
Adapted cells
in locations of
large pressure
gradients
Adapted Mesh (Multiple Adaptions
Based on Gradients of Pressure)
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
Pressure Contours on Adapted Mesh
3-20
April 28, 2009
Inventory #002600