Docstoc

wb cm

Document Sample
wb cm Powered By Docstoc
					                       CFX-Mesh




ANSYS, Inc.                       Release 12.0
Southpointe                       April 2009
275 Technology Drive              ANSYS, Inc. is
Canonsburg, PA 15317              certified to ISO
ansysinfo@ansys.com               9001:2008.
http://www.ansys.com
(T) 724-746-3304
(F) 724-514-9494
Copyright and Trademark Information
© 2009 SAS IP, Inc. All rights reserved. Unauthorized use, distribution or duplication is prohibited.

ANSYS, ANSYS Workbench, Ansoft, AUTODYN, EKM, Engineering Knowledge Manager, CFX, FLUENT, HFSS and any and
all ANSYS, Inc. brand, product, service and feature names, logos and slogans are registered trademarks or trademarks
of ANSYS, Inc. or its subsidiaries in the United States or other countries. ICEM CFD is a trademark used by ANSYS, Inc.
under license. CFX is a trademark of Sony Corporation in Japan. All other brand, product, service and feature names
or trademarks are the property of their respective owners.

Disclaimer Notice
THIS ANSYS SOFTWARE PRODUCT AND PROGRAM DOCUMENTATION INCLUDE TRADE SECRETS AND ARE CONFIDENTIAL
AND PROPRIETARY PRODUCTS OF ANSYS, INC., ITS SUBSIDIARIES, OR LICENSORS. The software products and document-
ation are furnished by ANSYS, Inc., its subsidiaries, or affiliates under a software license agreement that contains pro-
visions concerning non-disclosure, copying, length and nature of use, compliance with exporting laws, warranties,
disclaimers, limitations of liability, and remedies, and other provisions. The software products and documentation may
be used, disclosed, transferred, or copied only in accordance with the terms and conditions of that software license
agreement.
ANSYS, Inc. is certified to ISO 9001:2008.

U.S. Government Rights
For U.S. Government users, except as specifically granted by the ANSYS, Inc. software license agreement, the use, du-
plication, or disclosure by the United States Government is subject to restrictions stated in the ANSYS, Inc. software
license agreement and FAR 12.212 (for non-DOD licenses).

Third-Party Software
See the legal information in the product help files for the complete Legal Notice for ANSYS proprietary software and
third-party software. If you are unable to access the Legal Notice, please contact ANSYS, Inc.

Published in the U.S.A.
Table of Contents
What is CFX-Mesh? ..................................................................................................................................... 1
   Overview of the Meshing Process ............................................................................................................ 1
   Mesh Adaption ....................................................................................................................................... 3
Graphical User Interface ............................................................................................................................. 5
   Main Menu ............................................................................................................................................. 6
       File Menu ......................................................................................................................................... 6
       Tools Menu ...................................................................................................................................... 7
       View Menu ....................................................................................................................................... 8
       Go Menu .......................................................................................................................................... 8
       Help Menu ....................................................................................................................................... 8
   Toolbars and Icons .................................................................................................................................. 9
       File Toolbar ....................................................................................................................................... 9
       Graphics Interaction Tools ................................................................................................................. 9
            Rotation Cursors in the Rotate Mode ......................................................................................... 11
       Selection Tools ............................................................................................................................... 12
            Selection Filters ........................................................................................................................ 13
            Point Selection ......................................................................................................................... 13
       Selection Mode Toolbar .................................................................................................................. 14
       Display Toolbar ............................................................................................................................... 14
            Triad ......................................................................................................................................... 15
            Ruler ........................................................................................................................................ 15
            Mesh Edge Length Display ........................................................................................................ 15
       Geometry Toolbar ........................................................................................................................... 15
       Meshing Toolbar ............................................................................................................................. 16
       Interrupt ......................................................................................................................................... 16
   Tree View .............................................................................................................................................. 17
       Suppressing Objects ....................................................................................................................... 19
       Hiding Objects ............................................................................................................................... 20
   Details View .......................................................................................................................................... 21
   Graphics Window ................................................................................................................................. 22
   Messages Window ................................................................................................................................ 22
Geometry .................................................................................................................................................. 25
   Geometry Update ................................................................................................................................. 25
   Geometry Requirements ....................................................................................................................... 26
       General Geometry Requirements .................................................................................................... 27
       Multiple Bodies, Parts and Assemblies ............................................................................................. 27
       Geometry and Topology for Solid Bodies ......................................................................................... 27
            Bodies Joined by a Common Face ............................................................................................. 28
            Bodies Touching at a Face ......................................................................................................... 28
            Body with a Hole ...................................................................................................................... 29
            Body with an Enclosed Body ..................................................................................................... 29
            Bodies with an Enclosed Body and a Hole .................................................................................. 30
            Body with an Enclosed Body Touching the Face ......................................................................... 31
       Geometry and Topology for the Faces of Solid Bodies ...................................................................... 32
            Non-Manifold Geometry ........................................................................................................... 32
            Closed Faces ............................................................................................................................. 33
            Merging Topology .................................................................................................................... 34
       Geometry and Topology for the Faces of an Inflated Boundary ......................................................... 34
       Geometry for Thin Surfaces ............................................................................................................. 35
            Thin Surface Topology Restrictions ............................................................................................ 35

                               Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                           of ANSYS, Inc. and its subsidiaries and affiliates.                                             iii
CFX-Mesh

                   Example 1: Free Floating Thin Surface .................................................................................. 36
                   Example 2: Attached Thin Surface ........................................................................................ 36
              2D Regions for Thin Surfaces ..................................................................................................... 37
         Poorly-Parameterized Surfaces ........................................................................................................ 37
              Example 1: Distorting the Square .............................................................................................. 39
              Example 2: Circle ....................................................................................................................... 39
              Example 3: Uneven Parametric Lines ......................................................................................... 39
              Example 4: Degenerate Surfaces ............................................................................................... 40
              Example 5: Cusps ...................................................................................................................... 40
         Degenerate Geometry .................................................................................................................... 40
    Geometry Checking .............................................................................................................................. 41
         Sliver Edge Checking ...................................................................................................................... 42
         Sliver Face Checking ....................................................................................................................... 43
         Parameterization Face Checking ..................................................................................................... 43
         Verify Options ................................................................................................................................. 43
    Geometry Fixing: Short Edge Removal ................................................................................................... 44
    Suppression of Bodies and Parts ........................................................................................................... 45
    Geometry Display ................................................................................................................................. 46
Virtual Topology ....................................................................................................................................... 47
    General Information on Virtual Topology ............................................................................................... 47
    Virtual Faces ......................................................................................................................................... 48
    Virtual Edges ........................................................................................................................................ 51
         Virtual Edges and Short Edge Removal ............................................................................................ 53
    Automatic Virtual Topology ................................................................................................................... 55
Regions ..................................................................................................................................................... 57
    2D Regions ........................................................................................................................................... 57
         2D Regions and Faces ..................................................................................................................... 57
         Composite 2D Regions and Default 2D Region ................................................................................ 58
    Named Selections in CFX-Mesh ............................................................................................................. 59
Meshing Features ..................................................................................................................................... 63
    Spacing ................................................................................................................................................ 63
         Body Spacing ................................................................................................................................. 63
         Face Spacing .................................................................................................................................. 64
         Edge Spacing ................................................................................................................................. 65
         Angular Resolution ......................................................................................................................... 67
         Relative Error .................................................................................................................................. 67
    Controls ............................................................................................................................................... 68
         Point Spacing ................................................................................................................................. 68
         Point Control .................................................................................................................................. 69
         Line Control .................................................................................................................................... 70
         Triangle Control .............................................................................................................................. 71
    Periodicity ............................................................................................................................................ 72
         Periodic Pair ................................................................................................................................... 73
         Geometry Requirements for Periodic Pairs ....................................................................................... 74
         Mesh Generation Process for a Periodic Pair ..................................................................................... 74
         Extruded Periodic Pair ..................................................................................................................... 75
    Inflation ............................................................................................................................................... 75
         Inflation - Details ............................................................................................................................ 76
              First Layer Thickness ................................................................................................................. 77
              Total Thickness ......................................................................................................................... 79
              Advanced Quality Checking ...................................................................................................... 80
         Inflated Boundary ........................................................................................................................... 81


                                Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
iv                                                          of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                                CFX-Mesh

           Inflating Between Thin Gaps ..................................................................................................... 82
           Inflating the Inside Walls of Cylindrical Pipes .............................................................................. 82
   Stretch ................................................................................................................................................. 83
   Proximity .............................................................................................................................................. 84
       Edge Proximity ............................................................................................................................... 84
       Surface Proximity ............................................................................................................................ 85
   Mesh Options ....................................................................................................................................... 86
       Global Mesh Scaling ....................................................................................................................... 86
       Surface Meshing ............................................................................................................................. 87
           Delaunay Surface Mesher ......................................................................................................... 87
           Advancing Front (AF) Surface Mesher ........................................................................................ 87
       Meshing Strategy ........................................................................................................................... 87
       Advancing Front and Inflation 3D .................................................................................................... 88
           Advancing Front Volume Mesher .............................................................................................. 88
           Parallel Volume Meshing ........................................................................................................... 88
       Extruded 2D Meshing ..................................................................................................................... 90
           Extruded 2D Meshing Options .................................................................................................. 91
           Extruded Periodic Pair ............................................................................................................... 93
           Geometry Requirements for Extruded 2D Meshing .................................................................... 94
           Mesh Generation Process for Extruded 2D Meshing ................................................................... 95
Previewing the Mesh ................................................................................................................................ 97
   Preview Group ...................................................................................................................................... 97
   Controlling the Display of Surface Mesh ................................................................................................ 98
Volume Meshing ..................................................................................................................................... 101
   Generating the Volume Mesh .............................................................................................................. 101
   Saving the Volume Mesh ..................................................................................................................... 101
CFX-Mesh Options on the Options Dialog Box ....................................................................................... 103
Troubleshooting ..................................................................................................................................... 107
   Common Queries ................................................................................................................................ 107
       Why can the Mesher Fail Trying to Create a Surface Mesh? ............................................................. 107
       Why can the Mesher Fail Trying to Create a Mesh with Inflation? .................................................... 107
       How can I Create a Mesh Greater than 1 km Across? ....................................................................... 108
       How can I Ask to See the Warning Messages that the Mesher Produces? ......................................... 108
       Which Part of my Model is Causing the Problem? ........................................................................... 108
       Why do I get Messages About Disk Space when I Have Plenty of Space in my Project Directory? ..... 108
       What are the Files which CFX-Mesh Produces? ............................................................................... 108
   Valid and Invalid Values for Parameters, Locations and Names .............................................................. 109
       Valid and Invalid Parameter Values ................................................................................................ 109
       Valid and Invalid Locations ............................................................................................................ 110
       Valid and Invalid Names ................................................................................................................ 111
   Meshing Warning and Error Messages ................................................................................................. 111
       The Advancing Front Surface Mesher Cannot be Used When Parametrically Closed Surfaces or Curves
       are Present in the Geometry .......................................................................................................... 111
       CAD Edge Referenced n Times by Faces ......................................................................................... 111
       CAD Model Contains Faces with Small Angles ................................................................................ 112
       CAD Vertex Referred to n Times by CAD Face ................................................................................. 112
       Edge is Periodic ............................................................................................................................ 112
       Face for Edge is Periodic ................................................................................................................ 112
       Face has Less than 2 Edges ............................................................................................................ 112
       Invalid Periodicity in Faces Detected .............................................................................................. 112
       Matching Periodic CAD Vertices Exceed Tolerance ......................................................................... 112
       No Edges Found in Search Box ...................................................................................................... 112


                               Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                           of ANSYS, Inc. and its subsidiaries and affiliates.                                               v
CFX-Mesh

         Storage Allocation Failed .............................................................................................................. 113
         Surface is Parametrically Closed .................................................................................................... 113
         Surface Mesh has Triangles which are Identical .............................................................................. 113
         There was a Problem Converting the Mesher Output into the GTM Database ................................. 113
         2 Transformations Specified .......................................................................................................... 113
         Two or More CAD Edges Between Non-inflated Surfaces Meet at a CAD Vertex on an Inflated Sur-
         face .............................................................................................................................................. 113
         The Volume Mesher Cannot Continue. It is Continually Adding and Removing the Same Ele-
         ments. .......................................................................................................................................... 114
         Zero Length Vector ....................................................................................................................... 114
Guidelines ............................................................................................................................................... 115
     Mesh Length Scale .............................................................................................................................. 115
I. CFX-Mesh Tutorials ............................................................................................................................... 117
     Introduction to the CFX-Mesh Tutorials ........................................................................................... 119
         List of Features ............................................................................................................................. 122
     Tutorial 1: Static Mixer ...................................................................................................................... 125
         The Meshing Process Using CFX-Mesh ........................................................................................... 125
         Geometry Creation ....................................................................................................................... 126
         Mesh Generation .......................................................................................................................... 136
     Tutorial 2: Static Mixer (Refined Mesh) ............................................................................................. 145
         Modifying the Mesh Generation .................................................................................................... 145
         Further Geometry Modification ..................................................................................................... 147
         Updating the Geometry in CFX-Mesh ............................................................................................ 150
     Tutorial 3: Process Injection Mixing Pipe .......................................................................................... 151
         Geometry Creation ....................................................................................................................... 151
         Mesh Generation .......................................................................................................................... 154
     Tutorial 4: Circular Vent .................................................................................................................... 157
         Geometry Creation ....................................................................................................................... 157
         Mesh Generation .......................................................................................................................... 159
     Tutorial 5: Blunt Body ....................................................................................................................... 163
         Geometry Creation ....................................................................................................................... 163
         Mesh Generation .......................................................................................................................... 167
     Tutorial 6: Butterfly Valve ................................................................................................................. 173
         Geometry Creation ....................................................................................................................... 173
         Mesh Generation .......................................................................................................................... 176
     Tutorial 7: Catalytic Converter .......................................................................................................... 181
         Geometry Creation ....................................................................................................................... 181
         Mesh Generation .......................................................................................................................... 187
     Tutorial 8: Annulus ............................................................................................................................ 189
         Geometry Creation ....................................................................................................................... 189
         Mesh Generation .......................................................................................................................... 190
     Tutorial 9: Mixing Tube ..................................................................................................................... 195
         Geometry Creation ....................................................................................................................... 195
         Mesh Generation .......................................................................................................................... 198
     Tutorial 10: Heating Coil ................................................................................................................... 201
         Geometry Creation ....................................................................................................................... 201
         Mesh Generation .......................................................................................................................... 206
     Tutorial 11: Airlift Reactor ................................................................................................................ 211
         Geometry Creation ....................................................................................................................... 211
         Mesh Generation .......................................................................................................................... 217
     Tutorial 12: Room with Air Conditioning .......................................................................................... 219
         Geometry Creation ....................................................................................................................... 219


                                Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
vi                                                          of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                                   CFX-Mesh

         Mesh Generation .......................................................................................................................... 223
    Tutorial 13: Can Combustor .............................................................................................................. 225
         Geometry Import .......................................................................................................................... 225
         Mesh Generation .......................................................................................................................... 227
    Tutorial 14: CAD Cleanup and Meshing ............................................................................................ 231
         Mesh Generation .......................................................................................................................... 231
Index ........................................................................................................................................................ 243




                                Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                            of ANSYS, Inc. and its subsidiaries and affiliates.                                               vii
       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
viii                               of ANSYS, Inc. and its subsidiaries and affiliates.
What is CFX-Mesh?
CFX-Mesh is a mesh generator aimed at producing high quality meshes for use in computational fluid dy-
namics (CFD) simulations. CFD requires meshes that can resolve boundary layer phenomena and satisfy
more stringent quality criteria than structural analyses.

CFX-Mesh produces meshes containing tetrahedra, prisms, and pyramids in standard 3D meshing mode,
and additionally can include hexahedra in the Extrude 2D meshing mode. The mesh produced in CFX-Mesh
can be stored as the meshing database file (.mshdb) or a CFX Mesh file (.gtm). Extensive advanced
surface and volume mesh generation controls are available in CFX-Mesh, including:

 •    Inflation for resolving the mesh in near wall regions
 •    Controls for mesh refinement
 •    Proximity for detecting edges and surfaces during mesh refinement
 •    Parallel mesh generation for volume meshes

The following topics are covered in this chapter:
 Overview of the Meshing Process
 Mesh Adaption

Overview of the Meshing Process
The steps to create a mesh are as follows:

 1.    Create the Geometry (p. 1)
 2.    Define the Regions (p. 1)
 3.    Define the Mesh Attributes (p. 2)
 4.    Generate the Surface Mesh (p. 2)
 5.    Generate the Volume Mesh (p. 3)

Create the Geometry
You can create geometry for CFX-Mesh from scratch in the DesignModeler application within ANSYS Work-
bench, or import it from an external CAD file. CFX-Mesh requires you to construct Solid Bodies (not Surface
Bodies) to define the region for the mesh. A separate Solid Body must be created for each region of interest
in the CFD simulation: for example, a region in which you want the CFD solver to solve for heat transfer
only must be created as a separate Solid Body. Multiple Solid Bodies are created in DesignModeler by use
of the Freeze command; see Freeze in the DesignModeler Help for more details.

There are some restrictions on the topology of your geometry. These are described in "Geometry" (p. 25).

Define the Regions
During the CFD simulation setup, you will need to define boundary conditions where you can apply specific
physics. For example, you may need to define where the fluid enters the geometry or where it leaves. Although

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               1
What is CFX-Mesh?

it would be possible to select the faces that correspond to a particular boundary condition in CFX-Pre, it is
rather easier to make this selection in CFX-Mesh. In addition, it is much better to define the location of
periodic boundaries before the mesh is generated to allow the nodes of the surface mesh to match on the
two sides of the periodic boundary, which in turn allows a more accurate CFD solution. You can define the
locations of boundaries by creating Composite 2D Regions in the appropriate locations from within CFX-
Mesh.

      Note

      Refer to Named Selections and Regions for CFX Applications under the Meshing Help in Workbench
      for important information about region definitions.


Define the Mesh Attributes
The mesh generation process in CFX-Mesh is fully automatic. However, you have considerable control over
how the mesh elements are distributed. In order to ensure that you get the best CFD solution possible with
your available computing resources, you can dictate the background length scale and where and how it
should be refined. In general, setting up the length scale field for your mesh is a three-step process, as
outlined below:

 1.   Assign a suitable background length scale by setting Body Spacing (p. 63).
 2.   Override the background length scale locally on faces and the regions close to them by setting Face
      Spacing (p. 64), Edge Spacing (p. 65), and Proximity (p. 84).
 3.   Override (1) and (2) locally where necessary using Mesh Controls.

In many simple cases, the need for mesh controls is removed by appropriately setting the local face mesh
spacings, edge proximity, and surface proximity. These controls can be used in isolation, or in combination.
Inflation is used to control the near-wall internal mesh distribution.

CFX-Mesh uses all the current Mesh Control settings to determine the appropriate size of the mesh in a
particular region. In general, the element size is determined by the minimum length scale from all Mesh
Controls, the local length scale from surface mesh parameters and global length scale.

Generate the Surface Mesh
The surface mesh will always be generated prior to the volume mesh generation. However, it is often helpful
to explicitly generate at least part of the surface mesh before volume meshing, to view it and ensure that
the chosen length scales and controls will have the desired effect. The surface mesh generation process in-
cludes a mechanism called Inflation (p. 75) that generates prism elements, and a small number of pyramids
as required, near the walls. Inflation is used for resolving the mesh in the near wall regions to capture flow
effects for viscous problems.

The surface mesh can be previewed before generating the volume mesh by using the Preview function.
Preview Groups can be used to view the surface mesh on selected faces or the whole surface mesh can be
generated at any time.

Two surface meshers are available in CFX-Mesh: Delaunay Surface Mesher (p. 87) and Advancing Front (AF)
Surface Mesher (p. 87).




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
2                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Mesh Adaption

Generate the Volume Mesh
The standard volume mesher in CFX-Mesh is the Advancing Front Volume Mesher (p. 88). It enables an
automatic tetrahedral mesh generation using efficient mesh generation techniques, including the use of
parallel mesh generation.

An alternative volume mesher, the Extruded 2D Meshing (p. 90), is available for two-dimensional or simple
extruded meshes.

The volume mesh can be written to a CFX Mesh file (.gtm) or imported into CFX-Pre by connecting a CFX
system to the Mesh cell and updating the Mesh cell. Opening CFX-Pre will automatically import the mesh.
The volume mesh cannot be viewed in CFX-Mesh, but interior mesh viewing capability is available in the
ANSYS Meshing application once the mesh has been generated and committed to the Meshing application
database (.mshdb). See Saving the Volume Mesh (p. 101) for more details.

Mesh Adaption
The ANSYS CFX software enables you to refine your mesh automatically as the solution to your CFD calculation
is obtained. This helps to ensure that a fine mesh is used where the solution is changing most rapidly. The
set-up for Mesh Adaption takes place in the CFX-Pre software, and not in CFX-Mesh. Mesh Adaption can be
used to improve a reasonable solution; it cannot be used to produce good solutions from an initial poor
quality mesh, so you must still generate a reasonable mesh to begin with.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                          3
    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
4                               of ANSYS, Inc. and its subsidiaries and affiliates.
Graphical User Interface




Elements of the CFX-Mesh Interface
The functional elements of CFX-Mesh interface are outlined below.

Interface Element               Description
Main Menu                       The main menu has five top-level menus that provide access
                                to CFX-Mesh features and commands.
Toolbars and Icons              The toolbars and icons are available for easy and quick ac-
                                cess to commands commonly used for meshing operations,
                                graphics manipulation, and viewer setup.
Tree View                       The tree view shows the current state of mesh settings us-
                                ing the symbols.
Details View                    The details view displays the information of the item selec-
                                ted in the tree view. It also enables you to edit the proper-
                                ties of the selected item.



                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               5
Graphical User Interface

Interface Element                Description
Graphics window                  The graphics window displays the geometry model of an
                                 item selected in the tree view.
Message Window                   The message window provides the feedback related to the
                                 meshing operations in the form of Errors, Warnings, and In-
                                 formation messages.

Status Bar
The status bar displays the information on meshing operations. During the execution of meshing operations,
the status bar displays the progress of the current operation and details of any unread error and warning
messages.

Online Help
Online help for CFX-Mesh is available under the Help menu. Also note that while using the software, pressing
the F1 key over the Tree View or Details View in CFX-Mesh will bring up relevant topic using the context-
sensitive help.

Main Menu

 File Menu
 Tools Menu
 View Menu
 Go Menu
 Help Menu

File Menu
The File menu contains the following items:

      File > Save                                           Saves the current project. The filename and location
                                                            can be seen in the Files view under ANSYS Work-
                                                            bench.
      File > Commit Mesh                                    Commits the generated mesh to the Workbench
                                                            project. By default, this happens automatically when
                                                            generating a mesh, but for large (potentially slow)
                                                            cases, you can set an option not to commit the
                                                            mesh to the Workbench project and choose to
                                                            manually commit the mesh.

                                                            You can change the default setting under Meshing
                                                            > CFX-Mesh Options > Volume Mesh > Commit
                                                            Mesh to Workbench project on Generate using
                                                            the Tools > Options menu. See Volume Mesh (p. 105)
                                                            under CFX-Mesh Options for more details.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
6                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Tools Menu


                                                                      Note

                                                                      The mesh settings are committed to the
                                                                      Workbench project file dynamically; the
                                                                      commit operation is purely for the gen-
                                                                      erated volume mesh.


      File > Export CCL...                                   Exports the current mesh settings as a CCL file. This
                                                             is further described in Exporting the Mesh Settings
                                                             as CCL (p. 7) (see below).
      File > Clear Settings                                  Clears all the user-defined settings from the CFX-
                                                             Mesh database by reinitializing the database. This
                                                             is equivalent to starting a new CFX-Mesh database
                                                             with the same geometry, but is quicker since the
                                                             geometry does not need to be re-imported.
      File > Revert Settings to Saved                        Reverts the settings to how they were when you
                                                             last saved the CFX-Mesh database.
      File > Close CFX-Mesh                                  Closes CFX-Mesh leaving the Meshing application
                                                             open.

Exporting the Mesh Settings as CCL
CCL is the ANSYS CFX Command Language. It is used in CFX-Mesh to encapsulate the mesh settings. One
of the uses of CCL in ANSYS CFX software is to specify the physical model setup for the ANSYS CFX Solver.
CFX-Mesh allows you to export the mesh setup as a CCL file. This would be useful if you wanted a summary
of the mesh settings in a readable format.

Tools Menu
The Tools menu contains the following items:

      Tools > Rotate                                         See Graphics Interaction Tools for details.

      Tools > Mouse Pan

      Tools > Mouse Zoom

      Tools > Box Zoom

      Tools > Zoom to Fit

      Tools > Pick Vertex                                    These functions are identical to Selection Filters
                                                             toolbar.
      Tools > Pick Edge

      Tools > Pick Region

      Tools > Pick Face

      Tools > Pick Body




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                       7
Graphical User Interface

      Tools > Options                                       Sets preferences both for CFX-Mesh and ANSYS
                                                            Workbench. See "CFX-Mesh Options on the Options
                                                            Dialog Box" (p. 103) for more details.

View Menu
The View menu contains the following items:

      View > Shaded Display with 3D                         These functions toggle the geometry display
      Edges                                                 between a view with shaded faces and a view with
      View > Wireframe Display                              just the wireframe outline. This setting is not stored
                                                            in the CFX-Mesh database but is a property of the
                                                            ANSYS Workbench session; that is, if you open a
                                                            different CFX-Mesh database within the same ANSYS
                                                            Workbench session, the setting persists.

                                                            You can change the default view type by setting
                                                            View under Assembly Display (p. 103) using Tools >
                                                            Options menu.
      View > Show Triad                                     These functions are identical to Display toolbar.

      View > Show Ruler

      View > Show Mesh Edge Length

      View > Restore Original Window                        Restores the original layout of the Details View, Tree
      Layout                                                View, and Graphics window.

Go Menu
The Go menu contains the following items:

      Go > Update Geo-             These functions are identical to Geometry toolbar.
      metry
      Go > Verify Geo-
      metry
      Go > Generate Sur-           These functions are identical to Meshing toolbar.
      face Meshes
      Go > Generate
      Volume Mesh

Help Menu
The Help menu contains the following items:

Help > CFX-Mesh Help                              Displays the online documentation on CFX-Mesh
                                                  located under the ANSYS Workbench Help.
Help > About CFX-Mesh                             Provides information on copyright, software build
                                                  date, and service pack version.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
8                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                       Mouse Actions and Model Manipulation

Using the Context Sensitive Help
You can also access the CFX-Mesh documentation by pressing the F1 key over Tree View or Details View to
bring up the online help at a relevant page. See Using Help for the detailed usage instructions and keyword
search.

Toolbars and Icons
Toolbars are displayed across the top of the window, below the menu bar. Toolbars can be docked to your
preference. The layouts displayed are typical. You can double-click the vertical bar in the toolbar to automat-
ically move the toolbar to the left.

The following toolbars are available in CFX-Mesh:

•   File Toolbar (p. 9)

•   Graphics Interaction
    Tools (p. 9)

•   Selection Filters (p. 13)

•   Selection Mode Tool-
    bar (p. 14)

•   Display Toolbar (p. 14)

•   Geometry Toolbar (p. 15)

•   Meshing Toolbar (p. 16)

•   Interrupt (p. 16)


File Toolbar

The File toolbar reproduces some of the functionality from the File menu.

       Clear Settings                                    See File Menu for details.

       Revert Settings to Saved

       Save File

       Commit Mesh


Graphics Interaction Tools
Mouse Actions and Model Manipulation




                          Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                      of ANSYS, Inc. and its subsidiaries and affiliates.                                9
Graphical User Interface

The following table outlines the default actions of mouse buttons and keyboard presses over the Graphics
window in CFX-Mesh. In some cases, holding down the Shift or Ctrl key while using the mouse also changes
its behavior.

                                            No Keypress                     Shift                      Ctrl
Left Mouse Button Click only                Single Select (using Selection tools), or
                                            Selects or restores the center of rotation in
                                            a Rotate mode
Left Mouse Button Click and                 Flood Select or Box Select (using Selection
Drag                                        tools), or
                                            Used for Model manipulation; see the behavi-
                                            or outlined under Tools for Model Manipula-
                                            tion.
Middle Mouse Button Click and                    Rotate                    Zoom                        Pan
Drag
Right Mouse Button Click and                                            Box Zoom
Drag
Mouse Wheel (if available)                                                 Zoom

You can also assign a different function to the mouse buttons by changing the settings under Common
Settings > Graphics Interactions in the Workbench Options.

Tools for Model Manipulation
The left mouse button is used both for selection and for model manipulation. Its behavior is determined by
whether a selection filter                           or graphic manipulation tool                                              is selected from the
Graphics toolbar, as shown below.

                                                                                Rotate mode is selected; see rotation cursors.

                                                                                Face Selection mode is selected; see Selection
                                                                                Filters.

The following table outlines the functions available for model manipulation using the left mouse button.

      Rotate               Activates rotational controls based on the position of the mouse cursor.

      Pan                  This function enables you to move (translate) the model about the display
                           screen as you move the cursor.
      Zoom                 This function enables you to zoom in on the model by dragging the mouse
                           cursor vertically toward the top of the graphics window, or zoom out by
                           dragging the mouse cursor vertically toward the bottom of the graphics
                           window. The center for the Zoom is the same as the center of rotation,
                           which can be set while in a Rotation Mode.
      Box Zoom             This function enables you to drag a box over the model in order to zoom
                           in to that area, which is expanded to fill the window.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
10                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                       Center of Rotation

      Zoom to Fit            This function zooms in or out from the model to fit the entire model in
                             the graphics window.


     Tip

     Use Triad (p. 15) at the bottom right corner of the Graphics window to quickly put the model
     into a desired viewing position.


Rotation Cursors in the Rotate Mode

The model can be rotated in Rotate mode        by holding either left or middle mouse button, and dragging
the mouse. The following table outlines the types of rotation cursors available to rotate the model.

        Free rotation.

        Rotation around an axis that points out of the screen (roll).

        Rotation around a vertical axis relative to the screen (“yaw” axis).

        Rotation around a horizontal axis relative to the screen (“pitch”
        axis).

Position of the Cursor
The type of cursor that is shown, and hence the type of rotation, depends on the starting location of the
cursor in the Graphics window. In general, if the cursor is near the center of the graphics window, the famil-
iar 3D free rotation occurs. If the cursor is near a corner or edge, a constrained rotation occurs: pitch, yaw
or roll.

Specifically, the circular free rotation area fits the window. Narrow strips along the edges support pitch and
yaw. Corner areas support roll. The following figure illustrates these regions.




Center of Rotation
A small red sphere in the middle of Graphics window indicates the center of rotation and it is available only
in Rotate mode     . While in Rotate mode, you can set the center of rotation by clicking over the model
with the left mouse button. This repositions the model relative to the red sphere, keeping the red sphere
in the middle of Graphics window.




                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                     of ANSYS, Inc. and its subsidiaries and affiliates.                                              11
Graphical User Interface

To restore the center of rotation to the model center, left-click some location in the Graphics window that
is away from the model. This re-centers the model by moving it in the middle of Graphics window.

Selection Tools

Many objects in the meshing definition need to be applied to a particular piece of geometry (such as a face)
or to be associated with another item (for example, a Point Control needs to be associated with a particular
Spacing Definition).

Selection in the Tree View
The objects can be selected in the Tree View (p. 17) as outlined below:

 1.       Click in the box in the Details View (p. 21) that requires the selection to make it active. This step may
          not be needed if Auto Activate is set to Yes and there is no valid selection already made.
 2.    Click on the item in the Tree View to select it.
 3.    Click on the Apply button in the relevant box in the Details View. The Graphics window displays the
       selected item in red color.

Selection in the Graphics Window
The process for selecting a geometric object from the Graphics window is similar to selection in Tree view.
The following points apply to selection in general:

 •    Highlighting: provides a visual feedback about the current pointer behavior (e.g., face selection mode)
      and location of the pointer (e.g., over a particular face). The boundary of highlighted object is shown
      in red color.
 •    Picking: clicking on visible geometry picks the selected object, replacing the previous selections. The
      object and its boundary are shown in green color. The selected items turn red after clicking Apply in
      the Details View.
      –     Use the left mouse button to select a single object.
      –     Hold down the Ctrl key on the keyboard to select a second or subsequent item.
      –     To remove an item from the selection, hold down the Ctrl key and select it again.
      –     To select multiple items at once, see Selection Mode Toolbar (p. 14).
      –     If you have faces in the Graphics window that are hidden behind other faces, then when you click
            on the front face, a stack of Selection Rectangles (shown below) will appear at the bottom left of the
            Graphics window. The rectangles are stacked in appearance, with the topmost rectangle representing
            the visible (selected) geometry and subsequent rectangles representing geometry hit by a ray normal
            to the screen passing through the pointer, front to back. The front face will be selected by default.
            You can deselect and/or select any of the hidden faces by clicking on the corresponding rectangles
            instead of the actual faces in the geometry, using the Ctrl key in the same way as for picking directly
            from the geometry. When multiple Solid Bodies with shared faces are present in the geometry, then
            the shared faces are represented by two linked rectangles, one for each side of the face or “2D Re-
            gion”.




                          Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
12                                                    of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                      Vertex Selection

      –    Sometimes you may want to select both objects from the Tree View and faces from the Graphics
           window - for instance, if you wish to apply Inflation (p. 75) to a set of faces that can be selected
           most conveniently by selecting a Composite 2D Region and then adding a few faces selected directly
           from the Graphics window. In this case, selecting the objects of the two different types acts inde-
           pendently. For instance, if you have selected a Composite 2D Region, you can simply click on a face
           in the Graphics window to add it to the selection, without holding down the Ctrl key. If you click
           on a face in the Graphics window (without holding down a key) then that will add that face to the
           selection and clear any existing selection of faces, but not affect any selection of Composite 2D Re-
           gions. If you want to clear the selection of Composite 2D Regions as well, you must explicitly deselect
           them (by holding down Ctrl and clicking on them).
 •    Usually, if you are required to select geometric objects of a particular type, then your selection will be
      automatically restricted to select the objects of the required type only. For instance, when selecting
      face to apply a Face Spacing to, then only faces will be allowed for selection. If the selection is not being
      restricted automatically but you want to enforce a restriction, then you can use a Selection Filter.

Selection Filters


When you activate a Selection Filter, your selection is restricted to the items of a particular type only, as
outlined below:

          Point                      Allows only points to be selected.

          Edge                       Allows only edges to be selected.

          Region                     Allows only regions to be selected.

          Face                       Allows only faces to be selected.

          Body                       Allows only bodies to be selected.


Point Selection
When you need to select a point from the Graphics window, then in general you can select either a model
vertex (corner of a face), an arbitrary point on any of the model faces, or specify coordinates. The following
sections outline the necessary steps for point selection.

Vertex Selection
 1.    If the Point entry in the Details View shows the word “None” on a yellow background, or some coordin-
       ates are displayed, then click on None or the coordinate entry, to make the Point entry change to
       show two buttons, Apply and Cancel.
 2.    Move the mouse over the required vertex in the Graphics window until a small red square appears
       (see the picture below). While the square is visible, click with the left mouse button.




 3.    Click on Apply in the Details View. The Point entry will now show 1 Vertex.




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                            13
Graphical User Interface

Point on a Face
 1.        If the Point entry in the Details View shows the word “None” on a yellow background, or some coordin-
           ates are displayed, then click on None or the coordinate entry, to make the Point entry change to
           show two buttons, Apply and Cancel.
 2.        Move the mouse over the part of the face in the Graphics window where you want the point to be,
           and click with the left mouse button.
 3.        If there is more than one face under the mouse at the point when you click, then the Selection Rect-
           angles will appear in the bottom left-hand corner of the Graphics window. If you click on one of these,
           you can move the point so that it appears not on the face closest to you, but one of the faces under-
           neath the mouse that is not at the front. In order to see the location of the point at this stage, you
           will need to make the geometry partially transparent.
 4.        Click on Apply in the Details View. The Point entry will now show the coordinates of the point that
           you picked. Note that these coordinates now specify the point, so if the geometry changes (from a
           geometry update), it is possible that this point may no longer lie on a face.

Specifying the Coordinates
 1.        If the Point entry in the Details View shows two buttons reading Apply and Cancel, click on Cancel
           to make the Point entry show the word “None” or show some coordinates.
 2.        Right-click on None or the coordinate entry and choose Edit.
 3.        Edit the coordinates as required. The only allowed formats are three numbers (X, Y, Z) separated by
           either spaces or commas (you can not use a comma to separate two numbers and only a space to
           separate the third number). You must not enter the units string (such as “[mm]”); CFX-Mesh will add
           that in for itself using the model dimensions. Press Return on the keyboard to finish editing the co-
           ordinates.

Selection Mode Toolbar

      or

There are two selection modes: Flood Select and Box Select. To switch between them, you use the Selection
Mode toolbar, which is located along with the rest of the toolbars at the top of the window.

 •        Flood Select - In this mode, you can select multiple geometric objects simply by pressing and
       holding down the left mouse button and then moving the mouse over them. Any object that the mouse
       touches is added to the selection.
 •        Box Select - In this mode, you can select geometric objects from the Graphics window by clicking
       with the left mouse button and then dragging it across other objects. All the objects that the box fully
       encloses are selected. If you hold down the Ctrl key while you draw the box, then these items will be
       added to the current selection.

Note that with both selection methods, any faces or bodies that are hidden or suppressed cannot be selected.
The faces or bodies must be made visible in the model view in order that they can be selected.

Display Toolbar

The Display toolbar controls what is visible in the Graphics window.


                          Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
14                                                    of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Geometry Toolbar

      Show Triad                   Toggles the display of the Triad (p. 15).

      Show Ruler                   Toggles the display of the Ruler (p. 15).

      Show Mesh Edge               Toggles the display of the Mesh Edge Length Display (p. 15).
      Length

Triad




The Triad in the bottom right corner of the Graphics window shows the orientation of the model. It can also
be used to position the model in one of several predefined viewing positions:

 •   Click on one of the arrows along the axes to put the model into a view normal to that arrow.
 •   Click on the cyan ball to put the model into an isometric view.

Moving the mouse over the Triad identifies the axis (X, Y, Z) and direction (+/-) of the arrow, using tool tips.
Positive-direction arrows are labeled and color-coded. Negative direction arrows display only when you
hover the mouse cursor over the appropriate region, but can still be clicked on to put the model in a view
normal to the arrow.

To control whether the Triad is visible or not, use the Display Toolbar (p. 14).

Ruler



You can use the ruler, shown at the bottom of the Graphics window, to obtain a good estimate of the scale
of the displayed geometry.

To control whether the Ruler is visible or not, use the Display Toolbar (p. 14).

Mesh Edge Length Display




The Mesh Edge Length display, shown at the top of Graphics window, gives an indication of the relative
mesh length scales for the following cases:

 •   On inflated boundary - The display shows the inflated mesh element height
 •   On mesh spacing - The display shows the Min/Max element size

To control whether the Mesh Edge Length display is visible or not, use the Display Toolbar (p. 14).

Geometry Toolbar


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                            15
Graphical User Interface

The Geometry toolbar gives you access to the actions that can be performed on the geometry.

      Update Geometry                           This enables you to re-import the geometry after it
                                                has been changed, keeping as many of the mesh
                                                settings applied as possible. See Geometry Up-
                                                date (p. 25) for more details.
      Verify Geometry                           See Geometry Checking (p. 41) for more details.


Meshing Toolbar

The Meshing toolbar gives you access to the meshing actions that can be performed on the model.

      Generate Surface Meshes                               This enables you to generate or regenerate the
                                                            surface mesh. You must use a Preview Group (p. 97)
                                                            to view the mesh in CFX-Mesh.
      Generate Volume Mesh                                  This enables you to generate or regenerate the
                                                            volume mesh and write a CFX Mesh file. See Gener-
                                                            ating the Volume Mesh (p. 101) for more details.

Interrupt


Sometimes you may want to interrupt a lengthy meshing operation before it finishes, perhaps because you
realize that you have made a mistake, or that the resulting mesh is going to take too long to generate or
will be too big. In this case, you can use the Interrupt (or “Halt current processing”) button. This is located
in the CFX-Mesh toolbar near the top of the ANSYS Workbench window.

Clicking on the Interrupt button will interrupt any meshing operation in progress (including the Verify
Geometry functionality). After a short delay, CFX-Mesh will return an error showing that the meshing oper-
ation has failed, and an Error will appear in the Messages Window (p. 22) that shows that the meshing has
terminated because you have interrupted it. The user interface is then unlocked for use again.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
16                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Tree View


Tree View




The Tree View, located towards the top left of the CFX-Mesh window, shows the current state of the mesh
settings. The symbols to the left of each item's name are called Status Symbols and show the state of that
particular item; their meanings are listed in the table below.

 •   To delete an item from the tree, right-click on its name and select Delete from the context menu that
     appears.
 •   To rename an item, right-click on its name and select Rename from the context menu that appears.
     Any name must start with an alphabetic character, can be any length and can contain alphabetic char-
     acters, numbers and single spaces.
 •   To change the settings of an object, left-click on its name and then edit the information in the Details
     View (p. 21) below.
 •   A plus symbol to the left of an item's icon indicates that it contains associated sub-items. Click on the
     plus symbol to expand the item and display its contents.
 •   To collapse an item, so that none of its sub-items are visible in the tree, click on the minus symbol to
     the left of the item's icon. To collapse all expanded items at once, double-click the Model name at the
     top of the tree.
 •   To insert a new sub-item, right-click on the item and select Insert from the context menu that appears.
     Some items are only allowed to appear once (e.g., Inflation, Stretch).
 •   To view all the items of a particular type, select the entry in the Tree View that contains them. The items
     will then be highlighted in the Graphics window. For example, to view all Virtual Topology, click on the
     Virtual Topology heading in the Tree View. All Virtual Topology entities (Virtual Faces and Virtual Edges)
     will then be highlighted.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                     17
Graphical User Interface

     For Regions and Spacings, there is a slight exception to this general rule. If you click on the Regions
     heading in the Tree View, all Composite 2D Regions are highlighted except for the Default 2D Region.
     If you click on the Spacing heading in the Tree View, all Face and Edge Spacings are highlighted except
     for the Default Face Spacing. The Default 2D Region and Default Face Spacing are excluded as these
     contain all the faces that are not otherwise assigned explicitly to a user-defined Composite 2D Region
     or a user-defined Face Spacing; if they were included then the whole model would be highlighted when
     either of these headings were selected.
 •   Several items are in the tree by default when the meshing database is created, and these cannot be
     deleted or renamed. They include Region (with the Default 2D Region), Preview, Spacing (with the two
     default spacing objects), Controls, Periodicity, Inflation, Stretch, Proximity and Options.

Status Symbols
Next to each item in the Tree View is a small symbol, known as a “Status Symbol” that gives you information
about the status of that item. If there is no symbol next to an item, then it is in a valid state. The description
of these symbols is given in the table below.

Basic      Description                                                          Hidden Sym-                  Suppressed              Preview
Sym-                                                                            bols a                       Symbols b               Group Sym-
bols                                                                                                                                 bols c
           An item without any symbol is valid.                                                              The item and
                                                                                                             its status sym-
                                                                                This symbol in-              bol become              This symbol
                                                                                dicates that                 gray on sup-            indicates that
                                                                                the Region is                pressing.               the Preview
                                                                                valid and hid-                                       Group is valid
                                                                                den.                                                 and hidden.
           Check mark: Everything is valid but the
           item has been automatically updated by
           CFX-Mesh and it is recommended to verify
           the changes.

           Example: This may occur if you have per-
           formed a geometry update that has resul-
           ted in a face that no longer exists. If that
           face was being used in the location list for
           any mesh feature, then it will be removed
           automatically as part of the update and
           CFX-Mesh marks the affected mesh feature
           with this status symbol.
           Padlock: Everything is valid but the item is
                   ,
           “locked” i.e., editing of this feature is restric-
           ted in some way. In general, items which are                         Example: The
           locked cannot be deleted, and most cannot                            Default 2D Re-
           be renamed or have their locations changed.                          gion is given
                                                                                this symbol
                                                                                when it cannot
                                                                                be deleted or
                                                                                renamed.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
18                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                         Suppressing Objects

Basic        Description                                                            Hidden Sym-                  Suppressed                Preview
Sym-                                                                                bols a                       Symbols b                 Group Sym-
bols                                                                                                                                       bols c
             Exclamation: This means that there is
             something invalid about the definition of
             the item or one of its sub-items that will                                                          This symbol
             also be marked with the same symbol. Of-                                                            indicates that
             ten this will be because no required selec-                                                         the item is
             tion has been made.                                                                                 suppressed
                                                                                                                 and will be
                                                                                                                 invalid when
                                                                                                                 it is unsup-
                                                                                                                 pressed.
             The item is locked and invalid. You must make the item valid before you can mesh again. In
             the case of a locked Virtual Edge, all you can do is do is delete it; in most other cases you must
             edit the location list to make it valid.

             See the description of the locked symbol                              above.
             This symbol indicates that an item contains associated sub-items. Left-click on the symbol to
             expand the item and display its contents.
             This symbol indicates that an item contains associated sub-items. Left-click on the symbol to
             collapse the item so that none of its sub-items are visible in the tree.
a
  Hidden Symbols: They apply to Regions when an item has been hidden in the Graphics window. As such, the item cannot be selected in
the Graphics window; however, the item is not suppressed and will still be meshed (although the mesh can be displayed on the item only
when the item is visible in the viewer).The symbols are paler versions of the basic symbols and their meanings correspond.
b
  Suppressed Symbols:The item and its status symbol become gray on suppressing.The suppressed item becomes inactive and is not included
in the mesh.You must unsuppress an object before you can edit or delete it.
c
  Preview Group Symbols:They apply to Preview Groups when the mesh has not been generated or the generated mesh is out-of-date, i.e.,
it does not reflect the current mesh settings.To generate an up-to-date mesh for the Preview Group, right-click over its name and select
Generate This Surface Mesh.To generate an up-to-date mesh on all Preview Groups, right-click Preview in the Tree View and select Gen-
erate All Surface Meshes.


Suppressing Objects
Items in the Tree View can be suppressed. This means that they become inactive. For instance, if you had
set up an Inflated Boundary, but wanted to try generating the mesh without it, then you could suppress
the Inflated Boundary, generate the mesh, and then, if required, simply unsuppress it to make it active again
with the same settings as before.

Most items can be suppressed, including Inflated Boundaries, Face Spacings and Controls. You can also
suppress higher-level objects. For example, you could suppress the entire Inflation entry to turn off Inflation,
or suppress the entire Controls entry to suppress all of the Controls.

      Note

      Suppressing geometry (Parts or Bodies) hides them from the Graphics window and stops them
      from being included in the mesh. More details on how this affects the resulting mesh is given in
      Suppression of Bodies and Parts (p. 45).




                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                       of ANSYS, Inc. and its subsidiaries and affiliates.                                               19
Graphical User Interface


     Note

     Geometry that has been suppressed in the Meshing application, will appear as unsuppressed in
     CFX-Mesh - if you wish to exclude this geometry from the meshing process, you must suppress
     it from within CFX-Mesh.

A suppressed object still shows in the Tree View, but its Status Symbol will become gray to indicate its status.

You must unsuppress an object before you can edit or delete it.

Items are suppressed by right-clicking on their names in the Tree View, and selecting Suppress. To unsuppress,
right-click again and select Unsuppress.

In addition to Suppress and Unsuppress, you can also Suppress All (when multiple entities exist), Unsup-
press All (when multiple entities exist), as well as Invert Suppression, which inverts the state of the sup-
pression for each entity at the same level in the Tree View.

Hiding Objects
Items in the Region section and Bodies in the Geometry section of the Tree View can be hidden. This means
that they are not displayed in the Graphics window.

A face or edge that is part of Composite 2D Region or Body that is hidden cannot be selected; however,
hiding an item does not exclude it from the meshing process and if, after meshing, the status of an item is
changed from hidden to shown, the mesh can be displayed.

     Note

     If you suppress geometry (Parts or Bodies) rather than hiding it, then this hides the geometry
     from the Model View and stops it from being included in the mesh. More details on how this affects
     the resulting mesh is given in Suppression of Bodies and Parts (p. 45).

A hidden object still shows in the Tree View, but its Status Symbol will become a pale color to indicate its
status.

Items are hidden by right-clicking on their names in the Tree View, and selecting Hide. To show again, right-
click again and select Show.

In addition to Hide and Show, users can also Hide All (when multiple entities exist), Show All (when multiple
entities exist), as well as Invert Visibility, which inverts the state of the visibility for each entity at the same
level in the Tree View.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
20                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Details View


Details View




The Details View is found to the bottom left of the CFX-Mesh window. It contains all of the available inform-
ation for any item in the Tree View (p. 17). You can access it by clicking with the left mouse button on the
item's name in the Tree View.

Details that are grayed out cannot be edited, but most can be edited by simply clicking in the relevant box
and typing. Press Enter on the keyboard after typing in a box to make the change take effect, or simply
move the cursor out of the box.

You can change the name of an item by right-clicking on its name in the Tree View. This is not available
through the Details View.

Where a box requires you to make a selection, you can do this either by picking items from the Graphics
window (where appropriate) or through the Tree View directly. Selection is explained in Selection Tools (p. 12).

Most of the parameters and settings that require you to enter a number will only take numbers within a
certain range. See Valid and Invalid Parameter Values (p. 109) for more details on valid ranges.

Selections of locations must satisfy the rules for the objects that you are trying to create. If you try to make
a selection that is invalid, then the selection will not be accepted. Some notes on valid selections are given
under the section that describes the feature that you are creating, and some notes for the case where you
have multiple Bodies in your geometry are in 2D Regions and Faces (p. 57).

To minimize the number of mouse clicks required to select a Location for any CFX-Mesh Model feature, the
Location selection is made active when you first create that feature (e.g., Inflated Boundary, Preview Group,
Composite 2D Region). For example, this means that you can create a new Inflated Boundary and then im-
mediately click in Graphics window to select the faces for it, without having to first activate the Location
selection by clicking in the Details View.

In general, if you select an object in the Tree View, the Location selection for the first item that does not
already contain a valid selection is activated.

If you prefer not to have the Location selection being automatically activated, then you can set the CFX-
Mesh option Auto Activate to No, under Properties View Options. The CFX-Mesh options and how to set
them are described in CFX-Mesh Options.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                        21
Graphical User Interface


Graphics Window




The Graphics window forms the largest section of the CFX-Mesh window, and is the place where the model
is displayed. It also shows the Ruler (p. 15) and the Triad (p. 15), the axes in the bottom right corner. How
to move the model around and put it into selected views is described in Graphics Interaction Tools (p. 9).

Messages Window




The Messages window displays any messages that have been produced by the meshers or the CFX-Mesh
user interface. The window is visible only when one or more messages are recorded by CFX-Mesh. The
window is split into a display section and a list section. The list displays all those messages currently recorded
by CFX-Mesh.

Types of Messages
The messages are broadly split into two types: Meshing messages and User Interface messages. Once a
message has been selected, the full body of the message can be read. The message is then grayed out to
indicate that it has been read.

Meshing messages are automatically marked as read when any meshing operation is performed (Verify
Geometry, Generate Surface Meshes, Generate Preview Mesh, Generate Volume Mesh). This enables you to
clearly see those messages that were produced from the last meshing operations. This behavior does not
apply to User Interface messages, which must be explicitly read by clicking in the message window.

In addition, the status bar displays an overview of the currently unread messages by displaying the count
of the warnings and errors that have not been read.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
22                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                 Operations Using the Messages Window


    Note

    The Information messages are not considered critical; as such, their count is not displayed in the
    status bar.


Operations Using the Messages Window
•   Pressing Delete key on a message will delete it from the recorded list.
•   Pressing t key will toggle between reading formats for the message.
•   Up or Down key can be used for navigation.




                    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                of ANSYS, Inc. and its subsidiaries and affiliates.                               23
     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
24                               of ANSYS, Inc. and its subsidiaries and affiliates.
Geometry
Before using CFX-Mesh, you must have already created the necessary geometry. In ANSYS Workbench, the
geometry handling tools can be accessed from the Geometry cell on the Project Schematic. You can either
create the geometry from scratch in the DesignModeler application or use an existing geometry created in
a external CAD package supported by ANSYS Workbench.

 •   For details on how to use the Geometry cell to import, create, edit or update the geometry model used
     for analysis, see information on the Geometry cell under Types of Cells.
 •   For details on how to use the DesignModeler application to create the geometry within ANSYS Work-
     bench, see the DesignModeler Help.
 •   For a complete list of CAD systems supported by ANSYS Workbench, see CAD Systems.

After importing the geometry for meshing, it is possible to update the modified geometry in CFX-Mesh. This
is described in Geometry Update (p. 25).

Whether the geometry originates from an external import or is created from scratch in DesignModeler, it
must satisfy certain requirements in order that it can be used successfully in meshing. Additionally, you
should bear in mind how you want to use the geometry in the ANSYS CFX software as you create it, because
if you want to model solid domains (e.g., for heat transfer), fluid subdomains (e.g., to specify a resistance
source) or thin surfaces, you will need to create the geometry using multiple Solid Bodies. You will also need
to make sure that each region you need for a boundary condition in ANSYS CFX is available as a separate
face or faces.

CFX-Mesh includes a geometry-checking utility which can be run to check for the presence of certain features
in faces and edges which can cause meshing difficulties.

If the geometry consists of multiple Bodies and/or Parts, then it is possible to choose to mesh the different
Bodies and Parts separately or together, or not at all. This is described in Suppression of Bodies and Parts
(p. 45).

CFX-Mesh also allows you to control the display of geometry in order to see the model more clearly and to
facilitate selection of faces in multiple body geometries.

Geometry Update
After you have imported a geometry for meshing, you may find at some stage that you need to modify it.
For instance, perhaps you made a mistake in the original construction, or you want to update a dimension
or remove a small feature that you do not want to resolve later in your simulation. CFX-Mesh has the capab-
ility to update your geometry while retaining most or all of the settings, depending on the complexity of
the changes made to the geometry, the CAD format and the method of import. Having altered your geometry
either by editing within DesignModeler or by changing a geometry parameter, ensure that the Geometry
cell in Workbench is up-to-date, either by Updating or by Refreshing the cell on the Project Schematic. Then
you can use CFX-Mesh to update the geometry using the Update Geometry button on the toolbar.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               25
Geometry

On import of the new geometry, CFX-Mesh checks to see whether the CAD entities (faces, edges, vertices,
etc.) that were present in the original geometry still exist in the new geometry. It then updates the features
in the Tree View as follows.

 •   If the geometric location for a CFX-Mesh feature (e.g., a list of faces for a Face Spacing) consists entirely
     of geometric entities which no longer exist, then CFX-Mesh marks that feature as invalid by using the
     invalid status symbol . In order to make the model valid again, you must either delete that feature
     or modify it to specify an appropriate location for the feature.
 •   If the geometric location for a CFX-Mesh feature (e.g., a list of faces for a Face Spacing) consists of both
     geometric entities which no longer exist and entities which do still exist, then the non-existent entities
     are removed from the location list. For example, if a Face Spacing is applied to three faces, and after
     the update one of these faces no longer exists, then the Face Spacing will be automatically modified
     so that after the geometry update, it is applied to just the two remaining faces. Where features are
     automatically updated in this way, CFX-Mesh marks them as such by using the status symbol . Where
     you see this symbol after a geometry update, you are advised to check that the feature is applied to
     where you expect it to be. If you want to clear this symbol, simply click on the feature name in the Tree
     View then click next to Location in the Details View and just press Apply without modifying anything.
 •   New faces are automatically added to the Default 2D Region, Default Face Spacing and Default Preview
     Group.
 •   If you perform a Geometry Update after creating Virtual Topology, then the Virtual Topology will con-
     tinue to be applied in its existing locations provided that all of these locations exist. If any of the locations
     no longer exist, then the Virtual entity will be marked as invalid and you will have to remove it or re-
     select its location in order to make the model valid again. If you remove the invalid Virtual entity, but
     then later undo the geometry modification and do the Geometry Update again, the Virtual entity will
     be re-created.

After a geometry update, you should always check that your settings are still applied to their required location.

In order to keep applying existing meshing features to the correct locations, CFX-Mesh needs to be able to
identify a geometric location such as a face as being the same in the old geometry and the new geometry.
How well it is able to do that depends on both the CAD format and the method of import.

If your geometry was created in DesignModeler, then you should find that most geometry updates work
with the minimum required modification to your meshing model. The one exception to this is that if you
combine bodies to form a single part using the Form New Part functionality, or use the Explode Part
functionality to reverse this change. In this case, the underlying faces do not maintain their identity during
the geometry update and you may need to re-apply the locations of all the mesh settings.

If you have used a direct CAD interface in plug-in mode, then once again you can expect that many geometry
updates will work with the minimum required modification to your meshing model. However, if you are
using a CAD interface in reader mode, then it is more difficult to maintain the identities of the geometric
locations during import, and you may find that you have to re-apply the locations of all the mesh settings.

Geometry Requirements
Geometry requirements and how to create certain desired topologies are described in the following sections.
 General Geometry Requirements
 Multiple Bodies, Parts and Assemblies
 Geometry and Topology for Solid Bodies
 Geometry and Topology for the Faces of Solid Bodies
 Geometry and Topology for the Faces of an Inflated Boundary
 Geometry for Thin Surfaces

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
26                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                   Geometry and Topology for Solid Bodies

 Poorly-Parameterized Surfaces
 Degenerate Geometry

General Geometry Requirements
 •   The geometry used for meshing must consist of one or more Solid Bodies which are grouped into one
     or more Parts. Surface Bodies in ANSYS Workbench are not supported. However, on import of certain
     geometry file formats (currently CATIA v5, IGES, Solid Edge and NX, ANSYS Workbench will convert sets
     of surfaces which fully enclose a volume into Solid Bodies, so the requirement to have a Solid Body
     does not restrict the use of these formats.
 •   The use of multiple Solid Bodies is described in Multiple Bodies, Parts and Assemblies (p. 27).
 •   Solid Bodies in a single Part must not overlap each other.
 •   Where Solid Bodies in a single Part touch, they must have common faces if you want a common mesh.
     This is illustrated in Bodies Touching at a Face (p. 28).
 •   It does not matter whether or not the Solid Bodies are Frozen in DesignModeler; they will still appear
     in CFX-Mesh and can be meshed regardless of this state. If you want to exclude a Solid Body from
     meshing, you must suppress it in CFX-Mesh or suppress or delete it in DesignModeler. Geometry that
     is suppressed in the Meshing application will not be suppressed in CFX-Mesh

Multiple Bodies, Parts and Assemblies
 •   Parts are groups or collections of Bodies. Parts can include multiple Bodies and are then referred to as
     Multi-body Parts. If your geometry contains multiple Parts then each Part will be meshed with separate
     meshes with no connection between them, even if they apparently share faces.
 •   You can convert a geometry which has multiple Parts into one with a single Part by using the Form
     New Part functionality in DesignModeler. Simply select all of the Bodies and then use Tools > Form
     New Part. If you have an external geometry file that has multiple Parts that you wish to mesh with one
     mesh, then you will have to import it into DesignModeler first and perform this operation, rather than
     importing it directly into the Meshing application.
 •   By default, every time you create a new Solid Body in DesignModeler, it is placed in a new Part. To
     create a single mesh, you will have to follow the instructions in the previous step to place them in the
     same Part after creation.
 •   Multiple Solid Bodies within a single Part will be meshed with one mesh provided that they have at
     least one face which CFX-Mesh recognizes as being “shared” with another of the Bodies in that part.
     This is the desired topology if you require a single mesh with multiple domains or subdomains in CFX-
     Pre. For a face to be shared in this way, it is not sufficient for two Bodies to contain a coincident face;
     the underlying representation of the geometry must also recognize it as being shared. Normally, geometry
     imported from external CAD packages (not DesignModeler) does not satisfy this condition and so sep-
     arate meshes will be created for each Body, even if they are in the same Part. However, if you have
     used the Form New Part function in DesignModeler to create the Part, then the underlying geometry
     representation will include the necessary information on shared faces when faces are coincident (i.e.,
     the Bodies touch).
 •   An Assembly is a collection of Parts. Multiple Assemblies are not supported.

Geometry and Topology for Solid Bodies
This section shows examples of allowed and disallowed topology for Solid Bodies together with notes on
the methods which can be used to generate them in DesignModeler. The two governing principles are:

 •   Solid Bodies must not overlap.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                 27
Geometry

 •     At the junction of Solid Bodies, they must share a common face if you want a single mesh.

The examples are:
 Bodies Joined by a Common Face
 Bodies Touching at a Face
 Body with a Hole
 Body with an Enclosed Body
 Bodies with an Enclosed Body and a Hole
 Body with an Enclosed Body Touching the Face

Bodies Joined by a Common Face
This example shows a simple configuration with two Solid Bodies which have a common face. Assuming
that they are contained within the same part, one mesh will be produced.




     3D representation             2D representation

The steps to construct this geometry in DesignModeler are outlined below:

 1.     Create a cube and Freeze it.
 2.     Now, create another cube.
 3.     Select both Bodies and combine them into one Part using Tools > Form New Part.

Bodies Touching at a Face
This example shows two Solid Bodies, which meet at a face. A single mesh will be produced throughout the
two Bodies only if they are in the same part and if they share a common face where they touch.

If you just create the two Bodies shown, then they do not meet at a common face: the circle at the end of
the cylinder is not one of the faces of the cube. The picture below shows this situation.




 3D representation         2D representation

In order to make a common face between the two, the cube needs to have the square face that touches
the cylinder split into two: one face is the circle at the end of the cylinder, and the other face is the remaining
square with a circular cut. This is shown in the picture below. Green and black are used to color the faces
of the cube.



                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
28                                                   of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                   Geometry and Topology for Solid Bodies




 3D representation      2D representation

The steps to construct this geometry in DesignModeler are outlined below:

 1.   Create a cylinder.
 2.   Freeze it and make a copy using the Body Operation Copy.
 3.   Now, create a cube.
 4.   Use the Body Operation Imprint Faces, selecting one copy of the cylinder as the Body, to split the
      face of the cube which touches the cylinder into the two required pieces.

      This operation removes one copy of the cylinder, leaving two Solid Bodies, the cube and the cylinder.
 5.   Select both Bodies and combine them into one Part using Tools > Form New Part.

Body with a Hole
This example shows a single Solid Body with a cube-shaped hole.




3D representation     2D representation

The steps to construct this geometry in DesignModeler are outlined below:

 1.   Create the outer cube.
 2.   Use an Extrude operation to create the inner cube, which forms the hole, and set Operation to Cut
      Material.

Body with an Enclosed Body
This example shows two Solid Bodies, one of which is entirely enclosed by the other. It is assumed that you
want to be able to refer to the mesh on the inner Body explicitly, perhaps because you want to model that
region as a conducting solid in your ANSYS CFX simulation. A single mesh will be produced throughout the
two Bodies (provided that they are in the same part) but the mesh on either Body will be available separately
for selection in ANSYS CFX.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                 29
Geometry




3D representation    2D representation

The steps to construct this geometry in DesignModeler are outlined below:

 1.   Create the inner cube.
 2.   Use the Enclosure operation, with Shape set to Box and Merge Parts? to Yes, to create the outside
      cube with the inner cube cut out of it, without removing the inner cube.

This method only works if the outside Body is a cube, sphere or cylinder, since these are the only Bodies
that the Enclosure operation can create directly. If the two Bodies were not just simple shapes, then to create
a geometry with this topology, you could do the following:

 1.   Create the inner Body.
 2.   Freeze it.
 3.   Now, create the outer Body.
 4.   Use the Enclosure operation with Shape set to User Defined, User Defined Body set to the outer
      Body, Target Bodies set to All Bodies, and Merge Parts? to Yes.

In this example, setting Merge Parts? to Yes has the effect of combining the two Bodies into one part
without having to do this explicitly.

The following configuration, in which the outer Body has no hole, is NOT correct:




 3D representation     2D representation

Bodies with an Enclosed Body and a Hole
This example shows two Solid Bodies, one inside the other, with a hole in the center of both. It is assumed
that you want to be able to refer to the mesh on the inner Body explicitly, perhaps because you want to
model that region as a conducting solid in your ANSYS CFX simulation. A single mesh will be produced
throughout the two Bodies (provided that they are in the same part) but the mesh on either Body will be
available separately for selection in ANSYS CFX.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
30                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                  Geometry and Topology for Solid Bodies




3D representation    2D representation

The steps to construct this geometry in DesignModeler are outlined below:

 1.   Create the middle cube that forms the outside faces of the red Body.
 2.   Use the Enclosure operation to create the outside cube with the middle cube cut out of it, without
      removing the inner cube.
 3.   Use an Extrude operation to create the inner cube that forms the hole, setting Operation to Cut Ma-
      terial.
 4.   Select both Bodies and combine them into one Part using Tools > Form New Part.

Once again, this method only works if the outside Body is a cube, sphere or cylinder, since these are the
only Bodies that the Enclosure operation can create. If the two Bodies were not just simple shapes, then to
create a geometry with this topology, you could do the following:

 1.   Create the middle cube that which forms the outside faces of the red Body.
 2.   Freeze it.
 3.   Now, create the outer Body.
 4.   Use the Enclosure operation with Shape set to User Defined, User Defined Body set to the outer
      Body, Target Bodies set to All Bodies, and Merge Parts? to Yes.
 5.   Unfreeze the middle cube and choose to Freeze Others?, to make the middle cube an active Body.
 6.   Use an Extrude operation to create the inner cube that forms the hole, setting Operation to Cut Ma-
      terial.

In this example, setting Merge Parts? to Yes has the effect of combining the two Bodies into one part
without having to do this explicitly.

Body with an Enclosed Body Touching the Face
This example shows two Solid Bodies, one of which is contained by the other but touching at a face. It is
assumed that you want to be able to refer to the mesh on the inner Body explicitly, perhaps because you
want to model that region as a conducting solid in your ANSYS CFX simulation. A single mesh will be produced
throughout the two Bodies (provided that they are in the same part) but the mesh on either Body will be
available separately for selection in ANSYS CFX.




 3D representation     2D representation

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                 31
Geometry

Since the cylinder is not entirely enclosed by the outside Body, you cannot use the Enclosure operation to
make a geometry with this topology. In order to construct this geometry in DesignModeler, you could

 1.   Create a cylinder.
 2.   Freeze it.
 3.   Now, create the outer cube.
 4.   Use the Enclosure operation with Shape set to User Defined, User Defined Body set to the outer
      Body, Target Bodies set to All Bodies, and Merge Parts? to Yes.

In this example, setting Merge Parts? to Yes has the effect of combining the two Bodies into one part
without having to do this explicitly.

The following configuration, in which the cube has no hole, is NOT correct:




 3D representation      2D representation

Geometry and Topology for the Faces of Solid Bodies
The Solid Bodies to be meshed can all be thought of as a volume enclosed by a set of faces. The geometry
and topology of these faces can affect how well the surface meshing process is able to produce a good-
quality surface mesh, so it is important to bear the following considerations in mind.
 Non-Manifold Geometry
 Closed Faces
 Merging Topology

Non-Manifold Geometry
The CFX-Mesh surface meshers are unable to mesh certain face topologies. An example of one such topology
is non-manifold face topology, as shown below. Four faces are associated with one edge: two with the
outer body, and two with the inner body.




The way to work around this particular problem is to split the outer body as shown in the picture below.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
32                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                              Geometry and Topology for the Faces of Solid Bodies




Problems can also arise even if there is no non-manifold edge present but due to a face which has a non-
manifold vertex, as shown below.




Closed Faces
A closed face has two distinct edges which occupy the same location in space. The most common example
of a closed face is a cylindrical face. Both of the two cylinders shown below have a closed face - the curved
part of the cylinder is made up of just one face.




Closed faces are not a problem for the default surface mesher, the Delaunay Surface Mesher (p. 87). However,
they cannot be meshed with the Advancing Front (AF) Surface Mesher (p. 87). If you want to use the Advancing
Front Surface Mesher, then you will have to split the cylindrical face into two parts:




In DesignModeler this can be done as follows, assuming that the cylindrical face was created by Extruding,
Revolving or Sweeping a circle.

 1.   Select the sketch containing the circle, and then use Split from the Modify Toolbox of the Sketching
      tab to divide the circle into two or more distinct edges.
 2.   On the Details View for the Extrude/Revolve/Sweep that created the face, set Merge Topology? to
      No. Then click on Generate to regenerate the cylindrical face.

The second step is required to stop DesignModeler from optimizing the topology of the created face(s),
which would have resulted in this case in DesignModeler still creating a single face, even though the circle
being extruded/revolved/swept was formed of two edges.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               33
Geometry

Merging Topology
CFX-Mesh will create a surface mesh on each individual face. This means that in cases containing very narrow
faces, a small mesh length scale must be used in order to mesh the face. However, this is much finer mesh
than is required to resolve the flow characteristics for the CFD simulation.

In some cases, this may not be avoidable. However, if you are using DesignModeler to generate your geometry,
then you may be able to avoid this situation by setting Merge Topology to Yes when creating the Solid
Bodies in DesignModeler. In summary, this setting allows DesignModeler to optimize the faces created and
in some cases this will result in faces that would otherwise be separate being merged into one face. More
details can be found in the DesignModeler Help under Merge Topology.

CFX-Mesh also allows you to merge two or more faces into one Virtual Face. The surface meshing operation
will then mesh across the Virtual Face rather than the smaller constituent faces, thus removing the requirement
for the mesh length scale to resolve the width of any of these constituent faces. Virtual Faces and their
limitations are discussed in "Virtual Topology" (p. 47).

Geometry and Topology for the Faces of an Inflated Boundary
There is a class of face topologies for which Inflation (p. 75) can be performed, but where the results might
not be what you expect. An example is shown in the picture below.




If you try to perform Inflation with such a topology, you will not get a uniform thickness of inflation near
where the triangular Face A touches the inflation face. Instead, the number of layers of inflation at the point
where Face A meets the inflation face will be reduced to zero; as one moves away from this point, the
number of layers will increase by 1 in successive elements, until it reaches the number of layers that you
requested.

There are two ways of overcoming this problem:

 1.   Redefine the non-inflated faces to be inflated ones. In this case the inflation will cause elements to be
      produced normal to these faces, and the problem does not arise.




 2.   You can edit the non-inflated faces by merging them, and so removing one of the internal edges. One
      way to merge the faces is to make use of the Merge Topology feature in DesignModeler; another way
      is to use the "Virtual Topology" (p. 47) feature in CFX-Mesh.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
34                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                        Geometry for Thin Surfaces




Geometry for Thin Surfaces
Suppose that you are trying to model a geometry which has a very thin feature (for example, a thin sheet
of metal in an enclosure). If you mesh such a geometry as a three-dimensional feature, you would have to
use a very small mesh edge length on the end of the thin protrusion. In ANSYS CFX, you can model this as
a two-dimensional Thin Surface as shown below.




The ANSYS CFX Solver treats each side of the Thin Surface uniquely and computes the flow variables for
both sides separately.

The Thin Surface must be the face of a Solid Body, so to set up a Thin Surface in CFX-Mesh, you must have
more than one Solid Body present in the model, and this must be a consideration when constructing the
geometry. You can also set up a Composite 2D Region which actually forms the Thin Surface boundary
condition for the CFD simulation, if you choose.
 Thin Surface Topology Restrictions
 2D Regions for Thin Surfaces

Thin Surface Topology Restrictions
The following points should be noted when creating geometries with Thin Surfaces.

 •   The Thin Surface must be the face of a Solid Body.
 •   The Thin Surface must have mesh on both its sides. For this reason it is not possible to create a Thin
     Surface that forms part of the external boundary of the model (unless it is embedded into a Periodic
     Pair - see below). Thin Surfaces are allowed to share a vertex or vertices with the model boundary.
 •   Thin Surfaces are allowed to share a vertex or vertices with a face forming a Periodic Pair (p. 73).
 •   If you need to embed a Thin Surface into a Periodic Pair, you must make sure that identical faces are
     embedded into each location of the Periodic Pair. The example below shows one possible configuration.




The following examples demonstrate the use of multiple Solid Bodies to create Thin Surfaces. There is usually
more than one way in which the Solid Bodies can be defined to create the same Thin Surface.
 Example 1: Free Floating Thin Surface
 Example 2: Attached Thin Surface



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                          35
Geometry

Example 1: Free Floating Thin Surface




Key:                                        Solid Body
                                            Solid Body
                                            Desired Thin Surface

In each case, the Solid Bodies have been created in order to put the Thin Surface at the edge of a Solid
Body. They must also satisfy the rules for creating multiple Solid Bodies:

 •     Solid Bodies must not overlap.
 •     Where Solid Bodies meet, they must share a common face.

In each case, the Solid Bodies are contained within the same part. More details on allowed configurations
of Solid Bodies can be found in Geometry and Topology for Solid Bodies (p. 27).

Example 2: Attached Thin Surface




In each case, the Solid Bodies have been created in order to put the Thin Surface at the edge of a Solid
Body. They must also satisfy the rules for creating multiple Solid Bodies:

 •     Solid Bodies must not overlap.
 •     Where Solid Bodies meet, they must share a common face.

In each case, the Solid Bodies are contained within the same part. More details on allowed configurations
of Solid Bodies can be found in Geometry and Topology for Solid Bodies (p. 27).

In addition, for case (1) above, the intersection between the two Solid Bodies must consist of two faces, one
for the Thin Surface and one for the part not in the Thin Surface. To break the face, which forms the inter-
section, you can use Imprint Faces in DesignModeler - see the DesignModeler Help for more details. The
following steps outline the steps to construct this geometry (1) in DesignModeler.

 1.     Create the left-hand body (colored blue),
 2.     Create the thin surface (colored red), perhaps by extruding a sketch containing a single line,
 3.     Use the Body Operation Imprint Faces, selecting the thin surface as the Bodies and turning on Preserve
        Bodies?,
 4.     Freeze the model,

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
36                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                   Poorly-Parameterized Surfaces

 5.   Create the right-hand body (colored green),
 6.   Use the Body Operation Imprint Faces, selecting the thin surface as the Bodies and turning off Preserve
      Bodies?, and
 7.   Select both Bodies and combine them into one Part using Tools > Form New Part.

2D Regions for Thin Surfaces
To create a Composite 2D Region that will be used for a Thin Surface in CFX-Pre, simply create the Composite
2D Region on a face or faces required. After importing the mesh into CFX-Pre, you will find that two regions
will exist - one for each side of the Thin Surface. You must then assign boundary conditions to BOTH sides
to create a Thin Surface.

Poorly-Parameterized Surfaces
Some external CAD packages may allow some control over the type of surfaces which can be created. This
section gives some guidelines which can be applied when using these CAD packages, in order to produce
high-quality surfaces which are the most suitable for meshing. It is intended for advanced users only. You
will need to refer to your CAD package's documentation to find out what control over surfaces it allows.

A four-sided surface is often a parametric surface, that is, it can be thought of as topologically equivalent
to a flat square which has been distorted, as shown below. The position of a point upon the surface can
then be described by the values of two parameters, ξ1 and ξ2, which usually take values in the range 0 to
1.




A poorly-parameterized surface is one where the shape of the surface is distorted so much that this parametric
description of the surface becomes difficult to work with. For example, near the “corners” of the surface, a
small change in actual position on the surface can lead to a very large change in the values of ξ1 and ξ2, or
vice versa.

The parameterization of a surface can affect the quality of the mesh produced on it. For a non-trimmed
parametric surface, the surface mesh is created on a unit square in parametric space. This mesh is then
mapped back to corresponding physical locations on the actual surface. The uniformity of the mapping
between parametric and physical space is an important factor in retaining the quality of the triangulation
in physical space.

Parametric lines are the lines in physical space which map to even straight lines parallel to the edges of the
square in parametric space. By visualizing the parametric lines on a surface, you can gain a qualitative rep-
resentation of the parameterization of a surface; consult your CAD package documentation to see if this is
possible within it. As a guide, the more uniform the distribution of these lines, the better the parameterization
of the surface. Parametric lines should also not meet at very small or very large angles. You can clearly see
that the parametric lines on the circular parametric surface meet at angles very far away from 90 degrees,
when 10 equally-spaced parametric lines are used in the diagram below.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                        37
Geometry




To improve the parameterization of the surface, it may be possible to merge it with another surface to form
a Virtual Face. Alternatively it may be possible to regenerate the surface in the original CAD package. To
identify and fix poorly-parameterized surfaces in the original CAD package, you need to understand how a
surface is represented and how a mesh is created on the surface. One of the simplest examples is a unit
cube. The six planar surfaces which share common edges form a solid enclosing a volume of 1 unit cubed.
Let us assume that the edges of the cube are aligned with the three principle axes (X, Y, Z). The surface
meshing algorithms implemented in CFX-Mesh are, in effect, two-dimensional meshing algorithms, creating
a group of connected planar triangles for each individual planar surface of the cube. Each surface mesh is
then mapped to the physical coordinates of the geometry. For a unit cube it is relatively simple to see how
this mapping takes place. The two-dimensional coordinates map to each side of the cube, so ξ1 and ξ2 directly
replace the x or y or z physical coordinates, as shown in the table and diagram below.




Surface Location    Mapping (ξ1, ξ2) to (x, y, z)
Low X               (0, ξ1, ξ2)
High X              (1, -ξ1, ξ2)
Low Y               (-ξ1, 0, ξ2)
High Y              (ξ1, 1, ξ2)
Low Z               (ξ1, ξ2, 0)
High Z              (ξ1, -ξ2, 1)

The range of ξ1and ξ2 is [0,1] (for a parametric surface) and in the case of a unit cube the coordinates (x, y,
z) also have a range [0,1], so the mappings between ξ1, ξ2 and x, y, z are one-to-one. This is obviously not
the case for all surfaces and geometries, simply stretching the unit cube in the x-direction by scaling the
geometry using the vector (3,1,1) immediately changes the mapping between ξ1, ξ2 and the x-coordinate.
This implies that there is a direct relationship between the parametric and physical coordinates for a surface
and that we need to consider the linearity of the mapping between the two coordinate systems. This is
particularly true in the case of parametric surfaces where we mesh a unit square in parametric space which
is mapped to the related geometrical surface. The following examples demonstrate particular problems:
  Example 1: Distorting the Square
  Example 2: Circle
  Example 3: Uneven Parametric Lines
  Example 4: Degenerate Surfaces
  Example 5: Cusps




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
38                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                   Poorly-Parameterized Surfaces

Example 1: Distorting the Square
(i)




In case (i) it is easy to see that any triangle created in parametric space will be mapped to a triangle in
physical space which possesses the same internal angles.

(ii)




In case (ii), the internal angles of a mapped triangle can be seen to be different, but not by a significant
amount.

(iii)




In case (iii) there is a significant variation in the internal angles and in the case where a triangle is created
at the origin of (ξ1, ξ2) the mapping to physical space does not create a valid triangle. The parametric lines
provide you with guidance with respect to the amount of distortion relating to the parameterization.

Example 2: Circle
The second example is that of a circular parametric surface created from four curves. Near the “corners” of
the surface (where ξ1 and ξ2 are zero, for example), a small change in actual position on the surface can
lead to a very large change in the values of ξ1 and ξ2. The parametric lines are displayed to show the surface
more clearly.




A workaround to this problem is to re-create the surface as some sort of planar surface which is trimmed
by the circle boundary. In some CAD packages you may be able to do this by creating the circle from five
edges rather than four.




Example 3: Uneven Parametric Lines
The uneven distribution of parametric lines can also cause surface meshing problems. This usually occurs
when a surface is generated using a collection of unequally spaced curves. The image below shows the

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                        39
Geometry

distribution of 8 parametric lines on a surface. The parametric lines are equally spaced vertically, however,
horizontally this is not the case. It can be seen that two of the parametric lines are very close together and
this means that when the mesh is mapped from parametric space to physical space the mesh will also be
distorted, as shown in the second image.




Some CAD packages may allow such a surface to be refitted to have a more even distribution of the para-
metric lines. Otherwise the surface will have to be regenerated using a different method or using a collection
of more evenly spaced curves.

Example 4: Degenerate Surfaces
Two examples of degenerate surfaces are shown below:




A degenerate surface occurs when one or more sides of the parametric quadrilateral surface used for
meshing collapse to a singularity.

Degenerate surfaces should be recreated ensuring that the singularity is avoided. More information is given
in Degenerate Geometry (p. 40).

Example 5: Cusps
Another example of a poorly-parameterized surface is shown below. The problem is the sharp point on the
surface (the sharper the point, the more likely it is to cause a problem).




This time, a large change in position may correspond to only a small change in ξ1 and ξ2.

One way to avoid this problem in some CAD packages is to break one of the curves into two pieces, so that
surface has five sides and can no longer be a parametric surface, as shown below. You may also be able to
merge surfaces to form a Virtual Face to eliminate this problem.




Degenerate Geometry
Degenerate entities are those whose length, area or volume degenerate to zero because of the coincidence
of one or more points or vertices.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
40                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Geometry Checking

Although CFX-Mesh can handle some forms of degenerate geometry, you may find that if you try to mesh
degenerate geometry, you may get an error message when the surface or volume meshing operations en-
counter the degenerate geometry entity, and the meshing operation will terminate. Whether the mesher
terminates at the surface meshing or volume meshing stage depends on the type of degeneracy it has en-
countered.

The most common problems with degenerate geometry occur as a result of importing parametric surfaces
and parametric solids which comprise degenerate edges or faces. A parametric surface is a four-sided surface
which is represented as topologically equivalent to a flat square which has been distorted (see Poorly-Para-
meterized Surfaces (p. 37)). A parametric solid is a six-faced solid which is represented as topologically
equivalent to a cube which has been distorted.

Surface Meshing
Surface meshing problems usually occur as a result of the surface mesher trying to mesh a surface of zero
area. This can occur if your imported parametric solid or B-rep solid contains a solid face which has degen-
erated to an edge. Meshing problems will occur if:

 •    during creation of a B-rep solid your original surface list contained a zero area degenerate surface; or
 •    a zero area degenerate face is present in a parametric solid. This can occur if you used a degenerate
      entity to create the solid (e.g., creating a solid prism by extruding with a three-sided triangular parametric
      surface) or you explicitly defined a parametric solid with a degenerate face (e.g., by defining two pairs
      of vertices at the same location).

In both cases, depending upon the CAD package used to create the geometry, the solution could involve
the following steps.

 1.    Disassemble your solid into its constituent surfaces.
 2.    Identify the zero area surface, and delete it.
 3.    Recreate a B-rep solid from the remaining surfaces.

Volume Meshing
Volume meshing problems with degenerate geometry tend to occur when Inflation (p. 75) is used on faces
which are connected to a degenerate edge of a non-inflated face. If Inflation cannot proceed along a non-
inflated adjacent face edge the mesher will fail trying to create inflated elements. The general solution is to
follow the guidelines for Inflation described in Geometry and Topology for the Faces of an Inflated Bound-
ary (p. 34).

Geometry Checking

The geometry checking facility in CFX-Mesh checks for the presence of certain undesirable features in faces
and edges, which can cause the mesher to generate a low quality mesh or to fail to generate a mesh at all.

You can access it by right-clicking on Geometry in the Tree View and selecting Verify Geometry. Alternatively,
it is available from the Meshing toolbar                       .

The results of all of the checks are recorded in the Messages window, located below the Graphics window.
The last message issued by CFX-Mesh gives a summary of the checks:

 Information

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                             41
Geometry


     Summary for CAD quality checking
     ================================


     Sliver edge checking
     --------------------
     Shortest edge 1.877E+00 (Tolerance =                     1.600E-01)

     Sliver face checking
     --------------------
     Worst sliver factor 6.145E+00 (limit =                      2.500E+01)

     Parameterization face checking
     ------------------------------
     Worst parameter 4.587E-01 (limit =                   1.000E+01)

The Messages window also displays other warnings related to particular faces or edges that fail each check.
Clicking on any warning messages related to faces will highlight the corresponding faces in the Graphics
window. If it is difficult to see the highlighted face, you could hide the display of the geometry before
clicking on the error. The part of the model causing the error will still highlight, which should make it much
easier to see. Hiding the geometry (or part of the geometry) can be done by right-clicking on the name of
the Body or Part under Geometry in the Tree View.

Note that a failed check may not necessarily result in a poor mesh, particularly if default tolerances are used.
However, it may be worth checking the mesh on any faces which fail the checks, to ensure that a high-
quality mesh has been achieved.

Also note that these checks will not pick up all problems which can be associated with the geometry; they
only check for a few specific problems. General geometry requirements are described in Geometry Require-
ments (p. 26).

To set the limits and tolerances used to judge when an edge or face has failed the checks, you can use the
Verify Options (p. 43) under Geometry in the Tree View.

The individual checks are described separately:

 •   Sliver Edge Checking (p. 42)
 •   Sliver Face Checking (p. 43)
 •   Parameterization Face Checking (p. 43)

Sliver Edge Checking
Sliver Edge Checking looks for short edges in the geometry. These edges can produce a mesh which is over-
refined in regions near the short edges. A more detailed description and details on how these short edges
can be removed is given in Geometry Fixing: Short Edge Removal (p. 44) and Virtual Edges (p. 51).

The default tolerance given depends upon the size of the geometry. As a general rule of thumb, you should
start by adjusting this so that it is a bit less than the finest mesh length scale that you want to use, so that
you can see regions where short edges will affect the mesh.

Sliver Edge Checking is one of the checks performed when using the Geometry Checking (p. 41) feature. You
can change the tolerance used for the check by using Verify Options (p. 43); valid values for the Short Edge
Limit are anything above zero.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
42                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Verify Options

Sliver Face Checking
Sliver Face Checking computes a ratio of perimeter length to area for each face. This is known as the sliver
factor. Faces with a high sliver factor can result in a poor quality surface mesh. The sliver factor associated
with a face is computed as:



The table below shows some examples of sliver factors that would be computed.

Surface Description                               Sliver Factor
Square                                            1.27
Circle                                            1
Rectangle with sides 10 and 1 units               3.85
Rectangle with sides 100 and 1 units              32.47

When the Sliver Face Check is run, faces with a sliver factor greater than the limit set will be identified as
potential sliver surfaces. The default value of 25 is usually sensible. Each face identified will be highlighted
when the individual warning message is selected.

Sliver Face Checking is one of the checks performed when using the Geometry Checking (p. 41) feature. You
can change the limit used for the check by using Verify Options (p. 43). The Sliver Factor Limit must be
greater than 1.0.

Faces identified that possess an unacceptable sliver factor may be removed by merging them with neigh-
boring faces. More details of this process can be found in Virtual Faces (p. 48).

Parameterization Face Checking
Parameterization Face Checking provides guidance on the parameterization quality of the surfaces. Each
potentially poorly-parameterized surface will be highlighted when the individual warning message is selected.

More details on what is meant by face parameterization is given in Poorly-Parameterized Surfaces (p. 37).

Parameterization Face Checking is one of the checks performed when using the Geometry Checking (p. 41)
feature.

Faces identified as being potentially poorly-parameterized may be removed by using "Virtual Topology" (p. 47)
to merge them with neighboring faces. More details of this process can be found in Virtual Faces (p. 48).
Merging poorly-parameterized surfaces using Virtual Topology changes the underlying parameterization.

Verify Options

The Verify Options item, located under Geometry in the Tree View, allows you to set the tolerances and
limits for the Geometry Checking (p. 41) feature.

The available options are:

 •   Short Edge Limit - This limit is used with Sliver Edge Checking (p. 42). When the check is performed,
     all edges which are shorter than this limit will generate warnings.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                          43
Geometry

 •   Sliver Factor Limit - This limit is used with Sliver Face Checking (p. 43). When the check is performed,
     all faces which have sliver factors greater than the limit will generate warnings.

Geometry Fixing: Short Edge Removal

Sometimes, particularly with imported geometries, there may be some short edges which are part of the
boundary of a face, where the length of the edges is much less than the required mesh spacing in that region
of the geometry. Since the mesher will place a minimum of three points on every edge which makes up a
face, the presence of these short edges will result in some elements that are of the same size as these short
edges, rather than a mesh using the required spacing. This results in an uneven mesh with many more mesh
elements than would have been desired.

To get around this problem, CFX-Mesh allows you to remove short edges. To set this up, use the Fix Options
item under Geometry in the Tree View. The default is NOT to remove any edges.

If you set Remove Short Edges to Yes, then you will be asked for an Short Edge Tolerance (which must be
shorter than the Maximum Spacing set for the Default Body Spacing). All edges shorter than this length will
be ignored by the mesher (although they will still show up in the geometry display) and the two ends will
collapse to a point. You must make sure that the Short Edge Tolerance specified is shorter than the mesh
length scale at any point where edges may be removed, and you must also make sure that removing the
edges does not cause any face to collapse (to give a face with zero area).

The pictures below show the effect of short edge removal. The face shown is a square with sides of 1 m.
However, the bottom of it is made up from two edges: one is only 2 cm long and the other is 98 cm long.
The mesh is shown first without short edge removal, meshed with a length scale of approximately 0.1 m.
The short edge has caused a patch of fine mesh which was not required. The magnified inset clearly shows
the mesh resolving the short edge.




The second picture shows the mesh after short edge removal. The edge tolerance was set to 0.08 m. The
mesh is much smoother since it does not need to resolve the short edge.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
44                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                Suppression of Bodies and Parts




Removing short edges in this way does not give you control over individual edges; you can only specify a
length and then remove all edges shorter than this length. CFX-Mesh allows you to remove individual short
edges in certain circumstances by merging them with adjacent edges to form a Virtual Edge. This is described
in Virtual Edges (p. 51), and a comparison between the Short Edge Removal described in this section and
Virtual Edges is given in Virtual Edges and Short Edge Removal (p. 53).

Suppression of Bodies and Parts


By default, all Parts and Solid Bodies imported into CFX-Mesh are listed in the Tree View, displayed in the
Graphics window and will appear in the surface and volume meshes. This behavior can be changed by using
the Suppress functionality.

In order to suppress a Body or Part, right-click over the relevant entry under Geometry in the Tree View, and
select Suppress. For example, to suppress Body 1, right-click on the entry for Body 1. To unsuppress a Body
or Part which has previously been suppressed, right-click on its name and select Unsuppress. Note that
suppressing a Part is equivalent to suppressing all of the Bodies within the Part.

Suppressing a Body has the following effects:

 •   The Body or Part will be listed in the Tree View as being suppressed, using the following status symbol:
        or     instead of        or
 •   The Body will no longer be displayed in the Graphics window. This can make it easier to manipulate
     and select from geometrical objects in the Graphics window when you have complex geometries.

          Note

          You can also use the Hide functionality to achieve this effect.


 •   The faces, edges and vertices of the Body are no longer available for selection. This means, for example,
     that if you have multiple Bodies and want to select all of the faces in one Body for a 2D Composite
     Region, then you can suppress all the other Bodies, use Box Select to select all visible faces, then unsup-
     press the other Bodies.

          Note

          You can also use the Hide functionality to achieve this effect.


 •   The Body will not appear in any mesh that you generate. Features that are applied to a suppressed
     Body only will be ignored: for example, a Face Spacing which is applied to only a single face on a sup-

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                       45
Geometry

     pressed Body will be ignored as if it was suppressed itself. A features which is applied to both suppressed
     and unsuppressed Bodies will be applied to just the unsuppressed Bodies: for example, a Face Spacing
     which is applied to faces across several bodies will just be applied to those faces on unsuppressed
     Bodies. A Periodic Pair which has only faces from a suppressed Body in one of the two location lists will
     be ignored, even if the other location list contains faces from an unsuppressed Body.

Note that if you mesh multiple Bodies together, then in general you will get a different mesh than if you
mesh each one separately (by suppressing all the Bodies and then unsuppressing them one at a time). This
is because certain meshing features affect the mesh on nearby Bodies. An example of this would occur if
you have a Face Spacing on Body 1 which is close enough to affect Body 2. If you mesh the two Bodies to-
gether, then Body 2 is affected by the Face Spacing. If you mesh Body 2 without meshing Body 1, then the
Face Spacing is not applied and so the mesh on Body 2 is different. Features which can result in the mesh
being different if Bodies are meshed separately include Face Spacings, the existence of shared faces between
a suppressed Body and an unsuppressed Body, Periodic Pairs which are across multiple Bodies, and Surface
Proximity.

The model must always be valid regardless of the state of the suppression of the Bodies. For example, you
are not allowed to create a Periodic Pair (p. 73) on any shared faces. Even if you suppress one of the Bodies
which makes up half of that shared face so that it appears that the other half of the shared face is not shared
any more, you are still not allowed to create a Periodic Pair on that face, because that would be invalid if
the Body was then unsuppressed.

Note that suppressing a Body is different from hiding a Body. If you hide a Body, it is no longer available
for selection and no longer displayed in the Graphics window; however, it will still be included in any
meshing operation.

Control over how the Bodies are displayed is described in Geometry Display (p. 46).

Geometry Display
The display of geometry is controlled using the Geometry section of the Tree View. To change the appearance
of the geometry, left-click on Geometry in the Tree View and modify the controls in the Details View.

The available controls are:

 •   Length Units - shows the length units used for the geometry. This setting can not be changed.
 •   Transparency (%) - Choose the transparency of the Bodies. 100% means that the geometry is completely
     transparent (i.e., it won't show up) and 0% means that the geometry is completely opaque.
 •   Shine (%) - Shine controls how much light is reflected by the faces of the Bodies. 0% gives the lowest
     amount of reflection and will result in the geometry looking matt in texture. 100% gives the most
     amount of reflection and will make the geometry very bright.

It is also possible to control which parts and bodies are displayed; this is described in Suppression of Bodies
and Parts (p. 45) and Hiding Objects (p. 20).




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
46                                                of ANSYS, Inc. and its subsidiaries and affiliates.
Virtual Topology
By default, a surface mesh is generated on every face of each body to be meshed, and at least three mesh
vertices are placed on each edge. If you are meshing very short edges or very narrow faces using a "fine"
mesh length scale in order to resolve these elements, it produces a large mesh, even though the physics of
your CFD problem may not require a fine mesh in these areas. If you do not resolve these small features,
then the final mesh may be of low quality or the mesher may be unable to produce a mesh at all.

In order to remove this limitation, CFX-Mesh allows you to combine faces and edges into Virtual Faces and
Virtual Edges. Once faces and edges have been combined in this way, then the mesher can only see Virtual
Faces and Virtual Edges, and you do not need to resolve their constituent narrow faces or short edges. Vir-
tual Faces and Virtual Edges collectively are referred to as Virtual Topology.

The following topics are covered in this section:

 •   General Information on Virtual Topology
 •   Virtual Faces
 •   Virtual Edges
     –   Virtual Edges and Short Edge Removal
 •   Automatic Virtual Topology
     –   Automatic Merge Strategy
     –   Automatic Merge Option

General Information on Virtual Topology
The following rules apply to the creation of Virtual Topology:

 •   A Virtual Face or Virtual Edge can be created and then added to, or alternatively it may be included in
     a new Virtual Face or Virtual Edge. If an existing Virtual Face or Edge is added to a new Virtual Face or
     Edge and this is successfully created, then the original Virtual Face(s) or Edge(s) will be removed from
     the Tree View.
 •   Once Virtual Topology is created, then as far as the rest of CFX-Mesh is concerned, the underlying
     merged faces or edges no longer exist; the Virtual Faces and Virtual Edges are seen instead. This means
     that if you perform, for example, a Geometry Checking (p. 41), then short edges which have been merged
     into Virtual Edges will no longer show up as being short edges. Faces which have been merged into a
     Virtual Face will no longer be available for selection; you will only be able to select the Virtual Face.
     Virtual entities can be used wherever the ordinary geometric entities of the same type can be used.
 •   Where you use faces to create a Virtual Faces or Virtual Edges that were already in use for a meshing
     feature such as an Inflated Boundary, or a Preview Group, or a Composite 2D Region, then CFX-Mesh
     preserves this as far as possible. So if all of the faces were in the same Inflated Boundary, then the new
     Virtual Face constructed from these faces will also be placed in that Inflated Boundary. However, if only
     some of the faces making up the new Virtual Face were in the Inflated Boundary, then CFX-Mesh cannot
     determine what the intended behavior was and so does not place the new Virtual Face in any Inflated
     Boundary. For most features, if CFX-Mesh cannot determine what the intended behavior was, then the

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               47
Virtual Topology

     new Virtual Face or Edge is not added to any meshing feature of that type. The exceptions to this rule
     are that a new Virtual Face is added to the Default Face Spacing and the Default 2D Region when the
     faces making it up were not all in the same Face Spacing or same Composite 2D Region. Any new Vir-
     tual Face is always added to the Default Preview Group.

     If the creation of a Virtual Face or Virtual Edge results in any meshing feature becoming invalid (because
     its location is no longer valid), then this feature will be marked as invalid. In general, on creation of a
     Virtual entity, CFX-Mesh checks to see whether the CAD entities (faces, edges, vertices, etc.) that were
     present prior to the creation of entity still exist. It then updates the features in the Tree View as follows.
     –   If the geometric location for a CFX-Mesh feature (e.g., a list of faces for a Face Spacing) consists entirely
         of geometric entities which no longer exist, then CFX-Mesh marks that feature as invalid by using
         the invalid status symbol . In order to make the model valid again, you must either delete that
         feature or modify it to specify an appropriate location for the feature (perhaps the new Virtual Face).
     –   If the geometric location for a CFX-Mesh feature (e.g., a list of faces for a Face Spacing) consists of
         both geometric entities which no longer exist and entities which do still exist, then the non-existent
         entities are removed from the location list. For example, if a Face Spacing is applied to three faces,
         and after the creation of the Virtual Face one of these faces no longer exists, then the Face Spacing
         will be automatically modified so that after the creation of the Virtual Face, it is applied to just the
         two remaining faces. Where features are automatically updated in this way, CFX-Mesh marks them
         as such by using the status symbol . Where you see this symbol after creating Virtual Topology,
         you are advised to check that the feature is applied to where you expect it to be. If you want to
         clear this symbol, simply click on the feature name in the Tree View then click next to Location in
         the Details View and just press Apply without modifying anything.
     –   Where a Virtual Face or Edge is added to a geometric location (because all of its constituent faces
         or edges were formerly part of that location) then that feature is also marked with the same status
         symbol    as it has been modified by CFX-Mesh automatically.

     After the creation of Virtual Topology, you should always check that your existing mesh settings are
     still applied to their required location.
 •   If you perform a Geometry Update after creating Virtual Topology, then the Virtual Topology will con-
     tinue to be applied in its existing locations provided that all of these locations exist. If any of the locations
     no longer exist, then the Virtual entity will be marked as invalid and you will have to remove it or re-
     select its location in order to make the model valid again. If you remove the invalid Virtual entity, but
     then later undo the geometry modification and do the Geometry Update again, the Virtual entity will
     be re-created.
 •   Virtual Topology is removed along with all other settings if you choose to Clear Settings.
 •   If a Virtual Face or Edge is removed, then the constituent faces or edges are added into all of the
     meshing features which were previously using them. For example, if a Virtual Face was part of an Inflated
     Boundary, then when the Virtual Face is deleted, its constituent faces are all added to that Inflated
     Boundary.

Virtual Faces
Virtual Faces are created by merging together two or more faces from the geometry to make one larger
surface. The reason why you might want to do this is to avoid having to mesh individual faces. Normally, a
surface mesh is created for every face of each body which is being meshed. In order to produce a reasonable
quality mesh (or in some cases, any mesh at all) on a face which is very narrow, you may need to use a very
small mesh length scale (and hence a large mesh) for regions where the physics of the CFD model do not
require this. If you can merge such narrow faces with other faces, then you can drastically increase the mesh


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
48                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Virtual Faces

length scale in this region, which will result in a mesh with fewer elements. Additionally, you may be able
to merge faces together in such a way that very small angles on the original surfaces are eliminated, which
also leads to a higher quality mesh.

The following simple example shows the use of Virtual Faces.

                                                                                  The geometry contains a very narrow face (only
                                                                                  0.25 mm across compared to the overall dimen-
                                                                                  sions of 30 mm cubed).




                                                                                  If it is just meshed without Virtual Topology, then
                                                                                  even though the overall mesh length scale is rel-
                                                                                  atively coarse, a region of very fine mesh is pro-
                                                                                  duced around the narrow face to resolve it.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                         49
Virtual Topology

                                                                                  Create a Virtual Face from the three faces along
                                                                                  the front left of the cube, to merge the narrow
                                                                                  face with its immediate neighbors.




                                                                                  Now when the mesh is created, the coarse mesh
                                                                                  length scale is used to mesh right across the
                                                                                  narrow face, which is no longer resolved, as re-
                                                                                  quired.The creation of a Virtual Face will, where
                                                                                  possible, automatically merge its external edges
                                                                                  to form Virtual Edges. If this is not desired, auto-
                                                                                  matic merging of edges bounding a new virtual
                                                                                  surface can be turned off on the Virtual Topology
                                                                                  section of the Options panel.The figure to the
                                                                                  left shows the behavior if automatic edge mer-
                                                                                  ging is turned on (the default).

                                                                                  This figure shows the behavior if automatic edge
                                                                                  merging is turned off.This results in a fine mesh
                                                                                  along the two short edges that are left where the
                                                                                  ends of the narrow surface used to be. Even if
                                                                                  automatic edge merging is turned off, you can
                                                                                  still create any desired Virtual Edges manually;
                                                                                  see Virtual Edges.




To create a Virtual Face, right-click on Virtual Topology in the Tree View, and select Insert > Virtual Face.
You can then select the faces required from the Graphics window (you cannot select faces by selecting a

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
50                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Virtual Edges

Composite 2D Region). All faces must be adjacent so that the Virtual Face is a single continuous entity. Vir-
tual Faces are NOT restricted to groups of surfaces where the angle between the average combined surface
normal and any normal on the combined faces exceeds 90 degrees. However, Virtual Faces cannot form a
closed region, for example, all six sides of the cube shown above cannot be combined into a Virtual Face,
but if any one of the sides of the cube is not included, then the new Virtual Face is not a closed region and
creation is allowed.

Sometimes even when your selection of faces for a Virtual Face does not break the rules given above, the
Virtual Face will not be created. This is a limitation of the methods used to create Virtual Faces. In general,
if you have difficulty creating a Virtual Face, then try to include fewer faces to merge together, or merge
the face that you want to remove with the neighboring face that has the simplest geometry and topology.

Note that if you merge faces which do not meet at a tangent, then the sharp angle where they meet will
be rounded off over a distance of approximately 1 local element size.

Some general notes on Virtual Topology (which apply to Virtual Faces) are given in General Information on
Virtual Topology (p. 47).

Virtual Edges
Virtual Edges are created by merging together two or more edges from the geometry to make one larger
edge. The reason why you might want to do this is to avoid having to mesh an individual edge. Normally,
when the surface mesh is created for a face, at least three nodes are placed on every edge. This will result
in a very fine mesh near short edges, in regions where the physics of the CFD model do not necessarily require
this. If you can merge these short edges with other edges, then you can drastically increase the mesh length
scale in this region and make a mesh containing fewer elements.

The following simple example shows the use of Virtual Edges. Virtual Edges can be used to eliminate edges
independent of the presence of Virtual Faces.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                         51
Virtual Topology

                                                                                   The geometry is a cube which contains six square
                                                                                   faces, with side length 30 mm each. However,
                                                                                   two of the edges are broken into three segments
                                                                                   each, including a very short edge of only 0.25
                                                                                   mm across.The mesh is very refined around the
                                                                                   two short edges.




                                                                                   Create a Virtual Edge from three edges to merge
                                                                                   the short edge with its immediate neighbors.
                                                                                   Also create another Virtual Edge from the three
                                                                                   edges at the bottom of the cube to merge that
                                                                                   short edge, too (not shown in the diagram).




                                                                                   Now when the mesh is created, the coarse mesh
                                                                                   length scale is used to mesh right across the
                                                                                   whole geometry, with no need for small ele-
                                                                                   ments near where the short edge used to be.




To create a Virtual Edge, right-click on Virtual Topology in the Tree View, and select Insert > Virtual Edge.
You can then select the edges required from the Graphics window. All edges must be adjacent so that the

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
52                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                      Virtual Edges and Short Edge Removal

Virtual Edge is a single continuous entity. You can only merge edges which form part of the boundary of
the same two faces.

By default, whenever a Virtual Face is created, the perimeter of the new face is checked for edges which
can be merged. Wherever there are two or more edges which are shared between the same two faces (the
new Virtual Face and one other) and which meet at an angle which is less than some tolerance (default of
5 degrees), then a Virtual Edge is automatically created. Any such edges will appear in the Tree View with
the status symbol     which shows that the item has been automatically generated.

You can disable the automatic creation of Virtual Edges by using Tools > Options and setting the parameter
Meshing > Meshing > Virtual Topology > Merge Edges Bounding Manually Created Faces to No. Only
edges which meet at an angle of less than the specified tolerance will be merged; this means that sharp
corners on edges will be preserved. The tolerance can also be changed using Tools > Options, with the
Meshing > CFX-Mesh Options > Virtual Topology > Automatic Edge Merging Tolerance (Degrees)
parameter.

Sometimes a Virtual Edge will appear with the status symbol of . This can occur when a Virtual Face has
been created adjacent to the Virtual Edge, after the creation of the Virtual Edge. When this symbol is present
the Virtual Edge cannot be deleted as this would cause an inconsistent geometry definition. If you need to
delete this Virtual Edge, first delete the Virtual Face which was created after it and is adjacent to it. The Vir-
tual Edge will then be available for deletion.

Some general notes on Virtual Topology (which apply to Virtual Edges) are given in General Information on
Virtual Topology (p. 47). See Virtual Edges and Short Edge Removal (p. 53) for a discussion of why using Virtual
Edges is different from using Short Edge Removal.

Virtual Edges and Short Edge Removal
CFX-Mesh contains two ways of removing short edges: Short Edge Removal and Virtual Edges. This section
describes the differences between them.

Short Edge Removal removes all edges shorter than a certain length (which you specify) in the geometry.
When the mesher sees a short edge which is to be removed, the behavior is as if the edge was collapsed
to zero length: a single node is placed at one end of the edge and no other nodes are put on the edge at
all. As a result, you can only merge short edges which are shorter than the local mesh length scale, or your
resulting mesh will be badly distorted. There is no individual control over which edges should be regarded
as short; all edges below the specified length scale will be removed.

The creation of a Virtual Edge is effectively a merger of two or more edges, creating a single, longer edge.
The mesher will place nodes along the Virtual Edge with no regard for where the original edges were. There
is no requirement that the merged edges are smaller than the mesh length scale. However, you can only
merge edges which are shared between the same two faces of the geometry. You have individual control
over which edges are merged and can create each Virtual Edge separately. In some circumstances Virtual
Edges can also be created automatically; see Virtual Edges (p. 51) for more details.

Short Edge Removal and Virtual Edges can be used in the same mesh setup. Where the setup contains both,
Virtual Edges take precedence, i.e., Virtual Edges are created first, and then Short Edge Removal removes
any remaining edges of a length shorter than the given length scale.

In general, where it is possible, it is recommended that you remove short edges by using Virtual Edges rather
than Short Edge Removal. This approach results in greater consistency with other features of CFX-Mesh.

Some examples are shown in the table below.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                  53
Virtual Topology

 Ex-               Geometry                                   Mesh with short edge                                Mesh without short edge
ample
     1




         In this example, the short edge to be eliminated can be removed by using Short Edge Removal,
         provided that the mesh length scale is large enough and there are no shorter edges elsewhere in
         the geometry that you need to keep. In this example the mesh length scale is only a few times longer
         than the length of the short edge and so there is a very slight distortion in the mesh where the node
         from one end of the edge has been collapsed onto the node at the other end of the edge.The short
         edge cannot be removed using Virtual Edges because there is no edge shared between the same
         two faces that it can be merged with.
     2




         In this example there is a whole series of short edges to be removed. Short Edge Removal cannot
         be used because the entire length of the series of edges would be collapsed and the distortion
         would be too large. However, the series of short edges can be merged into one Virtual Edge.
     3




         In this example, either Short Edge Removal could be used or the short edge could be merged with
         its neighbor to its right to make Virtual Edge.The decision on which method to use would depend
         on whether you had other short edges you wanted to remove and whether you needed the indi-
         vidual control that you get by using Virtual Edges.The resulting mesh produced by the two methods
         is slightly different.The top mesh, produced by Short Edge Removal, is very slightly distorted since
         the mesh length scale is not much greater than the length of the short edge.The bottom mesh is
         produced by the Virtual Edge method.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
54                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                Generating the Virtual Topology


Automatic Virtual Topology
In addition to the manual creation of Virtual Edges and Faces in CFX-Mesh, there is a facility to automatically
create Virtual Topology for your model in order to improve the quality of your mesh. This capability involves
an automatic step to detect candidate edges and faces that could be merged based on geometric parameters
such as contact angle between faces, relative areas of faces, aspect ratios and shared boundary ratio. The
aim of this method is to detect sufficient candidates for merging in order to simplify the geometry to the
extent that a good CFD mesh can be generated with minimal user effort. Once these candidates have been
detected, virtual edges and faces are created automatically.

The user controls for this feature are very simple. When you select Virtual Topology in the Tree View, the
following controls are available in the Details View.

 •   Automatic Merge Strategy controls the aggressiveness of the automatic Virtual Topology algorithm.
     The Low option merges the worst faces and edges in the model, while the High option attempts to
     merge much more of the geometry.

     In some cases, using the High option for Automatic Merge Strategy may result in fewer Virtual Faces
     being created than the Low or Medium option. This can happen because more candidate faces are
     identified than with the lower strategies, but when attempting to do the actual merge of surfaces the
     parameterisation can fail. If this problem does occur, it is possible to apply the High strategy to a
     subset of the faces in the model. This may succeed where the global merge fails. An alternative approach
     is to start with a Low strategy and then subsequently re-run with a higher strategy.

          Note

          The High option may result in less robust meshing, as merging large numbers of surfaces
          can result in a distorted parameterization, which can be difficult to mesh. It is recommended
          that a Low or Medium option is used initially as this may be sufficient for your problem.


 •   Automatic Merge Option defines whether the automatic Virtual Topology operation should be applied
     to the whole model (the default) or whether it should only apply to a selection of faces. The face selection
     can be defined by selecting the faces directly from the graphics window or by selecting a Region name
     in the tree view.

Generating the Virtual Topology
To generate the Virtual Topology, select Virtual Topology > Generate Virtual Topology on Entire Model
or Virtual Topology > Generate Virtual Topology on Selected Set depending on your options. In addition,
it is possible to right-click on a control (such as inflated boundary) and select Simplify Location using Vir-
tual Topology.

This feature will honor existing Region definitions, Virtual groups and Mesh Controls. This means that while
a new Virtual Group may be created that lies within a selection, it will not propagate across the boundary
of the selection and will not invalidate these existing selections.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                       55
     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
56                               of ANSYS, Inc. and its subsidiaries and affiliates.
Regions
The geometry which defines your simulation is a collection of one or more Solid Bodies and the faces which
bound them. CFX-Mesh has several features which require you to select some part of the geometry in order
to provide a location for the feature.

CFX-Mesh also allows you to give names to parts of the geometry. These Composite Regions can then be
used for specifying locations in CFX-Mesh. They will also label collections of nodes or elements in the mesh
output from CFX-Mesh, for use in the CFX-Pre. Currently, only Composite 2D Regions can be created in CFX-
Mesh.

Composite 2D Regions can be created automatically from Named Selections created in DesignModeler.

You do not need to define any Composite Regions in CFX-Mesh, since you can always select the parts of
the geometry directly in CFX-Mesh. Mesh associated with particular Solid Bodies and faces is accessible in
CFX-Pre even without creating a Composite Region. However, it is often much easier or clearer to select
parts of the geometry for a Composite Region and then to use it by name later during the mesh setup than
it is to select the geometry directly each time it is to be used. It is also easier to select and name parts of
the geometry (for use in the CFD simulation) within CFX-Mesh than it is to select the appropriate mesh regions
within CFX-Pre.

The Regions part of the Tree View contains details of all of the Composite Regions which have been defined
in the model.
 2D Regions
 Named Selections in CFX-Mesh

2D Regions
When you are asked to select a 2D Location for your meshing feature, in most cases you will be able to select
2D Regions directly from the geometry or from a list of Composite 2D Regions which you have previously
defined.

If your geometry has more than one solid body meeting at a shared face, then you need to understand the
difference between a 2D Region and a face.

Available Composite 2D Regions are shown under Regions in the Tree View.

2D Regions and Faces
CFX-Mesh will often ask you to select one or more 2D Regions for the location of a meshing feature. Where
two Solid Bodies meet at a common face, there is just one face present in the geometry; however, there are
two 2D Regions, as shown in the example below.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               57
Regions

If your model has only one solid, then each face is also a 2D Region, and vice versa. If your model has more
than one solid, then all of the external faces will also be 2D Regions. However, two 2D Regions will exist for
every shared (internal) face (assuming that you have combined the solids into the same part). Each meshing
feature that requires you to specify a location has its own rules about whether or not you can set different
properties for the two 2D Regions which make up a shared face.

 •   Composite 2D Region: You may include any combination of 2D Regions in a Composite 2D Region (in-
     cluding just one or both sides of a shared face). However, if you are going to use a Composite Region
     to specify the location for any other meshing feature, then you must make sure that it only includes
     2D Regions which satisfy the requirements of the appropriate feature.
 •   Face Spacing (p. 64): It is important that you do not try to apply different Face Spacings to 2D Regions
     which are the two sides of a common face, since the surface mesh is generated on the common face,
     not on the 2D Regions separately. It is acceptable to include a 2D Region which forms one half of a
     shared face in a Face Spacing without including the other side of the shared face, but only if the 2D
     Region which forms the other side is not included in any other Face Spacing (other than the Default
     Face Spacing).
 •   Inflated Boundary (p. 81): When creating an Inflated Boundary, you can have different settings for the
     two different 2D Regions which make up a common face, i.e., you can apply Inflation to one 2D Region
     and not the other, or to both but with different settings. The example below shows the difference in
     one particular case.




 •   Preview Group (p. 97): A Preview Group can contain any combination of 2D Regions. It does not matter
     if 2D Regions are contained in more than one Preview Group, nor if a 2D Region is included which forms
     one half of a shared face, but the other half is not included.

If you try to pick a 2D Region which is half of a shared face, then the Selection Rectangles will appear. Each
shared face will be represented by two rectangles which are attached to each other, one for each side or
2D Region, as shown below. You can use these rectangles to select individual 2D Regions easily and accurately.




CFX-Mesh will not allow you to select locations for meshing features which break the rules given for each
feature.

Composite 2D Regions and Default 2D Region

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
58                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                 Named Selections in CFX-Mesh

In places where you are required to select a 2D Region to specify a location for a meshing feature, CFX-Mesh
recognizes two types of 2D Region: Primitive and Composite. The primitive regions are those which exist in
the geometry by default: there is one for every external face and two for each shared face (see 2D Regions
and Faces (p. 57) for more details). You can select these 2D Regions directly from the geometry in the
Graphics window. The composite regions are those which you create explicitly, and consist of one or more
primitive 2D Regions which you select and give a name to.

You can create a Composite 2D Region from any single primitive 2D Region or group of primitive 2D Regions.
No primitive 2D Region can be assigned to more than one Composite 2D Region. A Default 2D Region is
created by CFX-Mesh and cannot be renamed or deleted; this always contains any primitive 2D Regions that
have not been used in other Composite 2D Regions, and its contents change dynamically as you create and
modify other Composite 2D Regions. In this way, every primitive 2D Region is always assigned to exactly
one Composite 2D Region. If the Default 2D Region should become empty then it is automatically removed,
but will re-appear if any Composite 2D Region ceases to be used by the other user-defined Composite 2D
Regions.

To create a Composite 2D Region, right-click over Regions in the Tree View, and select Insert > Composite
2D Region. You can then select the required primitive 2D Regions from the Graphics window. A Composite
2D Region can be deleted or renamed by right-clicking over its name in the Tree View.

You can use the Composite 2D Regions to specify locations for meshing features in CFX-Mesh, rather than
having to select the faces individually. Simply click on the name of the Composite 2D Region from the Tree
View (p. 17) to select it, instead of clicking on the faces in the Graphics window.

Any Composite 2D Regions that you create in CFX-Mesh appear in CFX-Pre and can be used as locations for
boundary conditions and domain interfaces. The 2D Regions and their names are written to the CFX Mesh
file with the mesh. Even if you do not specify any Composite 2D Regions in CFX-Mesh, mesh on the primitive
2D Regions will still be available for selection to define boundary conditions in CFX-Pre. However, the following
advantages apply if you create at least some Composite 2D Regions in CFX-Mesh:

 •   It may be easier to select the primitive 2D Regions you require in CFX-Mesh than in CFX-Pre.
 •   If the faces you need are not available to be selected, then you will find this out before meshing the
     geometry, rather than creating the mesh and then discovering that the face you need is not available
     in CFX-Pre. This might happen, for example, if two faces that you expected to be separate actually form
     a single face, due to the way that you created the geometry.

You may also want to create additional Composite 2D Regions if, for example, you want to create plots on
individual or groups of faces during post-processing.

Named Selections in CFX-Mesh
Named Selections created in DesignModeler can be imported into CFX-Mesh as Composite 2D Regions.

     Note

     CFD users of the DesignModeler, Meshing, and CFX applications should refer to Named Selections
     and Regions for CFX Applications under the Meshing Help for important information about region
     definitions.

This functionality has to be enabled before it can be used, and then it only applies to new CFX-Mesh databases.
Existing databases (from both this release and previous releases) cannot be updated to use Named Selections
if it is not enabled when they are created.


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                      59
Regions

You can choose to enable this functionality for all databases or a single database. To enable it for all new
databases, do the following:

 1.    Open the Workbench Options. Under Geometry Import select the Named Selection check box.
 2.    To import all Named Selections regardless of their name, remove all characters from the Filtering
       Prefixes field.

       If you want to restrict the import of Named Selection according to their names, then enter the Named
       Selection prefix key into the Filtering Prefixes field. All Named Selections whose name starts with
       this prefix will then be imported.
 3.    Now, every time you start a new CFX-Mesh database using the DesignModeler, Named Selections will
       be imported into CFX-Mesh.

If you only want to enable this functionality for selected databases, then do the following:

 1.    On the Project Schematic, right-click the Geometry cell containing the DesignModeler geometry file
       and select Properties from the shortcut menu.

       A properties window opens for the selected cell.
 2.    In the properties window, turn on the option for Named Selections option in the Basic Geometry
       Options group.
 3.    To import all Named Selections regardless of their name, remove all characters from the Named Selec-
       tion Key field.

       If you want to restrict the import of Named Selections according to their names, then specify the desired
       name in Named Selection Key field. All Named Selections whose name starts with this prefix will then
       be imported.
 4.    Now, you can start a new CFX-Mesh database using the selected DesignModeler geometry file.

In CFX-Mesh there are restrictions on the use of Composite 2D Regions, in that no primitive 2D Region can
be assigned to more than one Composite 2D Region. This restriction does not apply to Named Selections
when created in DesignModeler and therefore, when geometry containing Named Selections is imported
into CFX-Mesh, all Named Selections will be ignored if any of them do not comply with the rules governing
CFX-Mesh Composite 2D Regions. The warning message will reference the Named Selections that are causing
the problem. If this occurs, then you will need to return to DesignModeler and remove the Named Selection(s)
that overlap. In CFX-Mesh, you can then perform an Update Geometry or open the geometry in a new
CFX-Mesh session.

If you later return to DesignModeler and modify the Named Selections, and then try to update the geometry
to incorporate these changes into CFX-Mesh, then the following behavior occurs.

 •    If you modify the location of an existing Named Selection in DesignModeler, then when you update
      the geometry in CFX-Mesh, this modification will be applied to the equivalent Composite 2D Region in
      CFX-Mesh as long as the new location does not overlap with the location of any existing Composite 2D
      Regions in CFX-Mesh (including other regions generated from Named Selections).
 •    If you delete a Named Selection in DesignModeler then when you update the geometry in CFX-Mesh
      the equivalent Composite 2D Region is not deleted. You must delete it manually if you no longer want
      this region in CFX-Mesh.
 •    If you rename a Named Selection in DesignModeler, then when you update the geometry in CFX-Mesh,
      the Named Selections will not be re-imported. You must either rename or delete the equivalent Com-
      posite 2D Region in CFX-Mesh before updating the geometry. This is because CFX-Mesh effectively sees


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
60                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                            Named Selections in CFX-Mesh

the renamed Named Selection as a new Named Selection, and then finds that its location overlaps with
the existing Composite 2D Region which has the original name of the Named Selection.




                Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                            of ANSYS, Inc. and its subsidiaries and affiliates.                                      61
     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
62                               of ANSYS, Inc. and its subsidiaries and affiliates.
Meshing Features
The following functions are available to control the mesh generation process:

 •   Body Spacing (p. 63)
 •   Face Spacing (p. 64)
 •   Edge Spacing (p. 65)
 •   Point Spacing (p. 68)
 •   Point Control (p. 69)
 •   Line Control (p. 70)
 •   Triangle Control (p. 71)
 •   Periodicity (p. 72)
 •   Inflation (p. 75)
 •   Stretch (p. 83)
 •   Proximity (p. 84)
 •   Mesh Options (p. 86)

In addition, faces can be merged and short edges removed using the Virtual Topology functionality.

Spacing

You can specify the background mesh length scale for a body or bodies by using a Body Spacing (p. 63).

You can also specify the mesh length scale for particular faces or edges using a Face Spacing (p. 64) or Edge
Spacing (p. 65). A Face or Edge Spacing can also influence the mesh in the nearby volume.

Other controls over the mesh length scale at any given point are described in Controls (p. 68), Stretch (p. 83)
and Proximity (p. 84).

Body Spacing

The Body Spacing for a body gives the background length scale for its volume, i.e., the length scale before
any Face Spacing (p. 64), Controls (p. 68) or other explicit length scale controls are applied. It should be set
to the coarsest length scale required anywhere in the body, since no elements can be created that are larger
than the Body Spacing in that body.

                                                         .
One Body Spacing exists by default: “Default Body Spacing” This applies to all bodies. Only one parameter
can be controlled for the Default Body Spacing:




                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                       of ANSYS, Inc. and its subsidiaries and affiliates.                               63
Meshing Features

 •   Maximum Spacing - This is the maximum element size which will be used when creating triangles on
     the faces of the body and tetrahedra in the volume of the body. The default is set to around 5% of the
     maximum extent of the model. CFX-Mesh will accept any length (greater than zero) for this size.

Currently, no other Body Spacing objects may be created.

Face Spacing

A Face Spacing is used to specify the mesh length scale on a face (or faces) and in the volume adjacent to
the selected faces.

                                                            .
One Face Spacing exists by default: “Default Face Spacing” This applies to all faces which have not been
explicitly selected for inclusion in other Face Spacings. Each additional Face Spacing is applied to a face or
faces which you must select.

To create a new Face Spacing, right-click on Spacing in the Tree View. After creation, Face Spacings (except
the Default Face Spacing) can be deleted, suppressed (made inactive) or renamed by right-clicking on their
names in the Tree View.

You must specify the following information to define a Face Spacing:

 •   Face Spacing Type - This can be set to one of four types:
     – Angular Resolution (p. 67)
     –   Relative Error (p. 67)
     –   Constant - Set a Constant Edge Length for the faces, overriding the Body Spacing (p. 63). You cannot
         set this length scale to be larger than the Maximum Spacing specified in the Default Body Spacing.
     –   Volume Spacing - Use the same spacing on the face as the Maximum Spacing specified for the
         Body on the faces selected.
 •   Minimum Edge Length - Enter the Minimum Edge Length for the surface mesh on the faces. This only
     applies when Angular Resolution or Relative Error has been selected as the Face Spacing Type.
 •   Maximum Edge Length - Enter the Maximum Edge Length for the surface mesh on the faces. This only
     applies when Angular Resolution or Relative Error has been selected as the Face Spacing Type. It must
     be given a value between the Minimum Edge Length and the Maximum Spacing set under Default Body
     Spacing.
 •   Radius of Influence - Specify the extent of the Face Spacing influence. If, for example, you specify a
     Radius of Influence of 2 cm then the region of space within 2 cm of the Face Spacing is filled with mesh
     with the same length scale as on the face itself. Beyond the Radius of Influence, the size of the elements
     expands as you move away from the faces, in accordance with the Expansion Factor. This parameter
     does not apply when the Face Spacing Type is set to Volume Spacing.
 •   Expansion Factor - Specify how fast the mesh length scale returns to its background value away from
     a region where it has been constrained by a Face Spacing. Each successive element as you move away
     from the face (outside the Radius of Influence specified above) is approximately one Expansion Factor
     larger than the previous one. Hence large values tend to coarsen the mesh rapidly away from the face.
     This parameter also governs how fast a local surface length scale that has been overridden near a curve
     (because of its curvature) expands back to its global value. It therefore controls both the rate of growth
     of volume elements away from faces and the rate of growth of surface elements away from curved
     boundaries into the middle of a flat face. It does not apply when the Face Spacing Type is set to Volume
     Spacing. Expansion Factors should be between 1.0 and 1.5.


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
64                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                      Edge Spacing

 •   Location - Select the face(s) of the model from the Graphics window to use for the Face Spacing. You
     can either select faces directly from the Graphics window or select Composite 2D Regions (or the Default
     2D Region) from the Tree View. The Default Face Spacing does not allow you to make this selection,
     since it automatically applies to all faces which have not been explicitly selected for inclusion in other
     Face Spacings.

     A face cannot be in more than one Face Spacing. If you have multiple Solid Bodies in your geometry,
     then you should read the information on the difference between faces and 2D Regions to understand
     how you can apply Face Spacings to the faces which form the boundaries between the bodies.

The figure below shows a Face Spacing on a 1 m cube, with a Constant Edge Length of 0.05 m, Radius of
Influence 0.2 m, and Expansion Factor 1.2.




Any Face Spacing other than the Default Face Spacing will have a volumetric effect, except when set to use
the Volume Spacing. The Radius of Influence determines the volume that the Face Spacing is applied to
away from the face. This will affect both the volume mesh and the surface mesh on faces within the Radius
of Influence.

The Radius of Influence can be set to zero, in this case the Face Spacing is applied only to the selected faces.
A volumetric effect will still be seen as the edge length scale is expanded back into the volume mesh, but
the expansion will begin as soon as you move away from the face.

When Face Spacings are used (other than the Default Face Spacing using the Volume Spacing option), then
nearby faces may also be affected. For example, if you create a Face Spacing with a Radius of Influence of
2 cm, then another face which is 2 cm away will also be affected. In order to achieve this, the surface
mesher will run twice; once to generate an initial mesh and detect faces which are within the region of in-
fluence of a Face Spacing, and then a second time after reducing the local background mesh length scale
based on the proximity of faces.

Edge Spacing


An Edge Spacing is used to specify the mesh length scale on an edge (or edges) and in the volume adjacent
to the selected edges.

To create a new Edge Spacing, right-click on Spacing in the Tree View. After creation, Edge Spacings can
be deleted, suppressed (made inactive) or renamed by right-clicking on their names in the Tree View.

You must specify the following information to define an Edge Spacing:

 •   Edge Spacing Type - This can be set to one of four types:
     –   Angular Resolution (p. 67)
     –   Relative Error (p. 67)


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                        65
Meshing Features

     –   Constant - Set a Constant Edge Length for the edges, overriding the Body Spacing (p. 63). You
         cannot set this length scale to be larger than the Maximum Spacing specified in the Default Body
         Spacing.
     –   Volume Spacing - Use the same spacing on the face as the Maximum Spacing specified for the
         Body on the faces selected.
 •   Minimum Edge Length - Enter the Minimum Edge Length for the surface mesh on the edges. This only
     applies when Angular Resolution or Relative Error has been selected as the Edge Spacing Type.
 •   Maximum Edge Length - Enter the Maximum Edge Length for the surface mesh on the edges. This
     only applies when Angular Resolution or Relative Error has been selected as the Edge Spacing Type. It
     must be given a value between the Minimum Edge Length and the Maximum Spacing set under Default
     Body Spacing.
 •   Radius of Influence - Specify the extent of the Edge Spacing influence. If, for example, you specify a
     Radius of Influence of 2 cm then the region of space within 2 cm of the Edge Spacing is filled with mesh
     with the same length scale as on the edge itself. Beyond the Radius of Influence, the size of the elements
     expands as you move away from the edges, in accordance with the Expansion Factor. This parameter
     does not apply when the Edge Spacing Type is set to Volume Spacing.
 •   Expansion Factor - Specify how fast the mesh length scale returns to its background value away from
     a region where it has been constrained by an Edge Spacing. Each successive element as you move away
     from the edge (outside the Radius of Influence specified above) is approximately one Expansion Factor
     larger than the previous one. Hence large values tend to coarsen the mesh rapidly away from the edge.
     It does not apply when the Edge Spacing Type is set to Volume Spacing. Expansion Factors should be
     between 1.0 and 1.5.
 •   Location - Select the edge(s) of the model from the Graphics window to use for the Edge Spacing. You
     can select edges directly from the Graphics window.

     An edge cannot be in more than one Edge Spacing.

The figure below shows an Edge Spacing on a 1 m cube, with a Constant Edge Length of 0.05 m, Radius of
Influence 0.2 m, and Expansion Factor 1.2.




Any Edge Spacing will have a volumetric effect, except when set to use the Volume Spacing. The Radius of
Influence determines the volume that the Edge Spacing is applied to away from the edge. This will affect
both the volume mesh and the surface mesh on faces within the Radius of Influence.

The Radius of Influence can be set to zero, in this case the Edge Spacing is applied only to the selected
edges. A volumetric effect will still be seen as the edge length scale is expanded back into the volume mesh,
but the expansion will begin as soon as you move away from the edge.

When Edge Spacings are used, then nearby edges and faces may also be affected. For example, if you create
an Edge Spacing with a Radius of Influence of 2 cm, then another edge or face which is 2 cm away will also
be affected.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
66                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Relative Error

There are certain circumstances where an Edge Spacing may not have the effect which you intend i.e.:

 •   one or both faces which are adjacent to the edge with the Edge Spacing have a Face Spacing defined
     with the Angular Resolution or Relative Error option, and
 •   the Edge Spacing refines the spacing on the edge to less than the Minimum Edge Length set for the
     one or both of the Face Spacings on the adjacent faces.

In this case the nodes would be placed on the edge in accordance with the Edge Spacing. However, when
nodes were then placed on the adjacent face(s) with the Minimum Edge Length which is greater than the
local edge spacing, the mesh length scale would immediately transition to the Minimum Edge Length specified
by the Face Spacing (rather than expanding away using the Expansion Factor specified by the Edge Spacing).
This would result in significant distortion of the mesh. However, the mesher is able to detect when this
would occur, and when this situation arises, it will coarsen the spacing on the edge back to the Minimum
Edge Length of the face with the largest Minimum Edge Length. This can make it appear as if the Edge
Spacing is being ignored. The way to avoid this situation occurring is to set the Minimum Edge Length of
the Face Spacing(s) of the two adjoining faces to be less than or equal to the smallest edge length arising
from the Edge Spacing.

Edge Spacings cannot be used with the Advancing Front (AF) Surface Mesher (p. 87). If you have enabled this
surface mesher then you will not be able to create any Edge Spacings and any existing ones will be hidden
and ignored.

Angular Resolution
The Angular Resolution option for Face Spacing (p. 64) and Edge Spacing (p. 65) allows the edge length on
particular faces or edges to vary depending upon the local curvature. That is, a short edge length is used
where the face or edge is highly curved, and a longer edge length is used where it is flatter. It is used for
automatically refining the mesh in geometries that have curved faces or edges and can replace the need
for other Controls (p. 68) in such geometries. It has a similar effect to using the Relative Error (p. 67) setting,
but is specified differently.

In order to control how much the curvature is resolved, you must set the Angular Resolution parameter.
This represents the maximum angle allowed to be subtended by the arc between two adjacent surface mesh
nodes. When the angle is made smaller, more nodes will be placed on the edge or surface to resolve the
curvature better. CFX-Mesh will allow you to set this parameter to anything between 1.0 degree and 90.0
degrees.




When this option is used, you can set a Minimum and Maximum Edge Length in the Details View for the
Face Spacing, to prevent over-refinement in regions of high curvature and over-coarsening on flat faces.

Relative Error
The Relative Error option for Face Spacing (p. 64) and Edge Spacing (p. 65) allows the edge length on partic-
ular faces or edges to vary depending upon the local curvature. That is, a short edge length is used where
the face or edge is highly curved, and a longer edge length is used where it is flatter. It is used for automat-
ically refining the mesh in geometries that have curved faces or edges and can replace the need for other
Controls (p. 68) in such geometries. It has a similar effect to using the Angular Resolution (p. 67) setting, but
is specified differently.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                          67
Meshing Features




In order to control how much the curvature is resolved, you must set the Relative Error. The Relative Error
is the maximum deviation of the resulting mesh away from the geometry face or edge expressed as



where r is the local radius of curvature. The value entered should be in the range of approximately 0.00004
to 0.292, which corresponds to 360 edges and 4 edges per circumference, respectively. When the Relative
Error is made smaller, more nodes will be placed on the edge or face to resolve the curvature better.

Controls

Mesh Controls are used to refine the surface and volume mesh in specific regions of your model. The mesh
refining effect decays with increasing distance from the control, generating progressively coarser elements.
Controls can be defined using any point on the model (e.g., a vertex or any point on any face of the model)
or by specifying coordinates. They can be located anywhere in the 3D space of your model: inside, outside
or on the edge.

Three types of volumetric Controls are available: Point, Line and Triangle. In addition, a volumetric effect
may be obtained by using a Face Spacing (p. 64) or Edge Spacing (p. 65).
 Point Spacing
 Point Control
 Line Control
 Triangle Control

You can suppress (make inactive) all of the Controls in the model by right-clicking on Controls in the Tree
View.

Point Spacing

Each of the three volumetric controls (Point, Line, and Triangle) require you to specify spacing attributes for
the Control at appropriate points. A Point Spacing is a set of values which can be used for this purpose.
There are three required values:

 •   Length Scale - a length scale for the mesh size in the locality of the point to which the Point Spacing
     is applied. This must be less than the Maximum Spacing set under Default Body Spacing.
 •   Radius of Influence - the radial extent of the fixed local length scale influence. If, for example, you
     specify a Radius of Influence of 2 cm then the region of space within 2 cm of the Control is filled with
     mesh with the length scale given by the Length Scale specified above.
 •   Expansion Factor - the mesh coarsening rate is determined by a geometric expansion factor. Each
     successive element as you move away from the Control (outside the radius specified above) is approx-
     imately one Expansion Factor larger than the previous one. Hence large values tend to coarsen the
     mesh rapidly from the Control. Expansion Factors should be set to between 1.0 and 1.5.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
68                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Point Control

A new Point Spacing can be created by right-clicking on Controls in the Tree View and selecting Insert >
Point Spacing. After creation, a Point Spacing can be renamed, deleted or duplicated by right-clicking on
its name in the Tree View. Also note that if you duplicate a Point Spacing, its values are copied into the new
Point Spacing, but there is no further link between them, i.e., if you change the original Point Spacing, then
the duplicate will not be updated in any way.

Point Control

A Point Control controls the mesh spacing in a spherical region.




You must specify two things to define a Point Control:

 •   Point - You can select a point for the Control by selecting a vertex from the model, selecting an arbitrary
     point on the model faces or by specifying its coordinates. See Point Selection (p. 13) for details.
 •   Spacing - Select a Point Spacing (p. 68) which defines the mesh attributes for the Point Control (Length
     Scale, Radius of Influence and Expansion Factor). To make the selection, click in the box next to Spacing,
     click on the name of the required Point Spacing in the Tree View, and then click on Apply back in the
     Details View.

The figure below shows a Point Control on a 1 m cube, with Length Scale 0.05 m, Radius of Influence 0.2
m, and Expansion Factor 1.2.




A new Point Control can be created by right-clicking on Controls in the Tree View and selecting Insert >
Point Control. After creation, a Point Control can be renamed, suppressed (made inactive), deleted or du-
plicated by right-clicking on its name in the Tree View. Note that if you duplicate a Point Control, its settings
are copied into the new Point Control, but there is no further link between them, i.e., if you change the
original Point Control, then the duplicate will not be updated in any way. If you want to suppress all the
Controls in the model, right-click over Controls and select Suppress.

Once a Point Control is created and is valid, then if you click on its name in the Tree View, the Point Spacing
that it refers to will be highlighted, and a small graphic similar to the one shown below will appear at the
location of the Point Control.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                         69
Meshing Features

In this graphic, the small sphere at the center shows you where the point itself is located. The middle sphere
(green in the picture) shows you the mesh Length Scale at that point, and the largest sphere (blue) shows
you the Radius of Influence. If the Radius of Influence is zero, then this sphere will not show up separately.

To view all Controls together, select the Controls entry in the Tree View. All Controls will then be highlighted
in the Graphics window.

Line Control

A Line Control controls the mesh spacing in a region defined by a cylindrical volume between two spheres.




You must specify a Point location and a Point Spacing (p. 68) for each of two points to define a Line Control.
The line for the control is the straight line between the two end-points, not the model edge which joins the
two points (if any).

Each of the two points which form the line can have different Point Spacings, which means different settings
of Length Scale, Radius of Influence, and Expansion Factor. Where the settings for any parameter are different,
the two values are blended linearly as you move along the line.

The items you need to specify for a Line Control are:

 •   Point 1 / Point 2 - You can select points for the Control by selecting vertices from the model, selecting
     arbitrary points on the model faces or by specifying coordinates. See Point Selection (p. 13) for details.
 •   Spacing Definitions - If you want to specify the same Point Spacing (p. 68) for both points, set Spacing
     Definitions to Uniform. If you want to specify a different Point Spacing (p. 68) for each point, set
     Spacing Definitions to Individual.
 •   Spacing / Spacing 1 / Spacing 2 - Select a Point Spacing (p. 68) which defines the mesh attributes. If
     you selected to set one Point Spacing for both points, then the selection you make for Spacing will
     apply to both points; if you selected to set a different Point Spacing for each point, then you must
     separately select a Spacing 1 and Spacing 2 to apply to Point 1 and Point 2 respectively. To make the
     selection, click in the box next to Spacing / Spacing 1 / Spacing 2, click on the name of the required
     Point Spacing in the Tree View, and then click on Apply back in the Details View.

The figure below shows a Line Control on a 1 m cube, with Length Scale 0.05 m, Radius of Influence 0.2 m,
and Expansion Factor 1.2.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
70                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Triangle Control

A new Line Control can be created by right-clicking on Controls in the Tree View and selecting Insert >
Line Control. After creation, a Line Control can be renamed, suppressed (made inactive), deleted or duplicated
by right-clicking on its name in the Tree View. Note that if you duplicate a Line Control, its settings are
copied into the new Line Control, but there is no further link between them, i.e., if you change the original
Line Control, then the duplicate will not be updated in any way. If you want to suppress all the Controls in
the model, right-click over Controls and select Suppress.

Once a Line Control is created and is valid, then if you click on its name in the Tree View, the Point Spacing
that it refers to will be highlighted, and a small graphic similar to the one shown below will appear at the
location of the Line Control.




In this graphic, the red line shows you where the line is located. The inner spheres (green in the picture)
show you the mesh Length Scale at that point, and the outer spheres (blue) show you the Radius of Influ-
ence. If the Radius of Influence is zero, then the green spheres will not show up separately.

To view all Controls together, select the Controls entry in the Tree View. All Controls will then be highlighted
in the Graphics window.

Triangle Control

A Triangle Control controls the mesh spacing in a region defined by a prismatic volume between three
spheres.




You must specify a Point location and a Point Spacing (p. 68) for each of the three points needed to define
the triangle. The triangle is formed from the three lines which join up the points, regardless of where the
model faces are.

Each of the three points which form the triangle can have different Point Spacings, which means different
settings of Length Scale, Radius of Influence, and Expansion Factor by selecting different Spacing Definitions
to apply at each point. Where the settings are different, the three values are linearly blended as you move
around the triangle.

The items you need to specify for a Triangle Control are:

 •   Point 1 / Point 2 / Point 3 - You can select points for the Control by selecting vertices from the model,
     selecting arbitrary points on the model faces or by specifying coordinates. See Point Selection (p. 13)
     for details.
 •   Spacing Definitions - If you want to specify the same Point Spacing (p. 68) for all three points, set
     Spacing Definitions to Uniform. If you want to specify a different Point Spacing (p. 68) for each point,
     set Spacing Definitions to Individual.
 •   Spacing / Spacing 1 / Spacing 2 / Spacing 3- Select a Point Spacing (p. 68) which defines the mesh
     attributes. If you selected to set one Point Spacing for all three points, then the selection you make for

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                            71
Meshing Features

     Spacing will apply to all the points; if you selected to set a different Point Spacing for each point, then
     you must separately select a Spacing 1, Spacing 2 and Spacing 3 to apply to Point 1, Point 2 and Point
     3 respectively. To make the selection, click in the box next to Spacing / Spacing 1 / Spacing 2 / Spacing
     3, click on the name of the required Point Spacing in the Tree View, and then click on Apply back in
     the Details View.

The figure below shows a Triangle Control on a 1 m cube, with Length Scale 0.05 m, Radius of Influence 0.2
m, and Expansion Factor 1.2.




A new Triangle Control can be created by right-clicking on Controls in the Tree View and selecting Insert
> Triangle Control. After creation, a Triangle Control can be renamed, suppressed (made inactive), deleted
or duplicated by right-clicking on its name in the Tree View. Note that if you duplicate a Triangle Control,
its settings are copied into the new Triangle Control, but there is no further link between them, i.e., if you
change the original Triangle Control, then the duplicate will not be updated in any way. If you want to
suppress all the Controls in the model, right-click over Controls and select Suppress.

Once a Triangle Control is created and is valid, then if you click on its name in the Tree View, the Point
Spacing that it refers to will be highlighted, and a small graphic similar to the one shown below will appear
at the location of the Triangle Control.




In this graphic, the red triangle shows you where the triangle is located. The inner spheres (green in the
picture) show you the mesh Length Scale at that point, and the outer sphere (blue) shows you the Radius
of Influence. If the Radius of Influence is zero, then the green spheres will not show up separately.

To view all Controls together, select the Controls entry in the Tree View. All Controls will then be highlighted
in the Graphics window.

Periodicity

Some CFD simulations can make effective use of periodic pair boundary conditions, which force the flow
leaving at one face to re-enter at that face's equivalent in the periodic mapping. The ANSYS CFX Solver is
capable of making more accurate calculations on this type of boundary condition if the mesh on each face
in the periodic boundary is identical to the mesh on the equivalent face in the periodic mapping. The use
of Periodicity allows you to generate identical meshes for faces that will later be specified as part of a peri-
odic boundary condition in the simulation set-up. This is achieved by the specification of Periodic Pairs in


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
72                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Periodic Pair

CFX-Mesh. When you create a Periodic Pair, you supply two faces (or lists of faces) and a transformation
which maps one face (or list) onto the other face (or list). The mesh on these two faces (or lists of faces) is
then constrained to be identical.
 Periodic Pair
 Geometry Requirements for Periodic Pairs
 Mesh Generation Process for a Periodic Pair
 Extruded Periodic Pair

Periodic Pair

To define a Periodic Pair, right-click on Periodicity in the Tree View and choose Insert > Periodic Pair. The
use of Periodic Pairs is described in Periodicity (p. 72).

You must specify the following items for the Periodic Pair definition:

 •   Location 1 - Select a face or a set of faces of the model from the Graphics window. You can either select
     faces directly from the Graphics window, or select a Composite 2D Region from the Tree View. In either
     case, all the faces selected must be on the external boundary of the model and must not be included
     in an Inflated Boundary.
 •   Location 2 - Select a face or a set of faces of the model from the Graphics window. The faces must be
     related to those selected for Location 1 as described in Geometry Requirements for Periodic Pairs (p. 74).
     Again, you can either select faces directly from the Graphics window, or select a Composite 2D Region
     from the Tree View.
 •   Periodic Type - This can either be set to Translation or Rotation. If Translation is selected, then in
     most cases no further input is required. If, however, Rotation is selected, then you must specify the axis,
     by specifying any two points on it. You can select the points by selecting vertices from the model, se-
     lecting arbitrary points on the model faces or by specifying coordinates. See Point Selection (p. 13) for
     details.
 •   Translation Vector - In certain cases, CFX-Mesh cannot determine automatically what the translation
     vector for a translational periodic pair is. In these cases, you will be asked to supply the translation
     vector for the Periodic Pair explicitly. You should specify the translation vector which moves the faces
     in Location 1 to those in Location 2.
 •   Angle of Rotation - In certain cases, CFX-Mesh cannot determine automatically what the rotation angle
     for a rotational periodic pair is. In these cases, you will be asked to supply the rotation angle for the
     Periodic Pair explicitly. You should specify the angle which rotates the faces in Location 1 to those in
     Location 2, using the right-hand rule. The vector for the rotation axis is the vector between the specified
     Point 1 and Point 2. Only angles greater than zero are permitted. If your setup requires the use of an
     angle less than zero, then switch Point 1 and Point 2 to reverse the rotation axis. See the picture below.




After creation, a Periodic Pair can be renamed, suppressed (made inactive) or deleted by right-clicking on
its name in the Tree View. If you want to suppress all the Periodic Pairs in the model, right-click over Peri-
odicity and select Suppress.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                         73
Meshing Features

When a Periodic Pair has been created, then if you click on its name in the Tree View, the faces it is using
will be highlighted. In addition, if the Periodic Pair is rotational, the axis of rotation will be shown as a
highlighted line.

More than one Periodic Pair can be created, as required.

Geometry Requirements for Periodic Pairs
Strict rules regarding the location and topology of faces in the Periodic Pair (p. 73) are enforced. For a valid
Periodic Pair, the following must be true:

 •    Each face in the Location 1 face list must map to an equivalent face in the Location 2 face list under
      either a rotation or translation.
 •    The mapping must be the same for each pair of faces.
 •    Each vertex on each face in Location 1 must map to an equivalent vertex on the equivalent face in
      Location 2 under the same mapping.
 •    Multiple faces can be selected for each of Location 1 and Location 2, provided each face in the Location
      1 face list maps onto a face in the Location 2 face list using the specified transformation.

Both the topology and location of the faces is checked to ensure that they are valid through the transform-
ation specified in the Details View. The transformation or Periodic Type can either be Translation by a fixed
vector or Rotation.

If it is not possible to conform to these rules for your geometry, then you should create standard Composite
2D Regions for the periodic faces (one for each half of the periodic pair). You will then be able to make a
periodic boundary using these faces when setting up your CFD simulation, but the mesh will not be
identical between the faces, which will reduce the accuracy of the ANSYS CFX solver on these boundaries.

Mesh Generation Process for a Periodic Pair
When a Periodic Pair (p. 73) has been specified, the surface mesher generates a surface mesh on all the faces
in the Location 1 list using all the available Control and Spacing information. It then uses the transformation
to map the mesh to the faces in the Location 2 list. These then form the basis for the remaining surface
mesh generation.

It is possible for Controls (p. 68) to affect the mesh in unexpected locations when Periodic Pair regions are
used. Controls originally located outside a Solid Body can be copied into the Body through the transformation
and affect the local face and volume mesh length scale.

The process which the mesher uses to generate mesh on periodic faces is as follows:

 1.    The faces are checked with the transformation.




 2.    Controls are mapped using this transformation.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
74                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Inflation




 3.   A surface mesh is produced for Location 1.




 4.   The surface mesh for Location 1 is mapped to Location 2.




 5.   The remaining faces are meshed.




Extruded Periodic Pair
An Extruded Periodic Pair is a specific example of a more general Periodic Pair. It is used to define the
transformation when using the Extruded 2D Mesh capability. More details about the Extruded Periodic Pair
and the rules for its creation can be found in Extruded 2D Meshing (p. 90).

Inflation

In near-wall regions, boundary layer effects give rise to velocity gradients which are greatest normal to the
face. Computationally-efficient meshes in these regions require that the elements have high aspect ratios.
If tetrahedra are used, then a prohibitively fine surface mesh may be required to avoid generating highly
distorted tetrahedral elements at the face.

CFX-Mesh overcomes this problem by using prisms to create a mesh that is finely resolved normal to the
wall, but coarse parallel to it. The mesher can use the local face element normals to 'inflate' 2D triangular
face elements into 3D prism elements at selected walls or boundaries. You can control the creation of these
elements and determine their size and distribution in near-wall regions.

The figures below show the inflated mesh region and the transition between the inflation mesh and the
tetrahedral mesh.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                     75
Meshing Features




You can set different inflation parameters for different faces. When two inflated faces meet at a common
edge and use different inflation heights, the heights are smoothed.

To apply inflation to any face in the model, you must define an Inflated Boundary (p. 81) which includes
that face. The Inflation process is controlled by a global set of parameters (located under Inflation in the
Tree View), as well as the parameters set for an individual Inflated Boundary. These are described in:

 •   Inflation - Details (p. 76)
 •   Inflated Boundary (p. 81)

Inflation can be applied to all ordinary boundaries but not to boundaries specified as a Periodic Pair (p. 73).
Inflation also can be applied to faces which are internal to the region to be meshed, and you can choose
separately to inflate off either side of the face. How to do this is described in 2D Regions and Faces (p. 57).

Inflation - Details

The following parameters are available for Inflation (p. 75) and provide global control over all Inflated
Boundaries. All can be set using the Details View for the Inflation object in the Tree View.

 •   Number of Inflated Layers - This controls the number of inflation layers. If First Layer Thickness is
     used to specify the thickness of the inflation layer, then this is a maximum number of inflation layers.
     Otherwise, it will be the actual number of inflation layers, except in places where layers are removed
     locally for reasons of improving mesh quality (e.g., where inflation layers would otherwise collide with
     each other). The Number of Inflated Layers is restricted to be no more than 100 and the default is 5
     layers.
 •   Expansion Factor - The relative thickness of adjacent inflation layers is determined by a geometric ex-
     pansion factor. Each successive layer, as you move away from the face to which the Inflation is applied,
     is approximately one Expansion Factor thicker than the previous one. Expansion Factors must be set to
     between 1.0 and 1.5.
 •   Number of Spreading Iterations
 •   Minimum Internal Angle
 •   Minimum External Angle
 •   Inflation Option - This option controls how the inflation height is specified. The two options are:
     –   First Layer Thickness


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
76                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Inflation - Details

      –   Total Thickness

The remaining parameters are dependent on which Inflation Option is chosen and are described in First
Layer Thickness and Total Thickness respectively.

First Layer Thickness
You can select this option and specify a height for the first prism layer by selecting First Layer Thickness
as the Inflation Option on the Details View for Inflation. This option does not control the overall height of
the inflation layers, but creates prisms based upon the first layer thickness, Expansion Factor and Number
of Inflated Layers (all set on the Details View for Inflation). This method of inflation creates a smoother
transition from the inflated prism mesh elements to the tetrahedral mesh elements than the alternative,
which is to set the Inflation Option to Total Thickness (p. 79).

The first layer thickness can be specified in two alternative ways by using the Define First Layer By setting.
The two options are:

 •    First Prism Height - This option allows you to specify the first layer thickness directly by setting the
      First Prism Height. The First Prism Height must be less than the Maximum Spacing set under Default
      Body Spacing.
 •    y+ - This option allows you to specify the first layer thickness in terms of a target y+ value, given the
      Reynolds number and a Reference Length. You must supply the specified y+ (∆y+), Reynolds Number
      (Re) and Reference Length (L). The first layer thickness (∆y) is then calculated using the following for-
      mula:


      The motivation for and derivation of this equation can be found in the ANSYS CFX online help in the
      ANSYS CFX-Solver Modeling Guide under the section titled “Guidelines for Mesh Generation”.

      For your information, CFX-Mesh displays the calculated first layer thickness directly underneath the
      Reference Length specification, although you cannot alter this directly.

The process used for creating the layers of prisms when using the First Layer Thickness option (with Extended
Layer Growth set to No) is as follows:

 1.    Put a single layer of prisms against the faces of the inflated boundary, of a height equal to the first
       layer thickness.
 2.    Check the aspect ratio of the prisms (ratio of height to base length). Where this is unity or the height
       is already greater than the base length, stop adding prisms. Where the height is still less than the base
       length, add another layer of prisms of height calculated by multiplying the height of the previous
       layer by the Expansion Factor.
 3.    Repeat step 2 until all the prisms have a height approximately equal to the base length, or until the
       Number of Inflated Layers setting is reached (this setting is used as a maximum number of inflated
       layers).

If you set Extended Layer Growth to Yes, then you can carry on adding prisms even after the aspect ratio
has reached 1. The prisms are added with a height equal to the base length, until the Number of Inflated
Layers is reached. The following two pictures show the difference.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                               77
Meshing Features




The upper picture shows the situation where Extended Layer Growth is set to No. Although the Number
of Inflated Layers was set to 20, only 14 layers have been created, because unit aspect ratio was reached.
The lower picture shows the situation where Extended Layer Growth is set to Yes. The extra 6 layers have
now been added, all with a height equal to their base length.

It is recommended that you examine the mesh wherever possible to allow you to visualize the extent of the
inflation and the quality of the transition from the prisms to the tetrahedral elements. You can view the in-
flated mesh (and so see the extent of the inflation) by using a Preview Group (p. 97). The Details View for
Preview allows you to specify exactly how you view the inflated mesh. The full volume mesh can be viewed
in CFD-Post.

The following two images help to demonstrate the effect of enabling the First Layer Thickness option. The
first image uses default values and the Total Thickness option, and the second uses a specified First Prism
Height.




The following two images help to demonstrate the effect of combining Controls (p. 68) with a specified First
Prism Height. The first image uses default values and the Total Thickness option with the Point Control, and
the second uses a specified First Prism Height.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
78                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                      Inflation - Details




An additional option is Layer by Layer Smoothing, which by default is set to No. This option allows prisms
to grow out normal (orthogonal) to the face. The layer normals and heights are then progressively smoothed,
during the creation of each layer, to maximize the number of layers obtained. Layer by Layer Smoothing
can only be employed when the Inflation Option is set to First Layer Thickness. Note that invoking Layer
by Layer Smoothing will result in longer mesh generation times as the smoothing process is applied on each
prism layer rather than just the once that happens by default.

                                                    Layer by Layer Smoothing off




                                                    Layer by Layer Smoothing on




Total Thickness
You can select this option by selecting Total Thickness as the Inflation Option on the Details View for In-
flation.

With this option enabled, the total thickness of the inflation is controlled by the Thickness Multiplier, the
local element edge length and the Maximum Thickness,

      where the local element edge length is determined by the Face Spacing (p. 64) and Controls (p. 68), and
      the Maximum Thickness is set individually for each Inflated Boundary (p. 81).

This method of inflation creates a less smooth transition from the inflated prism mesh elements to the tet-
rahedral mesh elements than the alternative, which is to set the Inflation Option to First Layer Thick-
ness (p. 77). However, the number of inflated layers is more constant, and you can have some control over
the height of the inflation layers on a face-by-face basis, given that the Maximum Thickness parameter can
be specified separately for each individual Inflated Boundary.

The process used for creating the layers of prisms when using the Total Thickness option is given below:

 1.     Calculate the total thickness of the inflation layers as follows:

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                                               79
Meshing Features

      a.   Multiply the Thickness Multiplier by the local element edge length.
      b.   Where this is less than the specified Maximum Thickness, then this gives the total thickness of
           the layers.
      c.   Where this is greater than the specified Maximum Thickness, then the Maximum Thickness is taken
           to be the total thickness of the layers.
 2.   Use the specified Number of Inflated Layers and Expansion Factor to calculate the height of each layer,
      given the total thickness that has just been calculated.

If the element edge length changes in the region of the inflation layer, e.g., due to a Control, then the inflation
thickness will not be constant over the inflated face. The figure below shows what happens to the inflation
thickness in the vicinity of a Point Control.




Additionally, sometimes inflation layers may be removed (for example, where the inflation layers from two
different faces would otherwise collide) and this will also cause the total thickness of the inflation layer to
decrease.

Some comparisons between the effect of choosing the Total Thickness option and choosing the First Layer
Thickness option are shown in First Layer Thickness (p. 77).

Advanced Quality Checking
There are three controls associated with the quality of the resulting prism elements in the inflated layers.
The three controls are set on the Details View for Inflation. In general, you will not need to change these.

Number of Spreading Iterations - This governs how far the effects of deleted elements propagate. By default
it is set to zero and only the original elements marked for deletion will actually be deleted. However by in-
creasing this value, neighboring elements are also marked for deletion. The value specifies the number of
layers of neighboring elements that are also deleted. It cannot be set to above 10.




For adjacent inflation boundaries where the relative gap between inflation elements is small, interstitial
tetrahedral elements can become distorted. Increasing the number of spreading iterations reduces the
probability of this occurring, although the default settings do not usually require modification.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
80                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Inflated Boundary

Minimum Internal Angle - This governs the minimum angle that is allowed in the triangular face of a prism
nearest to the surface before it is deemed to be of unacceptable quality and marked for deletion. The default
value is 2.5 degrees but you may want to increase this if you are having problems with high aspect ratio
elements adjacent to inflated layers. You must set a value between 0.0 and 40.0 degrees.

Minimum External Angle - This governs the minimum angle that is allowed in the triangular face of a prism
farthest from the surface before it is deemed to be of unacceptable quality and marked for deletion. The
default value is 10 degrees but you may want to increase this if you are having problems with high aspect
ratio elements adjacent to inflated layers. You must set a value between 0.0 and 40.0 degrees. This parameter
controls the minimum angle in a triangular face seen by the tetrahedral volume mesher: triangles containing
small angles are more difficult to create tetrahedra on and therefore increasing this parameter will increase
the reliability of the volume mesher.

Inflated Boundary

The creation of an Inflated Boundary is how you specify which faces you want Inflation (p. 75) to apply to.
There are some limitations on the topology that you can have for the inflation process to work well.

When creating an Inflated Boundary, you must specify two things:

 •   Location - Select the face(s) of the model from the Graphics window. You can either select the faces
     directly from the Graphics window, or select a Composite 2D Region from the Tree View. A face cannot
     be in more than one Inflated Boundary, and it may not be in both an Inflated Boundary and a Periodic
     Pair (p. 73). If you have multiple Solid Bodies in your geometry, then you should read the information
     on the difference between faces and 2D Regions to understand how you can apply Inflation to the faces
     which form the boundaries between the bodies and determine which side(s) of these faces have Inflation.
 •   Maximum Thickness - Set the Maximum Thickness for the whole inflation layer. The way that this
     parameter is used is described in Total Thickness (p. 79). It must be set to a value less than the Maximum
     Spacing set under Default Body Spacing. The parameter is not used if the Inflation Option is set to First
     Layer Thickness in the Inflation - Details (p. 76).

A new Inflated Boundary can be created by right-clicking on Inflation in the Tree View and selecting Insert
> Inflated Boundary. After creation, an Inflated Boundary can be renamed, suppressed (made inactive) or
deleted by right-clicking on its name in the Tree View. If you want to suppress all the Inflated Boundaries
in the model, right-click over Inflation and select Suppress.

An inflated boundary can also be created on any internal face; this includes faces that are intended to be
Thin Surfaces. Inflation will not occur on an exposed edge of such a face, as such the inflation layers will be
gradually reduced to zero as the mesh approaches the exposed edge nodes.




You can also choose to inflate only one side of a face that will be used as a Thin Surface. How to do this is
described in 2D Regions and Faces (p. 57).




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                             81
Meshing Features




There are some considerations to make when setting up the Inflated Boundary, particularly when setting
the Maximum Thickness (and not using First Layer Thickness):
 Inflating Between Thin Gaps
 Inflating the Inside Walls of Cylindrical Pipes

Inflating Between Thin Gaps
When using the Total Thickness (p. 79) option from the Inflation Details, care must be taken when inflating
from faces which are close but not touching. If the Thickness Multiplier is set to 1 (the default) and the
Maximum Thickness is set to anything larger than the local mesh length scale on the faces in question, then
the total thickness of the inflation layer is approximately equal to the local length mesh scale. In this case,
if you ensure that the local length scale is less than a quarter of the gap thickness then this will allow inflation
to be performed between the gaps in a way that leaves a sufficient gap for the volume mesher to fill the
remaining void with good quality tetrahedra.




If you change the setting of the Thickness Multiplier and/or the Maximum Thickness, then you will have to
ensure that enough of a gap remains between the inflation layers for the volume mesher to be able to fill
the remaining void with good quality tetrahedra.

The refinement of the surface mesh in order to fulfill this criteria can be undertaken automatically using
Surface Proximity (p. 85), and the default setting of four elements across the gap satisfies exactly this criteria.

Inflating the Inside Walls of Cylindrical Pipes
If you inflate the inside walls of a cylindrical pipe then there are two potential problems:

 •   The inflated layers will grow towards each other and eventually collide on the axis of the cylinder. Even
     if they stop short of colliding they will leave a narrow cylindrical void that must be filled by the volume
     mesher.
 •   The quality of the exposed element faces on the inflated layer deteriorates as the thickness of the inflated
     layer grows. The face topology of the inflated triangulated face is the same as the original one so the
     exposed triangles have a greater aspect ratio.

If the inflation thickness is too great then the resulting void can be difficult to mesh and can lead to either

 •   volume meshing failure, or,
 •   high aspect ratio elements in the volume mesh.

When using the Total Thickness (p. 79) option in the Inflation Details View, then provided that the Thickness
Multiplier is set to 1 (the default) and the Maximum Thickness is set to something larger than the local mesh



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
82                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Stretch

length scale on the faces which form the cylinder, then the total thickness of the inflation layer is approxim-
ately equal to the local mesh length scale.

A simple calculation shows that in this case, the inflated layers will not meet in the middle as long as there
are at least seven equal sub-divisions around the circumference of the pipe. For a more typical value of sub-
divisions (i.e., 12 or more), it will also guarantee that the resulting void is not too thin and that the exposed
faces are of a reasonable quality.




If you do encounter problems, there are a number of possible solutions:

 •   Increase the number of sub-divisions around the circumference of the pipe. This can be done by applying
     a Face Spacing (p. 64) to the faces of the cylinder.
 •   Modify the Maximum Thickness of the inflated layers on these faces to restrict their growth. This can
     be done in the Details View of the Inflated Boundary (p. 81) that they are part of.
 •   Increase the value of the Minimum External Angle. This will ensure that any prismatic elements with a
     high aspect ratio triangular face are removed from the inflated layer. The parameter can be changed
     using the Details View for Inflation (p. 75).
 •   Increase the Number of Spreading Iterations. This will increase the number of layers that are removed
     when a collision is detected and should leave a larger gap. The parameter can be changed using the
     Details View for Inflation (p. 75).

Stretch

Stretch can be used to expand or contract the mesh elements in a particular direction. In practice, the geometry
is expanded by the specified factors, meshing takes place and then the geometry is contracted back to its
original size.

The Stretch object is present in the Tree View by default. Three items are required to specify the stretch:

 •   Stretch in X - Stretch in the X-direction (default is 1.0)
 •   Stretch in Y - Stretch in the Y-direction (default is 1.0)
 •   Stretch in Z - Stretch in the Z-direction (default is 1.0)

The maximum and minimum stretches allowed are 0.2 and 5.0 respectively. Stretch factors below 0.6 are
not recommended.

The following pictures show the effect of stretching.

Before stretching:




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                   83
Meshing Features




After stretching:




                                Stretch in X = 1.0                                                           Stretch in X = 0.5
                                Stretch in Y = 1.0                                                           Stretch in Y = 3.0
                                Stretch in Z = 2.0                                                           Stretch in Z = 1.0

When a stretch factor is used, the effective influence of a Point Control (p. 69), which is treated as a spherical
mesh control whilst meshing takes place, will NOT be modified to elliptical. Hence a Point Control will appear
to influence an elliptical region when the mesh is examined; this is caused by the modified influence of the
mesh control not being mapped between stretched and non-stretched space. A Line Control (p. 70) and
Triangle Control (p. 71) will be affected in a similar way.

Stretch cannot be used if the Extruded 2D Meshing option is enabled. Any stretch factors set will be ignored.

Proximity

The Proximity settings control automatic refinement of the mesh when edges or faces are found to be in
close proximity to other edges or faces, but not connected. There are two types of proximity setting:
 •   Edge Proximity (p. 84)
 •   Surface Proximity (p. 85)

Edge Proximity is ON by default, but Surface Proximity is OFF.

Edge Proximity
When Edge Proximity is enabled, your model will be examined for locations where relatively small mesh
elements are used on a curved face in close proximity to relatively large coarse elements on a flat face. In
these locations, the coarse elements will be automatically refined to improve the model in this region.

The effect of using Edge Proximity is carried over to adjacent faces. This can be seen in the figure below
where the mesh has been refined on the lower face when Edge Proximity is ON.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
84                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Surface Proximity




     Edge Proximity ON               Edge Proximity OFF

There are no user controls for Edge Proximity, other than allowing it to be enabled and disabled. The default
is for it to be enabled.

Edge Proximity is only available when using the Delaunay Surface Mesher (p. 87).

Surface Proximity
When Surface Proximity is enabled, your model will be examined for locations where distinct faces are in
close proximity. The surface mesh will then be automatically modified to reduce the mesh size in regions
where faces are in close proximity and the original mesh does not resolve the gap sufficiently.

When using Surface Proximity, you need to specify two things:

 •    Number of Elements Across Gap - The aim when Surface Proximity is enabled is to have at least the
      number of elements specified by this setting spanning the gap between the faces. We do not recommend
      using a value less than the default of 4. This will allow higher quality inflated (prismatic) and tetrahedral
      volume elements to be created in the gap region. If you use values of 1 or 2, and inflation is applied
      to the faces, then you may encounter meshing problems. The maximum allowed setting is 10.
 •    Maximum Number of Passes - This specifies the maximum number of times that the surface mesher
      will run in order to satisfy the criteria for Number of Elements Across Gap. It must be between 1 and
      10.

The Surface Proximity process requires an initial surface mesh to be generated. The relative proximity of
triangular face elements is then compared with the size of the triangles themselves. If the triangular element
size is greater than 1/n of the gap between the faces, where n is the setting of Number of Elements Across
Gap, then local mesh controls are introduced into the mesh and the surface mesh is modified accordingly.

The process allows the mesh length scales to be reduced by a factor of 2 each time the mesh is modified,
and the process is applied up to a maximum of n times, where n is the Maximum Number of Passes. This
results in the Surface Proximity option potentially reducing an original triangular edge to 1/2n of the initial
length if the maximum reduction in length scale is applied on each pass of the surface meshing. For reference,
a setting of n = 5 gives up to a 1/32 reduction in edge length, and this corresponds to an original triangle
being replaced by approximately 1000 triangles.

Surface Proximity is available for both the Delaunay Surface Mesher (p. 87) and Advancing Front (AF) Surface
Mesher (p. 87). An example of the effect of Surface Proximity is shown below.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                             85
Meshing Features




The surface mesh was created using Angular Resolution as the Face Spacing (p. 64) option. This refines the
mesh on the cylindrical pipes but not the box. It can be seen that the mesh on the cylindrical pipes is con-
siderably finer where the pipes are in close proximity and the same is true where the pipe and box are close.
In the corresponding volume mesh (not shown), the number of volume elements crossing the gap region
is 4.

Caution should be exercised on geometries where one geometrical component intersects a second component
at an acute angle. If Surface Proximity is used in this case, the mesh length scale may be dramatically reduced
in the region of the intersection. It is important, therefore, to introduce a minimum mesh length scale, possibly
using the Minimum Edge Length available when the Angular Resolution option is used for the Face Spa-
cing (p. 64).

Note that Surface Proximity only checks for nearly faces which are in the same Body as each other.

Mesh Options

The following settings are available under the Options part of the Tree View:

 •   Global Mesh Scaling (p. 86)
 •   Surface Meshing (p. 87)
 •   Meshing Strategy (p. 87) (including the choice of 2D or extruded meshing)
 •   Advancing Front and Inflation 3D (p. 88) (including the choice of parallel meshing)

Global Mesh Scaling
The Global Mesh Scaling factor is a property of the whole mesh, and is set using Options settings in the
Tree View.

Every length scale (except for those applied to Face Spacings and Edge Spacings) that you set anywhere in
CFX-Mesh is multiplied by the Global Mesh Scaling factor before meshing takes place. This can be very
useful if you have set up a mesh including several Controls and then want to refine it uniformly without
having to change all of these settings.

The Global Mesh Scaling Factor can be given a value between 0.5 and 2. Making it smaller makes the mesh
length scales smaller, i.e., gives you a larger mesh.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
86                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Meshing Strategy

Only mesh length scales are affected by the Global Mesh Scaling factor. For example, the Radius of Influence
for Controls is not affected. This makes its behavior different to just using Stretch (p. 83) with Stretch in X,
Stretch in Y and Stretch in Z all set to the same values. If you try to scale the mesh using the Stretch
functionality in this way, then all lengths (including Radius of Influence) will be affected.

Note that the Global Mesh Scaling factor is only applied at the meshing stage. For instance, the display of
the size of Controls will show the size as if the Global Mesh Scaling factor is set to 1, although when the
mesh is generated, the actual size of the mesh in the vicinity of the Control will be affected by this factor.

Surface Meshing
Two surface meshers are available in CFX-Mesh:
 Delaunay Surface Mesher
 Advancing Front (AF) Surface Mesher

Delaunay Surface Mesher
Delaunay surface meshing is characterized by its speed and its ability to mesh closed faces. In general it is
recommended that the Delaunay Surface Mesher be used for surface meshing, and this is the default. In
some cases where faces are poorly-parameterized, improved mesh quality may be obtained by using the
Advancing Front (AF) Surface Mesher (p. 87).

The surface mesher used by CFX-Mesh can be changed using the Options settings in the Tree View.

Advancing Front (AF) Surface Mesher
The Advancing Front Surface Mesher is slower than the Delaunay Surface Mesher (p. 87), but for some geo-
metries it can be more robust and may produce a higher quality mesh. It is not possible to mesh closed
faces using the AF Surface Mesher. Edge Proximity and Edge Spacings cannot be used with the AF Surface
Mesher.

The surface mesher used by CFX-Mesh can be changed using the Options settings in the Tree View.

Meshing Strategy
The Meshing Strategy option, set on the Details View for Options in the Tree View, controls the global be-
havior of the mesher. This setting has fundamental implications for the type of meshing which takes place.
The following options are available.

 •   Advancing Front and Inflation 3D - This is the default choice of meshing strategy. This meshing
     strategy creates a 3D mesh consisting of tetrahedra, with prisms and pyramids if Inflation (p. 75) is used.
     Most models will require the use of this meshing strategy.
 •   Extruded 2D mesh - This meshing strategy allows you to generate a 2D or simple extruded mesh. It is
     only applicable for geometries (or parts of geometries) which can be created by a rotation or translation
     of a collection of faces. It generates a mesh consisting of prisms, with hexahedra if Inflation (p. 75) is
     used.

These options are described in more detail below:

 •   Advancing Front and Inflation 3D (p. 88)
 •   Extruded 2D Meshing (p. 90)




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                            87
Meshing Features

Advancing Front and Inflation 3D
Advancing Front and Inflation 3D is the default meshing strategy, creating a 3D mesh consisting of tetrahedra,
with prisms and pyramids if Inflation (p. 75) is used. Most models will need to use this strategy. If this is se-
lected (on the Details View for Options in the Tree View), then you have a further choice of your Volume
Meshing method. Both methods use the Advancing Front Volume Mesher and will produce essentially the
same mesh. The two choices are:

 •   Advancing Front - This is the default choice for volume meshing. It uses the Advancing Front Volume
     Mesher to generate a mesh using a single processor on your local machine (the machine which is running
     ANSYS Workbench).
 •   Parallel Advancing Front - This choice uses the Advancing Front Volume Mesher to generate a mesh
     using more than one process on both your local machine and other machines if desired. You may wish
     to use this if you are generating a large mesh and want to speed up the mesh generation process when
     more than one processor is available, or to overcome the memory limitations of a single process.

The Advancing Front Volume Mesher is described in Advancing Front Volume Mesher (p. 88), and using it in
parallel is described in Parallel Volume Meshing (p. 88).

Advancing Front Volume Mesher
The Advancing Front Volume Mesher is the default volume mesher in CFX-Mesh. It includes Inflation (p. 75),
which is used for resolving the mesh in the near wall regions to capture flow effects for viscous problems.
The Advancing Front Volume Mesher will rapidly generate a mesh consisting of tetrahedra (and prisms and
pyramids if Inflation (p. 75) is used), with low memory usage.

When the volume mesh of tetrahedral elements (together with prismatic and pyramidal elements if Inflation
is used) is generated, it is written to the CFX Mesh file.

Parallel Volume Meshing
When using Advancing Front and Inflation 3D (p. 88) as the Meshing Strategy (p. 87) (under Mesh Options (p. 86)
in the Tree View), you can use Parallel Volume Meshing by selecting Parallel Advancing Front for Volume
Meshing. This allows you to generate your volume mesh using multiple processes on the same or different
machines. You may wish to use this if you are generating a large mesh and want to speed up the mesh
generation process, or to overcome the memory limitations of a single process.

Parallel Volume Meshing has been implemented to increase the maximum mesh size that can be created.
You can also speed up mesh generation by running in parallel. A typical speed-up is of the order of 50%
when using 4 processors on a mesh greater than 5 million tetrahedral elements. To achieve a reasonable
speed-up, we do not recommend using less than 500,000 elements per partition for a tetrahedral mesh.

If you select to use the Parallel Advancing Front option, then you must specify the Parallel Meshing option.
The two choices are:

 •   PVM Local Parallel - Generates the mesh in parallel using multiple processes on the same machine
     (your local machine).
 •   PVM Distributed Parallel - Generates the mesh in parallel on multiple processors spread over your
     local machine and other machines. This is a beta feature.

When using Parallel Volume Meshing, the meshing process divides the geometry up into sections (“partitions”)
which are meshed separately (one in each process specified) and then the mesh is consolidated into one


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
88                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                               Advancing Front and Inflation 3D

volume mesh. A volume mesh produced in parallel is indistinguishable from a volume mesh produced in
serial (using only one process). You will NOT be able to see partition boundaries in the mesh.

Partitioning is the process of dividing the geometry into sections (partitions) each to be meshed individually.
To control this process, you must specify how many times the geometry should be divided along each of
the major coordinate axes X, Y and Z, by specifying Number of Partitions in X, Number of Partitions in
Y and Number of Partitions in Z. If you specify Number of Partitions in X to be 2, Number of Partitions
in Y to be 1, and Number of Partitions in Z to be 1, then the geometry is divided along the X-axis, giving
two partitions in total. In general, the product of these three numbers will give the total number of partitions
used for the parallel meshing operation.

In general, it is best to have as few mesh elements intersecting a partition boundary as possible, to minimize
the amount of communication required between processes. This means that if you have a long thin pipe
geometry, then it is best to partition the geometry so that it is divided along the coordinate direction which
is along the length of the pipe, for example.

Although you need to decide how many partitions there should be along each of the three major axes, you
do not need to specify the locations at which the geometry is divided. The location of the partitions in each
coordinate direction is determined automatically, taking into account variations in the mesh length scale,
in order to produce partitions that will each contain roughly the same number of volume elements. This is
important for getting the best speed-up for the number of partitions.

You should not use more partitions than there are processors on the local machine if you want to see a
speed-up in the mesh generation process, since this will cause more than one partition to be assigned to
some processors, resulting in slower volume meshing.

If you are using PVM Distributed Parallel (which uses processors on different machines), then you can use
as many partitions as you have available processors on the different machines. You should also bear in mind
that each processor will be given a similar size of mesh to produce, so adding in an extra processor which
is significantly slower than the others will actually slow the whole meshing process down, since it has to
wait for the slowest processor to finish.

If you are using the PVM Distributed Parallel option for generating your mesh, then you need to specify
which machines you want to use for the meshing process by using the Hosts List option. You can select
                                                                                  ,
any hosts to run on by entering a comma-separated list, e.g., “machine1,machine2” subject to the following
restrictions:
 •   PVM Distributed Parallel is a beta feature.
 •   PVM Distributed Parallel is only supported on machines which are of the same type (e.g., the machines
     in each parallel run must be all Windows machines, all HP machines, all SUN machines or all Linux ma-
     chines).
 •   Each machine you want to run on must have network access to the local machine and must have an
     installation of ANSYS Workbench which includes CFX-Mesh in the same location as the local machine.
 •   Each machine must have been set up to run ANSYS CFX software in parallel.
     –   The rsh service supplied with the ANSYS CFX software (not the ANSYS Workbench software) must
         be installed and available on each machine other than the local (master) machine. The setup of this
         rsh service is described in Installation and Licensing Documentation in the section “Configuring High
                                                                                                  .
         Performance Computing > Configuring ANSYS CFX Parallel > Setting up an rsh Service” Please note
         the relevant security warnings in this section.
 •   Your username must be the same on each machine.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                       89
Meshing Features

 •   Your local machine (the one which you are using to run CFX-Mesh) must be included in the list of ma-
     chines.
 •   Include a host name more than once if you want more than one process on that host.
 •   The total number of hosts selected must equal the number of partitions.

Extruded 2D Meshing
CFX-Mesh has the capability of generating 2D meshes (1 element thick) or simple extruded meshes. 2D
meshes can be used for 2D simulations, and extruded meshes can be used to create a mesh which is more
aligned with the flow, or with fewer elements than the equivalent 3D mesh (for example, if you have a long
thin pipe where there is little variation in the flow variables along the pipe length). In either case, the
method of creating the mesh is the same: you must specify which faces of the geometry the extrusion takes
place between, and then the Extruded 2D mesher generates the mesh on these faces and performs the ex-
trusion between them (more detail is given below). An example of a simple extruded mesh is shown below.

                                                         This image shows a curved pipe, meshed with the default Advan-
                                                         cing Front Volume Mesher, including Inflation.The surface mesh
                                                         is a mixture of triangles and quads, and the volume mesh is a
                                                         mixture of triangular prisms near the walls and tetrahedra in the
                                                         center of the pipe.



                                                         This image shows a curved pipe, meshed with the Extrude 2D
                                                         Mesh option, including Inflation.The surface mesh is a mixture
                                                         of triangles and quads, but the volume mesh is now a mixture of
                                                         hexahedra near the walls and triangular prisms in the center of
                                                         the pipe.




Only certain geometries are suitable for use with this meshing option. The basic requirement is that the
geometry must be capable of being created by taking a set of surfaces and either revolving them about an
axis to form a set of solids, or translating them along a fixed vector to form a set of solids (you do not need
to have actually created the geometry in this fashion for Extruded 2D Meshing to work). See Geometry Re-
quirements for Extruded 2D Meshing (p. 94) for more details.

To enable the Extruded 2D mesher, set Meshing Strategy (under Options in the Tree View) to Extrude 2D
Mesh. When you make this setting, then any Periodic Pairs currently in the Tree View are removed and re-
placed by a single Extruded Periodic Pair (p. 93) entry. You use the Extruded Periodic Pair entry to define
the faces for the extrusion, and the transformation between them. (If you later set the Meshing Strategy
back to Advancing Front with Inflation 3D then the original Periodic Pairs are restored and the Extruded
Periodic Pair is removed.)
 Extruded 2D Meshing Options
 Extruded Periodic Pair
 Geometry Requirements for Extruded 2D Meshing
 Mesh Generation Process for Extruded 2D Meshing




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
90                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Extruded 2D Meshing

Extruded 2D Meshing Options
Once Extruded 2D Meshing has been enabled (by setting Meshing Strategy, under Options in the Tree
View, to Extrude 2D Mesh), several extra entries appear in the Details View for Options to allow you to
control this process.

 •   2D Extrusion Option - The default setting for this option is Full, and this generates a mesh using the
     full extent of your geometry. However, if you want to generate a 2D mesh (1 element thick) then you
     may not wish to use the full extent of the geometry, but to select a thickness which allows high quality
     mesh elements to be generated. In this case, you can select Partial. When this setting is selected with
     a rotational extrusion, then CFX-Mesh automatically sets the angle of rotation for the extrusion to be
     3 degrees. When this setting is selected with a translational extrusion, then CFX-Mesh automatically
     determines a thickness which is appropriate given the local mesh element sizes. The example below il-
     lustrates this.

                        This image shows the geometry.




                        This image shows the 2D mesh that would be generated using the Full option. Note
                        that the elements have a very high aspect ratio.



                        This image shows the 2D mesh that would be generated using the Partial option with
                        a coarse mesh.The elements have an aspect ratio which is much closer to 1.



                        This image shows the 2D mesh that would be generated using the Partial option with
                        a finer mesh.The elements have an aspect ratio which is still reasonable, and to ensure
                        this, the length of the extrusion is lower than in the previous mesh.


     If you want to control the thickness of the extrusion exactly, then you must create the geometry with
     the appropriate thickness and use the Full option.

     If you select the Partial option, then you are restricted to having just one element thick and none of
     the other options listed below are available.
 •   Number of Layers - This setting allows you to control the number of layers which the extruded mesh
     is divided into.

                                                              Number of Layers set to 10.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                               91
Meshing Features

                                                             Number of Layers set to 20.




•    Distribution - This determines how the mesh elements are distributed along the length of the extrusion.
     It is only relevant if Number of Layers is set to 2 or greater. The options are described in the table
     below.

                                         This image shows the geometry, including which faces are set up to be
                                         Location 1 and Location 2 in the specification of the Extruded Periodic Pair.




                                         This image shows the 2D mesh that would be generated using the Uniform
                                         distribution.The elements are distributed uniformly throughout the extru-
                                         sion.




                                         This image shows the 2D mesh that would be generated using the Sym-
                                         metric distribution.The elements are distributed so that they are clustered
                                         near the ends of the extrusion.The size ratio between successive elements
                                         is determined by the Expansion Factor, described below.




                                         This image shows the 2D mesh that would be generated using the Grow
                                         From Location 1 distribution.The elements are distributed so that they
                                         are clustered near the faces specified as Location 1 for the Extruded Peri-
                                         odic Pair.The size ratio between successive elements is determined by the
                                         Expansion Factor, described below.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
92                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Extruded 2D Meshing

                                          This image shows the 2D mesh that would be generated using the Grow
                                          From Location 2 distribution.The elements are distributed so that they
                                          are clustered near the faces specified as Location 1 for the Extruded Peri-
                                          odic Pair.The size ratio between successive elements is determined by the
                                          Expansion Factor, described below.




 •   Expansion Factor - For the non-uniform Distribution settings, the Expansion Factor determines the
     rate of growth of the element thickness between successive elements. Each element is one Expansion
     Factor bigger than the previous one. Values between 1 and 1.5 are allowed.

Extruded Periodic Pair


An Extruded Periodic Pair is a specific example of the more general Periodic Pair which is used to define the
transformation for Extruded 2D Meshing.

Only one Extruded Periodic Pair is allowed, and this will be created automatically when you activate the
Extrude 2D Meshing option, and removed when you stop using the Extrude 2D Meshing option. An Extruded
Periodic Pair cannot be renamed, suppressed or manually deleted.

You must specify the following items for the Extruded Periodic Pair definition:

 •   Location 1 - Select a face or a set of faces of the model from the Graphics window. You can either select
     faces directly from the Graphics window, or select a Composite 2D Region from the Tree View. In either
     case, all the faces selected must be on the external boundary of the model and must not be included
     in an Inflated Boundary.
 •   Location 2 - Select a face or a set of faces of the model from the Graphics window. The faces must be
     related to those selected for Location 1 as described in Geometry Requirements for Extruded 2D Mesh-
     ing (p. 94). Again, you can either select faces directly from the Graphics window, or select a Composite
     2D Region from the Tree View.
 •   Periodic Type - This can either be set to Translation or Rotation. If Translation is selected, then in
     most cases no further input is required. If, however, Rotation is selected, then you must specify the axis,
     by specifying any two points on it. You can select the points by selecting vertices from the model, se-
     lecting arbitrary points on the model faces or by specifying coordinates. See Point Selection (p. 13) for
     details.
 •   Translation Vector - In certain cases, CFX-Mesh cannot determine automatically what the translation
     vector for a translational periodic pair is. In these cases, you will be asked to supply the translation
     vector for the Extruded Periodic Pair explicitly. You should specify the translation vector which moves
     the faces in Location 1 to those in Location 2.
 •   Angle of Rotation - In certain cases, CFX-Mesh cannot determine automatically what the rotation angle
     for a rotational periodic pair is. In these cases, you will be asked to supply the rotation angle for the
     Extruded Periodic Pair explicitly. You should specify the angle which rotates the faces in Location 1 to
     those in Location 2, using the right-hand rule. The vector for the rotation axis is the vector between
     the specified Point 1 and Point 2. Only angles greater than zero are permitted. If your setup requires
     the use of an angle less than zero, then switch Point 1 and Point 2 to reverse the rotation axis. See the
     picture below.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                               93
Meshing Features




When an Extruded Periodic Boundary has been created, then when you click on its name in the Tree View,
the faces it is using will be highlighted. In addition, if the Extruded Periodic Boundary is rotational, the axis
of rotation will be shown as a highlighted line.

Geometry Requirements for Extruded 2D Meshing
Only certain types of geometry are suitable for meshing using the Extruded 2D Mesher. All geometries used
must satisfy the following conditions:

 •   Each Body in the geometry must be capable of being constructed by taking a single face and either
     revolving it or translating it to define the solid Body.

        You do not need to have actually created the geometry in this fashion for Extruded 2D Meshing to
        work.
 •   To set up the Extruded 2D meshing, you need to define an Extruded Periodic Pair. The transformation
     specified for this Extruded Periodic Pair, which relates Location 1 and Location 2 in the Extruded
     Periodic Pair definition, must match the transformation (revolve or extrude) that could be used to con-
     struct the Body from a face.
 •   If there are multiple Bodies in the geometry, then each one must be capable of being constructed using
     the same transformation. Every Body in the geometry must have faces in both Location 1 and Location
     2 in the Extruded Periodic Pair.
 •   Each face in the Location 1 face list must map to an equivalent face in the Location 2 face list under
     the specified transformation. The mapping must be the same for each pair of faces. Each vertex on each
     face in Location 1 must map to an equivalent vertex on the equivalent face in Location 2 under the
     same mapping. Multiple faces can be selected for each of Location 1 and Location 2, provided each
     face in the Location 1 face list maps onto a face in the Location 2 face list using the specified transform-
     ation.

Some examples are shown below.

                                                     These two examples are the simplest examples of valid geometry
                                                     for extruded meshing.The geometry is constructed from a transla-
                                                     tion or rotation of a single face. Location 1 and Location 2, used
                                                     to define the appropriate Extruded Periodic Pair for the extruded
                                                     mesh, are marked.
                                                     This geometry is valid for extruded meshing as it can be constructed
                                                     by a single translation or revolution of the two end faces (marked
                                                     red and green).The geometry contains two Bodies. Both Location
                                                     1 and Location 2 must be defined to contain two faces, and this
                                                     marked on the diagram.
                                                     This geometry is invalid for extruded meshing with Location 1 and
                                                     Location 2 as marked; it contains two Bodies but neither is construc-
                                                     ted by rotating or translating the end face in the same single
                                                     transformation that relates Location 1 and Location 2. Neither

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
94                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Extruded 2D Meshing

                                                    Body contains faces in both Location 1 and Location 2. Note that
                                                    this geometry would be fine to mesh with the normal Advancing
                                                    Front and Inflation 3D meshing with a Periodic Pair on Location 1
                                                    and Location 2 as shown in the diagram.
                                                    This geometry is invalid for extruded meshing with Location 1 and
                                                    Location 2. If both Bodies are meshed, then this violates the condi-
                                                    tion that geometries with multiple Bodies are only valid for extruded
                                                    meshing if each Body has faces in both Location 1 and Location
                                                    2.You cannot suppress the second body in CFX-Mesh to get around
                                                    this, because the model must always be valid regardless of the state
                                                    of the suppression of the Bodies.

                                                          You could, however, suppress the second body in your CAD
                                                          package and then update the geometry.

                                                             Note

                                                             This geometry would also be invalid for meshing with
                                                             normal Advancing Front and Inflation 3D meshing
                                                             with a Periodic Pair (p. 73) on Location 1 and Location
                                                             2 as shown in the diagram.


                                                    This geometry is invalid for extruded meshing because the cut-out
                                                    from the middle of the geometry means that the geometry cannot
                                                    be constructed by single transformation of faces. However, this
                                                    geometry would be fine to mesh with the normal Advancing Front
                                                    and Inflation 3D meshing with a Periodic Pair on Location 1 and
                                                    Location 2 as shown in the diagram.

Mesh Generation Process for Extruded 2D Meshing
When an Extruded Periodic Pair has been specified, the surface mesher generates a surface mesh on all the
faces in the Location 1 list using all the available Control and Spacing information. It then uses the trans-
formation to map the mesh to the faces in the Location 2 list. These then form the basis for the creation
of the 2D or extruded mesh.

It is possible for Controls (p. 68) to affect the mesh in unexpected locations when Extruded Periodic Pairs
are used. Controls originally located outside a Solid Body can be copied into the Body through the trans-
formation and affect the local face and volume mesh length scale.

The process which is used to generate a 2D or Extruded Mesh is as follows:

 1.   The Extruded Periodic Pair faces are checked with the specified transformation.




 2.   Controls are mapped using this transformation.



                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                               95
Meshing Features




3.   A surface mesh is produced for the face(s) in Location 1.




4.   The surface mesh for Location 1 is mapped to Location 2.




5.   The remaining faces are meshed, using all of the usual meshing settings (e.g., Inflation, Controls). Al-
     though the surface mesh on these faces is not used in the final mesh, this step is necessary to allow
     the appropriate inflation elements to be generated. To avoid wasting large amounts of computing
     time, the mesher actually only creates the necessary parts of this surface mesh rather than the full
     mesh. This is the end of the surface meshing procedure.
6.   The Extruded 2D Mesher then removes the surface mesh from all faces but those in Location 1 and
     Location 2.
7.   The volume mesh is obtained by joining up the equivalent nodes on Locations 1 and 2, taking into
     account the settings for 2D Extrusion Option, Number of Layers and Distribution.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
96                                               of ANSYS, Inc. and its subsidiaries and affiliates.
Previewing the Mesh

The Preview function in the Tree View allows you to preview mesh on a face or faces of your geometry.

Faces are selected by creating a Preview Group (p. 97), in which you can choose whether to generate the
mesh on a few faces or on the entire surface. The Details View for Preview allows you to control how the
mesh is displayed in the Graphics window, including whether or not inflated elements are displayed if you
have set up Inflated Boundaries.
 Preview Group
 Controlling the Display of Surface Mesh

Preview Group

A Preview Group is created to allow you to specify which part of the surface mesh you want to preview, in
order to verify that the applied settings have the desired effect.

Default Preview Group is created automatically. This group contains all of the faces in the geometry and
can be used to view the full surface mesh. As you make changes to your geometry (e.g., through Geometry
Update or by using Virtual Topology) the Default Preview Group is automatically updated to contain all the
faces of the new geometry.

To create a new Preview Group, right-click on Preview in the Tree View and select Insert > Preview Group
. In the Details View, specify the location by selecting 2D Regions to form the group. Only 2D Regions can
be placed in a preview group; you cannot preview the mesh in the volume of a body (away from any faces).
If you want to preview the mesh on an edge, you must add a 2D Region which is bounded by that edge to
a Preview Group.

Once a new Preview Group is created, you can right-click on its name in the Tree View and choose Generate
This Surface Mesh or QuickView This Surface Mesh in order to preview the mesh on the selected faces.
Click on the name of a newly created Preview Group to display the mesh.

 •   Generate This Surface Mesh: generates and displays the surface mesh that will be used in generating
     the volume mesh

     If you are using Inflation (p. 75), Surface Proximity (p. 85) or Face Spacing, then the mesh on each face
     is affected by the mesh on the faces near it, and thus the full surface mesh will always be generated
     behind the scenes (otherwise the displayed surface mesh would not be the same mesh that you would
     get if you asked to create a volume mesh). In this case, you do not save any time by generating the
     mesh in a specific Preview Group using Generate This Surface Mesh as compared to generating the
     full surface mesh using Generate Surface Meshes. Also see Controlling the Display of Surface Mesh (p. 98).
 •   QuickView This Surface Mesh: generates the surface mesh, ignoring the inflation settings, proximity
     and volumetric effects (face/edge spacing). This does not reflect the surface mesh that will be used in
     generating the volume mesh, but is useful in trying to determine appropriate length scales to be specified.



                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               97
Previewing the Mesh

If you change the mesh settings, the mesh will no longer be up-to-date and the Preview Group title appears
with a yellow lightning bolt in the Tree View. You will still be able to view the existing mesh elements, but
the mesh will not reflect your latest settings. To regenerate the mesh in any preview group, just right-click
on its name and choose Generate.

If you have several Preview Groups, rather than regenerating the mesh on each one separately, you can instead
right-click over Preview and choose to Generate Surface Meshes. This will generate the full surface mesh,
and thus update all preview groups. To view the full surface mesh at once, just click on the Default Preview
Group name. The function Generate Surface Meshes is also available from the Meshing toolbar                                         and
in the Main menu under Go.

To hide the mesh, simply click on one of the other objects in the Tree View. To show the mesh again, click
on the Preview Group name. To delete a Preview Group, right-click over its name in the Tree View and select
Delete.

If you are generating a large mesh, you may find that after it has been displayed in ANSYS Workbench, that
the ANSYS Workbench process may be using a lot of memory. This may result in a volume mesh failure due
to a lack of available memory, or may decrease the viewer's respond time. In this case, right-click over Preview
in the Tree View, and select Clear Surface Mesh. This removes the surface mesh from memory. When you
do this you will only be able to view surface meshes again once you have regenerated them.

To see the statistics for the mesh, expand the Preview Group object in the Tree View (by clicking on the
plus sign next to its name) and then click on Mesh Statistics   . The numbers of quads (four-sided surface
elements) and triangles in the mesh is shown in the Details View.

Non-fatal warning or error messages produced by the mesher, will be shown in the Messages window. If a
message concerns a particular face or element, when you click on it, the appropriate face or element will
be highlighted in the Graphics window.

Fatal errors will also produce messages and can accessed in the same way as above. In addition, a pop-up
message will notify you that the meshing operation has failed.

You should note that by default, the surface mesh is displayed, taking into account the presence of any In-
flation Layers. An option to display the mesh before inflation or to display the inflated layers themselves is
available in the Details View for Preview.

If you want to view the volume mesh and 3D elements, you can do so in CFD-Post by loading either the
MSHDB, GTM, CMDB, or Results File.

Controlling the Display of Surface Mesh
To control how the mesh is displayed in the Graphics window, click on Preview in the Tree View and then
edit the parameters in the Details View.

 •   Display Mode - This options controls which components of the mesh are made visible. Choose between:

     –   Wire on Face Mesh - Shows the mesh faces and lines.
     –   Wire Mesh - Shows just the mesh lines.
     –   Face Mesh - Shows just the mesh faces.
 •   Display Mesh - This controls how the surface mesh elements are displayed if you are using Infla-
     tion (p. 75). The table below describes the different options and shows a simple case for each.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
98                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                               Controlling the Display of Surface Mesh

Geometry Be-     The pictures in the right-hand column show a simple, coarsely-
fore Mesh        meshed cube with inflation specified on a single face (shown
Generation       in green in the top picture).




Mesh Before      This option shows the mesh before any inflation is applied.
Inflation        It is the only Display Property available if you have not set up
                 inflation for your model. If you are using inflation, then it can
                 be useful to view this mesh if the inflation process has not
                 worked as expected, since the quality of this uninflated sur-
                 face mesh will affect the quality of the inflated elements.




Mesh After       This option shows the mesh after the inflated elements have
Inflation        been generated. It is the default if you have specified inflation
                 in your model. It shows the surface mesh as it will appear after
                 volume meshing, including the quad (four-sided) surface
                 elements created during the inflation process.




Inflated Front   This option shows the mesh along the top of the inflated
                 elements. If you view this mesh on all faces, you can see the
                 space which the volume mesher has to fill with tetrahedral
                 elements.This can be useful for determining why the volume
                 mesher is having difficulty creating an element or to predict
                 areas where there may be a low quality volume mesh (for in-
                 stance, if there is only a very narrow gap for it to fill).



Inflated Mesh    This option shows only the inflated layers. It is helpful to view
                 exactly how the inflated layers have been generated, to en-
                 sure that the inflation settings selected are what is desired.
                 Note: if the Preview Group selected for display does not
                 contain any inflated surfaces, then no mesh will be displayed.




The Display Mesh parameter is not available if the Extruded 2D Meshing option is enabled. When this
meshing option is used, the surface mesh is always displayed after both the inflation and extrusion
processes have taken place.



                 Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                             of ANSYS, Inc. and its subsidiaries and affiliates.                                   99
Previewing the Mesh

•     Transparency (%) - Choose the transparency of the mesh. 100% means that the mesh is completely
      transparent (i.e., it won't show up) and 0% means that the mesh is completely opaque.
•     Shine (%) - Shine controls how much light is reflected by the faces of the mesh. 0% gives the lowest
      amount of reflection and will result in a matte looking mesh. The amount of light reflected by the mesh
      is also affected by the Shine setting under Geometry in the Tree View. In particular, if Shine under
      Geometry is set to 0%, then the Shine setting under Preview has no effect: the mesh is always displayed
      as matte.
•     Face Color Mode - This controls the color of the faces (if Display Mode is set to show the Face Mesh)
      or lines (if Display Mode is set to show the Wire Mesh). Choose between:
      –   Body - Shows the mesh in the same color as the body.
      –   Uniform - Choose a color for the mesh using the Uniform Color setting. Click on the displayed color
          in the Details View to change it. You can either select one of the predefined colors, or use Define
          Custom Colors to specify the exact color that you require.
      –   Rainbow - Shows the mesh on each face in a different color, chosen to be as different as possible.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
100                                                of ANSYS, Inc. and its subsidiaries and affiliates.
Volume Meshing
 Generating the Volume Mesh
 Saving the Volume Mesh

Generating the Volume Mesh

Once you have finished setting up your mesh, you can generate a volume mesh by right-clicking on Mesh
in the Tree View and selecting Generate Volume Mesh. You can also generate a volume mesh by using the
Meshing toolbar.

Within ANSYS Workbench, a volume mesh can be generated and, by default, will be stored in the Meshing
application database and saved in the Workbench project. When CFX-Pre is linked to a mesh cell in the
project schematic, the mesh data will be transferred automatically. Alternatively, a GTM file can be exported
from CFX-Mesh, which can be imported by CFX-Pre.

For information on how the mesh generation affects the Mesh cell state on the Project Schematic, see
Generating Mesh and Updating the Mesh Cell State in the Meshing Help.

You will not be able to view the volume mesh or any 3D elements (including the prism elements produced
by Inflation (p. 75)) in CFX-Mesh. Instead, after generating a mesh (not writing the mesh to a GTM file), you
can view it in the Meshing application or by loading it in CFD-Post.

To regenerate a mesh, simply right-click on Mesh in the Tree View and choose Generate Volume Mesh.

Non-fatal warning or error messages produced by the mesher, will be shown in the Messages window. If a
message concerns a particular face or element, when you click on it, the appropriate face or element will
be highlighted in the Graphics window.

Fatal errors will also produce messages and can accessed in the same way as above. In addition, a pop-up
message will notify you that the meshing operation has failed.

Saving the Volume Mesh
A volume mesh generated by CFX-Mesh can be stored in two different formats.

 •   MSHDB files (Meshing database files) contain mesh settings as well as mesh data. This file will contain
     the data for all parts of the problem, not only those parts meshed in CFX-Mesh.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               101
Volume Meshing


           Note

           Neither a MSHDB nor a MESHDAT file (which can be exported from the ANSYS Meshing ap-
           plication) can be imported directly into CFX-Pre. The mesh should be imported into CFX-Pre
           within ANSYS Workbench by connecting a CFX system to the Mesh cell and updating the
           contents of the Mesh cell once the connection is formed. Opening CFX-Pre will automatically
           import the mesh data. Closing CFX-Pre will create a CFX file (which can be seen using the
           File View option in ANSYS Workbench) that can be reopened using a standalone version of
           CFX-Pre on any supported platform, not just Windows.


 •    GTM files (CFX Mesh files) store both the mesh data, using double-precision coordinates, and region
      information that is required by ANSYS CFX-Pre. The use of GTM files is recommended for large meshes
      generated using only CFX-Mesh, as they can be imported directly into standalone CFX-Pre. For details,
      see Usage Information for the CFX-Mesh Method for more information about the *.gtm format.

For details on how to set the default file type for volume meshes, see the settings available for writing
volume meshes.

There are three ways to save a volume mesh.

Saving the mesh to a Workbench project file

 •    When you generate a volume mesh within a project and save the project, the mesh can be imported
      into CFX-Pre by dropping a CFX system onto the mesh cell and updating the mesh cell to export the
      mesh data. Saving the project will save the mesh within the project files.

Saving the mesh to a GTM file (default location)

 •    If the volume mesh is automatically written to a GTM file, then no dialog box will appear when the
      mesh has generated. GTM files are automatically saved to a default directory and do not override pre-
      existing GTM files, but instead the filename is incremented to generate a unique name. For details, see
      the GTM File Location setting.

      When you generate and save a volume mesh as a GTM file within a project, the GTM file will not be
      registered within the project. It will be necessary to create a separate Fluid Flow (CFX) or CFX system on
      the schematic and import the GTM file directly into CFX-Pre.

Saving the mesh to a GTM file (user-defined location)

 •    If the volume mesh is written to a user defined GTM file, a Save As dialog box will appear automatically
      when the volume mesh has generated. For details, see the GTM File Location setting.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
102                                                of ANSYS, Inc. and its subsidiaries and affiliates.
CFX-Mesh Options on the Options Dialog Box
The CFX-Mesh options are used to set global preferences for ANSYS Workbench sessions, rather than the
settings for a particular CFX-Mesh database.

You can configure CFX-Mesh options from the Options dialog box as outlined below:

 1.    From the CFX-Mesh main menu, select Tools > Options.

       An Options dialog box appears with the major options listed in the left pane. See Workbench Options
       for details on various major options.
 2.    In the left pane, expand Meshing and select CFX-Mesh Options.

       The CFX-Mesh Options appear in the right pane of Options dialog box:
 3.    In the right pane, change any of the options by clicking directly in the settings field to the right of the
       option. You will see a visual indication corresponding to the type of interaction required in the field.
       These include drop down menus, secondary dialog boxes or direct text entries.
 4.    Click OK to save the changes.

CFX-Mesh Options
The following CFX-Mesh Options appear in the right pane of Options dialog box:

      Assembly Display
      Mesh Display
      Tree Colours
      Properties View
      Geometry
      Mesh Edge Lengths
      Virtual Topology
      Volume Mesh
      Miscellaneous

Assembly Display
 •    View: This determines the geometry display type used in CFX-Mesh at the start of each ANSYS Workbench
      session. The View type can also be changed through the Tools menu and will remain when you open
      or create a new CFX-Mesh database. The View type is not a property of the CFX-Mesh database and is
      not stored in a CFX-Mesh database.

         Shaded Display with 3D Edges - See View Menu (p. 8) for details.
         Wireframe Display - See View Menu (p. 8) for details.

 •    Transparency: This determines the value of transparency that is given to the geometry whenever a
      new CFX-Mesh database is started. The transparency of the mesh is stored in the database and can be
      changed in the Details View for Geometry through the normal CFX-Mesh user interface. See Geometry
      Display (p. 46) for details.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               103
CFX-Mesh Options on the Options Dialog Box

 •    Shine: This determines the value of shine that is given to the geometry whenever a new CFX-Mesh
      database is started. The shine of the mesh is stored in the database and can be changed in the Details
      View for Geometry through the normal CFX-Mesh user interface. See Geometry Display (p. 46) for details.

Mesh Display
 •    Transparency: This determines the value of transparency that is given to the mesh whenever a new
      CFX-Mesh database is started. The transparency of the mesh is stored in the database and can be
      changed in the Details View for Preview through the normal CFX-Mesh user interface. See Controlling
      the Display of Surface Mesh (p. 98) for details.
 •    Shine: This determines the value of shine that is given to the mesh whenever a new CFX-Mesh database
      is started. The shine of the mesh is stored in the database and can be changed in the Details View for
      Preview through the normal CFX-Mesh user interface. See Controlling the Display of Surface Mesh (p. 98)
      for details.

Tree Colours
 •    Normal: This setting determines the normal color of the text in the Tree View.
 •    Dimmed: This setting determines the dimmed color of the text in the Tree View that is used when the
      Tree View is not in focus, i.e., you are entering information in the Details View.
 •    Highlight: This setting determines the text color when a Tree View entry is highlighted; for example,
      Point Spacing will be highlighted if a Point Control that uses that Point Spacing, is selected.

Properties View
 •    Auto Activate Invalid Entries: If this is set to Yes, then an item that is invalid and requires selection
      is opened automatically when you click on an object in the Tree View. For example, if you create a new
      Inflated Boundary, then it requires that you to select a location for the inflation. If Auto Activate is
      turned on, then you can select the required faces from the Graphics window immediately. If Auto Ac-
      tivate is turned off, then you must click next to Location in the Details View before you can selecting
      faces.

      The default setting is Yes. Select No if you want to revert back to the behavior of CFX-Mesh 8.1 or
      earlier.

Geometry
 •    Auto Verify on Change: If you set this to Yes, then every time you perform a Geometry Update or
      Clear Settings operation, the Geometry Check operation is performed on the new setup. This would
      be useful if you were making changes to your geometry and wanted to find out immediately if it was
      invalid or poor, before you did any other operations. The default setting is No.

Mesh Edge Lengths
 •    Adjust 'Default Mesh Scale' on Geometry Change : When you perform geometry update (i.e., if the
      geometry has changed in DesignModeler, and you want to reflect these changes in CFX-Mesh) this
      option will recalculate any default length scales based in the new geometry dimensions. However, any
      settings that you have explicitly made (e.g., inflation layer thickness) will not be modified. See Geometry
      Update for details.
 •    'Default Mesh Scale Factor' : This allows you to customize the default length scales used in CFX-Mesh.
      Currently, there is a built in default face and body spacing. You can apply a factor to this if you find the
      built in default too small or large.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
104                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                           CFX-Mesh Options on the Options Dialog Box

Virtual Topology
•   Automatically Remove Invalidated Virtual Cells: If this is set to Yes (default setting), then every time
    a virtual face or edge is edited to include an existing virtual face (or edge), that virtual entity will auto-
    matically be deleted. If this is set to No, then existing virtual entities cannot be added to a new or ex-
    isting virtual face (or edge).

•   Automatic Edge Merging Tolerance (Degrees): This angle sets the threshold at which the connected
    edges on a newly created virtual face can be automatically merged.

Volume Mesh
•   Volume Mesh Output: The following settings determine how volume mesh is written:

         Add to Workbench project files - volume mesh is merged into Workbench project files
         Write GTM File - volume mesh is written to an external GTM file
         Both Workbench and GTM - volume mesh is merged into the Workbench project and GTM files

    For details, see Saving the Volume Mesh (p. 101) and Usage Information for the CFX-Mesh Method for
    more information about the *.gtm format.

•   Commit Mesh to Workbench project on Generate: This action will automatically commit the generated
    mesh into a Workbench project file when Yes is selected. For large (potentially slow) cases, you can
    choose to turn off this automatic function by selecting No, and manually commit the mesh.
•   GTM File Location: The following settings determine the location of GTM file:

         Automatic - writes the GTM file to the default directory (same directory as used by Workbench
         project files)
         User Defined - writes to a user defined directory

Miscellaneous
•   Frequency of Auto Backup: This determines how often a backup file is written. The options are Fre-
    quently that will back up your CFX-Mesh database after (approximately) every 10 changes to your mesh
    setup, Moderately that will back up after every 20 changes, Infrequently that will back up after every
    40 changes, and Never. The default is Moderately. Additionally, you can choose to backup your database
    just before each meshing action; see below for details.
•   Auto Backup Before Action: In addition to the backups that take place after every so many changes,
    you can also choose to take a backup copy of your CFX-Mesh database immediately before performing
    any meshing action, by setting this option to Yes (the default).
•   Keep Backup Files: If this option is set to Yes, then backup files are not deleted when ANSYS Workbench
    is exited. The default is to delete them.

    Backup files are saved in a directory called <tmpdir>\cfx.cm.vXX.Y\recovery, where <tmpdir>
    is the Folder for Temporary Files, a file management setting available under Workbench Options.
    XX.Y are the numbers automatically chosen by ANSYS Workbench to make the directory name unique.
    If your original .cmdb name was Project.cmdb, then the backup file will be called _Current.cmdb.
    In order to restore these backup files, you should do the following:
    1.    Open a new ANSYS Workbench session. On the Project Schematic, choose to Open an existing file
          and set the filter to look for existing Meshing files. Browse to locate the required backup files in
          the temporary folder.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               105
CFX-Mesh Options on the Options Dialog Box

      2.   Once CFX-Mesh has opened, choose File > Save As... and save the backup files to the name and
           location that you wish to restore them to.
      3.   Close the project without saving it.

           Note

           Do NOT just manually move and rename the files back to where you want them, or CFX-
           Mesh will NOT be able to re-open them.


 •    Show CFX-Mesh Retirement Message: The CFX-Mesh Method has been superseded by the Patch
      Conforming tetrahedron mesh method. The CFX-Mesh Method will be retired in a future release. You
      are strongly encouraged to learn and use the Patch Conforming tetrahedron mesh method instead of
      CFX-Mesh. For these reasons, a warning message will appear when you insert the CFX-Mesh Method
      control or select Mesh> Edit in CFX-Mesh from the Meshing application toolbar. To turn off the message,
      select Tools > Options from the Meshing application main menu, click CFX-Mesh Options on the
      Options dialog box, and change the setting of Show CFX-Mesh Retirement Message to No.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
106                                                of ANSYS, Inc. and its subsidiaries and affiliates.
Troubleshooting
 Common Queries
 Valid and Invalid Values for Parameters, Locations and Names
 Meshing Warning and Error Messages

Common Queries
 Why can the Mesher Fail Trying to Create a Surface Mesh?
 Why can the Mesher Fail Trying to Create a Mesh with Inflation?
 How can I Create a Mesh Greater than 1 km Across?
 How can I Ask to See the Warning Messages that the Mesher Produces?
 Which Part of my Model is Causing the Problem?
 Why do I get Messages About Disk Space when I Have Plenty of Space in my Project Directory?
 What are the Files which CFX-Mesh Produces?

Why can the Mesher Fail Trying to Create a Surface Mesh?
There are several reasons why this could occur:

 1.   You may be trying to mesh Closed Faces (p. 33) with the Advancing Front (AF) Surface Mesher (p. 87),
      which cannot mesh such faces.

      The simplest solution to this problem is to use the Delaunay Surface Mesher (p. 87) which is selected
      by default. If you need to use the AF Surface Mesher, then there are two possible solutions to this
      problem.

      For relatively simple geometries you can recreate your model without closed faces, for example using
      two curved faces to define a cylinder. You can find more help with this in Closed Faces (p. 33).

      For larger, more complicated, or imported models, you can break closed faces into one or more non-
      closed faces using the Split action in DesignModeler to split the Solid Body in such as way as to also
      break the closed face.
 2.   You may be trying to mesh an invalid face topology. Some non-manifold topologies cannot be meshed
      with either surface mesher.

Also see Meshing Warning and Error Messages (p. 111) for additional information on meshing warnings and
error messages.

Why can the Mesher Fail Trying to Create a Mesh with Inflation?
Check your geometry model to make sure adjoining non-inflated faces do not contain two or more edges
which meet at an intermediate edge point.

For tips on how to use the surface meshers most effectively, see Geometry and Topology for the Faces of
Solid Bodies (p. 32).



                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               107
Troubleshooting

How can I Create a Mesh Greater than 1 km Across?
The geometry kernel underlying ANSYS Workbench has a built-in limit of a cube 1 km across, centered on
the origin. DesignModeler will not allow you to generate any geometry feature which touches or extends
beyond this box.

If you want to create a mesh which is larger than this, then we suggest that you generate a scaled-down
version of your geometry and mesh. It is then straight-forward to scale the mesh up again on import into
CFX-Pre.

How can I Ask to See the Warning Messages that the Mesher Produces?
All error, warning and information messages are displayed in the Messages window. This window shows
the history of messages from CFX-Mesh. These can be accessed by selecting a particular message in the left
hand panel and the body of the message will be displayed in the right hand panel.

Which Part of my Model is Causing the Problem?
If a particular part of your model is causing the mesher to fail or to produce warning messages, then by
clicking on the error in the Messages window, any relevant part of the geometry will be highlighted to in-
dicate where the problem has occurred.

Why do I get Messages About Disk Space when I Have Plenty of Space in my
Project Directory?
The meshers work in a temporary directory before writing the CFX Mesh file back into the project directory.
If the temporary directory does not have enough disk space then they cannot complete.

The temporary directory is specified on starting CFX-Mesh for the first time by the TEMP environment variable,
or, if this environment variable is not set, by TMP or TMPDIR, or if neither of these are set, the directory
used is C:\Temp. After the first start-up of CFX-Mesh the temporary directory location is stored in the CFX-
Mesh preferences and these environment variables will not be looked at again unless the stored temporary
directory no longer exists.

You can change the temporary directory by setting an appropriate value for Folder for Temporary Files,
a file management setting available under ANSYS Workbench Options. Changes do not take effect until the
next time CFX-Mesh is started in a new ANSYS Workbench session.

What are the Files which CFX-Mesh Produces?
The files used and produced by CFX-Mesh are as follows:

 •    Project.wbpj - ANSYS Workbench project file.
 •    Project.agdb - DesignModeler geometry file. This is used by DesignModeler and read by the
      Meshing application the first time it is initiated, and during any geometry updates. (If you are not using
      DesignModeler for producing geometry, then you will not have this type of file; instead you will have
      the CAD files from whichever CAD package you are using.)
 •    Project.mshdb - Meshing database. This contains the mesh settings and the volume mesh data
      (when using the Add to Workbench project files option for volume meshing). For details, see Saving
      the Volume Mesh (p. 101).



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
108                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                             Valid and Invalid Parameter Values

 •   Project.gtm - A generic CFX Mesh format. This contains the volume mesh data (when using the
     Write GTM File option for volume meshing). These files can be imported directly into CFX-Pre. The
     .gtm format file is not supported at the Workbench project level.

If you need to contact customer support then all of the files must be provided to allow your problem to be
reproduced, the simplest way to achieve this is to use the Archive option on the File menu in ANSYS Work-
bench.

Valid and Invalid Values for Parameters, Locations and Names
 Valid and Invalid Parameter Values
 Valid and Invalid Locations
 Valid and Invalid Names

Valid and Invalid Parameter Values
Most of the parameter settings which require you to enter a number will only allow you to set numbers
within a particular range. This section lists the valid ranges, with some notes on the reason for the restriction.

Tree Section                                      Parameter                                               Range of Validity
Geometry                                          Transparency (%)                                        0 to 100
Geometry                                          Shine (%)                                               0 to 100
Geometry > Verify Options                         Short Edge Limit                                        above zero
Geometry > Verify Options                         Sliver Factor Limit                                     above 1.0
Geometry > Fix Options                            Short Edge Tolerance                                    below 5% of the maximum ex-
                                                                                                          tent of the geometry
Mesh > Spacing > Default Body                     Maximum Spacing                                         above zero
Spacing
Mesh > Spacing > (Default) Face                   Angular Resolution [Degrees]                            1.0 to 90.0
Spacing
Mesh > Spacing > (Default) Face                   Constant Edge Length                                    below 50% of the maximum ex-
Spacing                                                                                                   tent of the geometry
Mesh > Spacing > (Default) Face                   Expansion Factor                                        1.00001 to 1.5
Spacing
Mesh > Spacing > (Default) Face                   Maximum Edge Length                                     below the maximum extent of
Spacing                                                                                                   the geometry, above the Minim-
                                                                                                          um Edge Length
Mesh > Spacing > (Default) Face                   Minimum Edge Length                                     below 5% of the maximum ex-
Spacing                                                                                                   tent of the geometry
Mesh > Spacing > (Default) Face                   Radius of Influence                                     above zero
Spacing
Mesh > Spacing > (Default) Face                   Relative Error                                          0.000038 to 0.292 (corresponds
Spacing                                                                                                   to between 360 and 4 edges
                                                                                                          round a circle
Mesh > Controls > Point Spacing                   Expansion Factor                                        1.00001 to 1.5
Mesh > Controls > Point Spacing                   Length Scale                                            below 5% of the maximum ex-
                                                                                                          tent of the geometry


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                      109
Troubleshooting

Tree Section                                      Parameter                                               Range of Validity
Mesh > Controls > Point Spacing                   Radius of Influence                                     above zero
Mesh > Periodicity > Periodic Pair                Angle of Rotation                                       -360 to 360 degrees
Mesh > Periodicity > Periodic Pair                Translation Along Axis (all three any real number
                                                  axes)
Mesh > Inflation                                  Expansion Factor                                        1.00001 to 5.0
Mesh > Inflation                                  First Prism Height                                      below 5% of the maximum ex-
                                                                                                          tent of the geometry
Mesh > Inflation                                  Minimum Internal Angle                                  0.0 to 40.0
Mesh > Inflation                                  Minimum External Angle                                  0.0 to 40.0
Mesh > Inflation                                  Number of Inflated Layers                               Greater than 0
Mesh > Inflation                                  Number of Spreading Iterations 0 to 10
Mesh > Inflation > Inflated Bound-                Maximum Thickness                                       above zero
ary
Mesh > Stretch                                    Stretch in X/Y/Z                                        0.2 to 5.0
Mesh > Proximity                                  Elements Across Gap                                     1 to 10
Mesh > Proximity                                  Maximum Number of Passes                                1 to 10
Mesh > Options                                    Global Mesh Scaling                                     0.5 to 2.0
Mesh > Options                                    Number of Layers                                        1 to 10,000
Preview                                           Transparency (%)                                        0 to 100
Preview                                           Shine (%)                                               0 to 100

Valid and Invalid Locations
If CFX-Mesh won't allow you to select the locations that you require (either by selecting from the Graphics
window or selecting a Composite 2D Region from the Tree View), then it will be due to one or more of the
following restrictions:

 •    The location of an Inflated Boundary must not be contained in any other Inflated Boundary or any
      Periodic Pair or Extruded Periodic Pair.
 •    The location of a Periodic Pair must not be contained in any Inflated Boundary or any other Periodic
      Pair.
 •    The location of an Extruded Periodic Pair must not be contained in any Inflated Boundary.
 •    The location of a Composite 2D Region must not be contained in any other Composite 2D Region.
 •    The location of a Face Spacing must not already be contained in any other Face Spacing, except the
      Default Face Spacing.
 •    The locations used to create a Virtual Face must be adjacent to each other (so that the Virtual Face is
      a single continuous entity) and must not form a closed region (e.g., you can combine any five faces of
      a cube to make a Virtual Face but you cannot combine all six).

CFX-Mesh allows you to select any combination of locations from the Graphics window and Tree View and
then checks that the selection does not break any of the rules above at the time when you press Apply in
the Details View. If the new selection does break one of the rules, then the new selection will not be applied
and the contents of the Location will remain as they were. So even if it is only one part of the selection that
breaks the rules, the whole new selection will be reverted.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
110                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                    CAD Edge Referenced n Times by Faces

Sometimes even when your selection of faces for a Virtual Face does not break the rules given above, the
Virtual Face will not be created and the contents of its location will remain as they were. The reasons for
this are described in Virtual Faces (p. 48).

If you have multiple bodies in your geometry, then you should refer to 2D Regions and Faces (p. 57) for more
details on what is valid to apply to 2D Regions which form the two sides of a face.

Valid and Invalid Names
When naming or renaming anything in the Tree View, you must take account of the restrictions on what
names can be used. Any name must start with an alphabetic character, can be any length and can contain
alphabetic characters, numbers, single spaces and underscores. Names are case-sensitive, i.e., “inlet” and
“Inlet” are treated as different. Two named objects of the same type cannot differ by only spaces. For example,
you cannot have two objects of the same type named "Spa cing 1" and "S p acing1".

Meshing Warning and Error Messages
The following error messages may be produced from CFX-Mesh. Note that where specific geometry is referred
to in the message, this will be highlighted in the geometry.
 The Advancing Front Surface Mesher Cannot be Used When Parametrically Closed Surfaces or Curves are Present
 in the Geometry
 CAD Edge Referenced n Times by Faces
 CAD Model Contains Faces with Small Angles
 CAD Vertex Referred to n Times by CAD Face
 Edge is Periodic
 Face for Edge is Periodic
 Face has Less than 2 Edges
 Invalid Periodicity in Faces Detected
 Matching Periodic CAD Vertices Exceed Tolerance
 No Edges Found in Search Box
 Storage Allocation Failed
 Surface is Parametrically Closed
 Surface Mesh has Triangles which are Identical
 There was a Problem Converting the Mesher Output into the GTM Database
 2 Transformations Specified
 Two or More CAD Edges Between Non-inflated Surfaces Meet at a CAD Vertex on an Inflated Surface
 The Volume Mesher Cannot Continue. It is Continually Adding and Removing the Same Elements.
 Zero Length Vector

The Advancing Front Surface Mesher Cannot be Used When Parametrically
Closed Surfaces or Curves are Present in the Geometry
Closed surfaces and curves are described in Closed Faces (p. 33). To mesh a geometry which contains such
surfaces, you cannot use the Advancing Front (AF) Surface Mesher (p. 87) but must instead use the Delaunay
Surface Mesher (p. 87). You can switch between the two meshers by using the Surface Mesher option from
the Mesh Options (p. 86) section in the Tree View.

CAD Edge Referenced n Times by Faces
This is the error message that can result from trying to mesh a geometry with a non-manifold edge.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                111
Troubleshooting

CAD Model Contains Faces with Small Angles
This message occurs when one or more faces contain edges which meet at small angles. It is only a warning
message and your mesh may generate successfully and be of the expected high quality. However, it may
be worth checking the mesh in the region of the face with the small angle to ensure that the quality is what
you expect.

CAD Vertex Referred to n Times by CAD Face
This is the error message that results from trying to mesh a geometry that contains a non-manifold vertex.

Edge is Periodic
If you are using the Advancing Front (AF) Surface Mesher (p. 87), edges of faces that form closed loops must
not be made up of a single curve. See Closed Faces (p. 33) for help on working around this problem.

Face for Edge is Periodic
If you are using the Advancing Front (AF) Surface Mesher (p. 87), two ends of a face may not share the same
curve. See Closed Faces (p. 33) for help on working around this problem.

Face has Less than 2 Edges
The face has less than 2 edges. This usually occurs when a face is closed. This type of face cannot be meshed
with the Advancing Front (AF) Surface Mesher (p. 87).

Invalid Periodicity in Faces Detected

   CAD faces with double periodicity have been detected.
   These are most likely torii or connected components of
   toroidal surfaces. To mesh the problem you must cut these
   surfaces in two to avoid periodicity in at least one
   parametric direction.

This message occurs when the mesher detects a surface which is closed in two directions, such as a torus.
This is invalid geometry and the associated faces are highlighted in the Graphics window. You should elim-
inate the indicated faces, perhaps by splitting it into two parts as suggested in the error message.

Matching Periodic CAD Vertices Exceed Tolerance
This error message can occur if you have a Periodic Pair specified which is not actually periodic in the way
that you specified. For example, your faces may not be quite periodic, or you may have specified the trans-
lation or rotation angle incorrectly (in the few cases where you are asked to supply these). Although CFX-
Mesh will check your periodic specification and will not allow you to set up most invalid cases, it cannot
catch all problems in advance of the meshing stage.

No Edges Found in Search Box
This is an error message generated by the volume mesher. It occurs when there is a problem with the geo-
metry (e.g., mesh length scale is too large to resolve a feature) and you are using Proximity (p. 84) and
Stretch (p. 83). You may be able to avoid the problem by removing or reducing the amount of Stretch.



                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
112                                              of ANSYS, Inc. and its subsidiaries and affiliates.
          Two or More CAD Edges Between Non-inflated Surfaces Meet at a CAD Vertex on an Inflated Surface

Storage Allocation Failed
This message occurs when you are trying to generate a mesh which is too big for your machine's available
memory. You need to either reduce the size of the mesh (by making some of the length scales larger, for
instance), free up or add some more memory to your machine, or mesh on a different machine.

Surface is Parametrically Closed
This occurs when a face is closed. This type of face cannot be meshed with the Advancing Front (AF) Surface
Mesher (p. 87).

Surface Mesh has Triangles which are Identical
CFX-Mesh allows some cone faces to be meshed. However, if the angle at the apex is too small, then this
leads to a degenerate mesh with two triangles back to back at the apex, which can cause this message. The
only workaround is to remove the tip of the cone from the geometry.

There was a Problem Converting the Mesher Output into the GTM Database
The meshers work in a temporary directory before writing the CFX Mesh file back into the project directory.
If the temporary directory does not have enough disk space then they cannot complete, and this message
is one indication that this may the problem. You can change the temporary directory by setting an appro-
priate value for Folder for Temporary Files, a file management setting available under ANSYS Workbench
Options.

This message can also occur if the meshing fails right at the end, when occasionally the file file-
name.gtm.lck (where filename.gtm is the name of the temporary CFX Mesh file) is created and not
removed. After this happens, you will not be able to write to that file location again; you will continue to
get the same error each time you try. The workaround in this case is to remove the file filename.gtm.lck
manually from the directory.

2 Transformations Specified

 Source terms will be made periodic for each
 transformation. This may result in unexpected
 mesh densities occurring.

This warning occurs when you have two or more Periodic Pairs with different transformations. It is there to
warn you that when more than one transformation is in use, Controls (p. 68) will be mapped according to
all of the transformations, and that this can sometimes result in them being applied in locations that you
did not expect. It is recommended that you check the resulting mesh to ensure that it is all as you intended.

Two or More CAD Edges Between Non-inflated Surfaces Meet at a CAD Vertex
on an Inflated Surface
The situation which leads to this warning message is described in Geometry and Topology for the Faces of an
Inflated Boundary (p. 34).




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                               113
Troubleshooting

The Volume Mesher Cannot Continue. It is Continually Adding and Removing
the Same Elements.
This error message usually occurs when the mesh length scale is inappropriate for the geometry or the gap
between inflated layers. Check that the length scales specified will resolve all of the features in the geometry.
If you have surfaces which are in close proximity, you could try using Proximity (p. 84) to automatically refine
the mesh to ensure that the gap is resolved properly.

Zero Length Vector
This error message can occur when Inflation (p. 75) is applied at a point where the normals of the adjacent
faces are in opposite directions. An example of such a geometry is shown below.




In this case the average of the normal created at the point A is zero. This type of geometry is uncommon
and should be avoided when using Inflation.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
114                                               of ANSYS, Inc. and its subsidiaries and affiliates.
Guidelines
 Mesh Length Scale

Mesh Length Scale
Length scale is a term used to describe the size of a mesh element. CFX-Mesh automatically selects a global
length scale for the model, typically 5% of the maximum model dimension. This length scale is often referred
to as the background length scale or Maximum Spacing for the simulation domain as a whole.

The Maximum Spacing will be the actual length scale of the mesh all over the region to be meshed, unless
it is overridden as a result of some sort of mesh control, which is used to modify locally the size of mesh
elements. This is particularly beneficial in an area of highly irregular flow or in a local area of interest.

Finally, length scales can be described in two forms. A face length scale is used to describe the size of the
triangles of a two-dimensional surface mesh. A volume length scale is used to describe the size of volume
elements of a three-dimensional volume mesh.

The following points should be considered and noted as good meshing practice:

 •   The length scale you use should reflect the features of the flow you wish to model. It is important to
     resolve geometric features that affect the flow with adequate mesh resolution.
 •   If the size of the geometric features vary significantly, then you will require local control over the mesh.
     It is recommended that you use at least 10 elements across any features of interest.
 •   For the highest accuracy, you should generally seek a mesh-independent solution, which means that
     the results of your simulation do not change by reducing the mesh length scale. You can approach this
     by gradually decreasing the Maximum Spacing of your mesh (and that of any Controls, Face Spacings
     or Edge Spacings applied to it) and comparing solutions. A straightforward way to do this is to use the
     Global Mesh Scaling (p. 86). Mesh independence means that errors due to the scale of the mesh affecting
     the computed results have been eliminated. In the majority of industrial simulations, mesh independent
     solutions cannot be achieved due to limits of available memory and computing power. For these simu-
     lations, it is still sensible to perform simulations for two or more mesh sizes in order to be able to make
     some estimate of the accuracy of the solution.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               115
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
116                               of ANSYS, Inc. and its subsidiaries and affiliates.
Part I, CFX-Mesh Tutorials
Introduction to the CFX-Mesh Tutorials
The following topics are covered in this section:

 •    Setting CFX-Mesh as the Default Method for Meshing (p. 119)
 •    Getting CAD Files for CFX-Mesh Tutorials (p. 120)
 •    Can I Skip the Geometry Creation? (p. 120)
 •    What if I Don't Have a License to Run DesignModeler? (p. 120)
 •    Importing CAD files for CFX-Mesh Tutorials (p. 120)
 •    Tutorials Requiring Modifications When Importing CAD Files (p. 121)

The CFX-Mesh Tutorials demonstrate how to set up the geometry and mesh for a variety of different problems.
The tutorials cover the most commonly used geometry features from DesignModeler and most of the
meshing functionality available in CFX-Mesh. Each tutorial results in the generation of a mesh that can be
imported directly into CFX-Pre. A brief description on how to use the generated mesh for flow analysis is
provided in the section Generating the Volume Mesh (p. 142) at the end of Tutorial 1.

      Note

      Use the mesh files supplied with ANSYS CFX while running session files in CFX-Pre. Meshes created
      in CFX-Mesh may produce errors when run with session files for ANSYS CFX tutorials. This is because
      the CFX-Pre session files are set up to use the mesh files provided with ANSYS CFX, and some
      face and body identifications are different from the ones which you would get when creating
      meshes by following the instructions provided in the CFX-Mesh tutorials.

      As an alternative, you may still use the mesh files created in CFX-Mesh, but should expect errors
      that will need to be corrected after the session file has finished playing.

These tutorial instructions are based on ANSYS Workbench 12.0. Some of these tutorials will not work in
earlier versions of ANSYS Workbench as they rely on new features.

Setting CFX-Mesh as the Default Method for Meshing
You can configure the following options to ensure that CFX-Mesh loads automatically whenever you create
a new mesh for your project.

 1.    From the Meshing application’s main menu, select Tools > Options to open the Options dialog box.
 2.    In the Options dialog box, select Meshing > Meshing and set Meshing > Default Method to CFX-
       Mesh.
 3.    Click OK.

By setting the default mesh method as CFX-Mesh, a new model opens automatically in the CFX-Mesh interface
for the first time only. Once CFX-Mesh has been closed and if you want to re-edit your mesh in CFX-Mesh,
see other ways for launching CFX-Mesh in Tutorial 1.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               119
Introduction to the CFX-Mesh Tutorials

Getting CAD Files for CFX-Mesh Tutorials
Some tutorials require DesignModeler or Parasolid files as a starting point for the geometry creation. Where
such a file is required, the introduction at the beginning of tutorial explains this. The following files are
available for download:

DesignModeler files (.agdb)

 •    All tutorials: http://www.ansys.com/dm_how_tos/cm_geometry.exe
 •    Tutorial 14 only: http://www.ansys.com/dm_how_tos/cm_cadmeshing.exe

Parasolid files (.x_t)

 •    All tutorials: http://www.ansys.com/dm_how_tos/cm_geom_Parasolid.exe
 •    Tutorial 6 only: http://www.ansys.com/dm_how_tos/cm_pipevalve.exe
 •    Tutorial 13 only: http://www.ansys.com/dm_how_tos/cm_combustor.exe

You need to create a Samples directory and then extract CAD files by executing the downloaded .exe
files.

Can I Skip the Geometry Creation?
The tutorial instructions consist of two phases: Geometry Creation and Mesh Generation. If you are only inter-
ested in the mesh generation part of tutorials and want to skip the geometry creation, you should download
the DesignModeler geometry files for the tutorial of interest and follow the steps outlined in Importing CAD
files for CFX-Mesh Tutorials (p. 120).

What if I Don't Have a License to Run DesignModeler?
If you do not have a license to run DesignModeler, use the supplied Parasolid files (.x_t) for CFX-Mesh
Tutorials. For details, see Importing CAD files for CFX-Mesh Tutorials (p. 120).

Importing CAD files for CFX-Mesh Tutorials
The instructions for importing the relevant CAD files (Parasolid or otherwise) for CFX-Mesh Tutorials are as
follows:

 1.    Start ANSYS Workbench and add a standalone Mesh system on the Project Schematic. Save the project
       with the name suggested by the tutorial. For details, see Creating the Project in ANSYS Workbench (p. 126)
       in Tutorial 1.
 2.    On the Project Schematic, right-click Geometry cell in the Mesh system and select Import > Browse.
       In the Open dialog box, select the appropriate CAD file from your Samples directory. See Getting
       CAD Files for CFX-Mesh Tutorials (p. 120) for instructions to download the geometry file for the tutorial
       of interest.

       The geometry is now included in the project and the Geometry cell appears in an up-to-date state.
 3.    Continue with the tutorial from the beginning of the Mesh Generation section.




                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
120                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                    Tutorials Requiring Modifications When Importing CAD Files


     Note

     Instead of using the ANSYS Workbench-based geometry handling application, if you import the
     Parasolid files into your CAD package and then import the resulting CAD file into the Mesh system
     in ANSYS Workbench, you may occasionally find that while the geometry still looks the same af-
     terwards, certain features may change subtly due to differences in the geometry representation
     in your CAD package.


Tutorials Requiring Modifications When Importing CAD Files
This section contains information on CFX-Mesh tutorials that need minor modifications as a result of importing
Parasolid files (or other CAD files) directly:

 •   "Tutorial 2: Static Mixer (Refined Mesh)" (p. 145) - This tutorial uses the geometry developed in Tutorial 1.
     The section Further Geometry Modification (p. 147) in this tutorial requires you to use the DesignModeler
     geometry, either by creating a new geometry in DesignModeler or by using the supplied DesignModeler
     file, StaticMixer.addb. If you want to see how to update your geometry, it is recommended that
     you read through Updating the Geometry in CFX-Mesh (p. 150), as this is not covered by any other tutorial.
 •   "Tutorial 6: Butterfly Valve" (p. 173) - The units after you import the Parasolid file are always meters, but
     the tutorial instructions expect the geometry to be in millimeters. You will need to enter all given values
     in the correct units of meters, e.g., when the tutorial asks you to set a Default Body Spacing of 4.5 mm,
     you must enter 0.0045 m.
 •   "Tutorial 7: Catalytic Converter" (p. 181) - The units after you import the Parasolid file are always meters,
     but the tutorial instructions expect the geometry to be in centimeters. You will need to enter all given
     values in the correct units of meters, e.g., when the tutorial asks you to set a Default Body Spacing of
     1.0 cm, you must enter 0.01 m.
 •   "Tutorial 8: Annulus" (p. 189) - The units after you import the Parasolid file are always meters, but the
     tutorial instructions expect the geometry to be in feet. You will need to enter all given values in the
     correct units of meters, e.g., when the tutorial asks you to set a Default Body Spacing of 0.02 ft, you
     must enter 0.006 m. Conversions for the other values are given in the tutorial instructions.
 •   "Tutorial 9: Mixing Tube" (p. 195) - The units after you import the Parasolid file are always meters, but the
     tutorial instructions expect the geometry to be in millimeters. You will need to enter all given values
     in the correct units of meters, e.g., when the tutorial asks you to set a Default Body Spacing of 0.6 mm,
     you must enter 0.0006 m.
 •   "Tutorial 10: Heating Coil" (p. 201)
     –   The DesignModeler geometry puts both solid bodies into one part and creates shared faces between
         them, so that CFX-Mesh can create one mesh containing both bodies. However, the result of the
         direct Parasolid import will be to have two bodies each in a separate part, so CFX-Mesh will create
         one mesh file containing two separate meshes, and hence two separate assemblies in CFX-Pre. The
         resulting mesh can be used in CFX-Pre as usual; an example of how to deal with multiple assemblies
         in CFX-Pre is detailed in the Catalytic Converter under ANSYS CFX tutorials.

         You are strongly advised that if you want to work through the ANSYS CFX example after creating
         your mesh, you should use the CFX Mesh file HeatingCoilMesh.gtm supplied with your ANSYS
         CFX installation, because the tutorial instructions were written expecting one mesh containing both
         bodies.
     –   The tutorial instructions ask you to suppress one of the Bodies contained in Part 3. Instead, you
         should click on the name of each part in turn, and see which one corresponds to the coil and which
         one to the container. Then right-click over the part which corresponds to the coil, and select Suppress.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               121
Introduction to the CFX-Mesh Tutorials

          Later, in order to see which 2D Regions you have selected, suppress the other part in the same way.
          Afterwards, unsuppress both parts by right-clicking on their names and selecting Unsuppress.
 •    "Tutorial 11: Airlift Reactor" (p. 211)
      –   The DesignModeler geometry puts both solid bodies into one part and creates shared faces between
          them, so that CFX-Mesh can create one mesh containing both bodies. However, the result of the
          direct Parasolid import will be to have two bodies each in a separate part, so CFX-Mesh will create
          one mesh file containing two separate meshes, and hence two separate assemblies in CFX-Pre. The
          resulting mesh can be used in CFX-Pre as usual; an example of how to deal with multiple assemblies
          in CFX-Pre is detailed in the Catalytic Converter under ANSYS CFX tutorials.

          You are strongly advised that if you want to work through the ANSYS CFX example after creating
          your mesh, you should use the CFX Mesh file BubbleColumnMesh.gtm provided by your ANSYS
          CFX installation, because the tutorial instructions were written expecting one mesh containing both
          bodies.
      –   When you create the Composite 2D Region DraftTube, you may find that the selection rectangles
          appear in the order (from left to right): outside of the column, draft tube face (inside), draft tube
          face (outside), and face from symmetry plane, instead of the order listed in the tutorial instructions.
          You can tell which order they appear in, since the selection rectangle corresponding to the draft
          tube (outside) will be the same color as the outside of the column. This is the one which you require.
 •    "Tutorial 13: Can Combustor" (p. 225)
      –   The DesignModeler geometry puts all five solid bodies into one part and creates shared faces between
          them, so that CFX-Mesh can create one mesh containing all of the bodies. The result of the direct
          Parasolid import will be to have five bodies each in a separate part, so CFX-Mesh will create one
          mesh file containing five separate meshes, and hence five separate assemblies in CFX-Pre. The res-
          ulting mesh can be used in CFX-Pre as usual; an example of how to deal with multiple assemblies
          in CFX-Pre is detailed in the Catalytic Converter under ANSYS CFX tutorials.
      –   You are advised that if you want to work through the ANSYS CFX example after creating your mesh,
          you should use the CFX Mesh file CombustorMesh.gtm supplied with your ANSYS CFX installation,
          since the tutorial instructions were written expecting one mesh containing all of the bodies.

List of Features
The following table shows you which geometry features are covered in which tutorial.

                                        1      2       3       4      5       6       7      8       9      10 11 12 13 14
Sketching Mode
Draw Toolbox                             •      •       •      •       •      •       •       •      •       •       •      •
Modify Toolbox                                                 •       •              •                      •       •
Dimensions Toolbox                       •      •       •              •                                     •       •
Constraints Toolbox                                                    •                                             •
Settings Toolbox                         •      •       •                             •       •
3D Features
Extrude                                  •      •       •      •       •      •       •       •      •       •       •      •
Revolve                                  •      •                                     •              •               •
Sweep                                                   •                                                    •
Skin/Loft                                                                             •


                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
122                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                                  List of Features

                                           1      2       3       4      5       6       7      8       9      10 11 12 13 14
Other Features
Parasolid Import                                                                 •                                                        •
Multiple Bodies                                                                                                 •       •                 •
Freeze/Unfreeze/Add                                                       •      •                              •       •
Frozena
Body Operationsb                                                          •      •                              •
                                    c
Plane Creation from Faces                          •                                     •                      •       •
                    d
Imprint Faces                                                                                           •               •      •
Enclosure                                                                                                               •
a
  Freeze/Unfreeze/Add Frozen: for multiple bodies and for creating bodies that enclose another body
b
  Body Operations: for copying, moving, and subtracting bodies from other bodies
c
  Plane Creation from Faces: for 3D Feature operations on existing surfaces
d
  Imprint Faces: for Boundary Condition Surfaces

The following table shows you which meshing features are covered in which tutorial.

                                            1      2       3       4      5       6       7      8       9      10 11 12 13 14
2D Region Groups                            •       •       •      •       •      •       •       •      •       •       •      •         •   •
                    a
Face Spacing                                                •              •      •                              •              •
Curvature-Sensitive Meshing                                                       •                      •
            b
Controls                                                           •
Periodicity                                                                                       •
            c
Inflation                                           •       •      •       •      •       •       •      •       •              •         •   •
Stretch                                                                                                  •
                d
Proximity                                                                  •      •                              •
                        e
Preview Groups                              •       •       •      •       •      •               •      •       •                            •
Extruded 2D Meshing                                                                               •
Parallel Volume Meshing
Geometry Update                                     •
CAD Check                                                                                                                                     •
Virtual Faces and Edges                                                                                                                       •
Short Edge Removal                                                                                                                            •
a
  Face Spacing: for refining the mesh on a particular face or faces
b
  Controls: for refining the mesh near a point, line or triangle
c
  Inflation: for producing prism elements along a boundary in order to resolve the boundary better
d
  Proximity: for refining the mesh when two faces or two edges are close but not joined
e
  Preview Groups: for previewing part or all of the surface mesh




                            Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                        of ANSYS, Inc. and its subsidiaries and affiliates.                                                   123
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
124                               of ANSYS, Inc. and its subsidiaries and affiliates.
Tutorial 1: Static Mixer




This tutorial shows how to create the geometry and mesh for a simple static mixer. This tutorial assumes
that you have never used ANSYS Workbench before and gives detailed instructions on every step needed
to construct this model. The following geometry and meshing features are illustrated:

 •    Basic geometry creation, including Revolve and Extrude operations
 •    Basic meshing operations.

This tutorial discusses two ways to add a geometry to the project: importing an existing geometry and cre-
ating a new geometry. If you want to skip the geometry creation part of the tutorial, it may still be worth
reading through how to do so if you have not used ANSYS Workbench before as the tutorial contains
background information that is applicable to both CFX-Mesh and DesignModeler.

The Meshing Process Using CFX-Mesh
In order to create a mesh using CFX-Mesh, the steps are as follows:

 1.    Create the Project in ANSYS Workbench.
 2.    Create or import the Geometry.
 3.    Define the Regions.
 4.    Define the Mesh Attributes.
 5.    Generate the Surface Mesh (this is optional).
 6.    Generate the Volume Mesh.

Your first step after starting ANSYS Workbench is to create a new project on the Project Schematic. ANSYS
Workbench's file management system helps you to manage files created for your project. You can create
the geometry either in ANSYS Workbench or by importing it from a CAD package. The geometry creation
tool in ANSYS Workbench is DesignModeler, a parametric feature-based solid modeler. Most of the CFX-Mesh
tutorials include instructions on creating geometry in DesignModeler, although for full documentation you
should consult the DesignModeler Help.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               125
Tutorial 1: Static Mixer

After adding the geometry to the project, the remaining steps are carried out within CFX-Mesh, which can
be launched from within the Meshing application. The generation of the surface mesh is optional; if it is not
generated explicitly, then it will be generated as part of the creation of the volume mesh.

After generating the mesh, you can also perform the flow analysis using the ANSYS CFX software. See note
in Introduction to the CFX-Mesh Tutorials on using the mesh while running session files in CFX-Pre.

Geometry Creation
Creating the Project in ANSYS Workbench
The first step for any new case is to create the project in ANSYS Workbench.

 1.   Open ANSYS Workbench. Use the Windows Start menu and select ANSYS 12.0 > Workbench from
      the list of installed programs.

      The Project Schematic appears with an Unsaved Project. By default, ANSYS Workbench is configured
      to show the Getting Started dialog box that describes basic operations in ANSYS Workbench. Click
      the [X] icon to close this dialog box. To turn on or off this dialog box, select Tools > Options from the
      main menu and set Project Management > Startup > Show Getting Started Dialog as desired.
 2.   Now, add a Mesh system on the Project Schematic. From the Component Systems toolbox, double-
      click on the Mesh template, or drag it onto the Project Schematic.

      A standalone Mesh system appears on the Project Schematic.
 3.   The next step is to specify the location for your project files in ANSYS Workbench. Select File > Save
      from the main menu of ANSYS Workbench, and save the project as StaticMixer.wbpj in a directory
      of your choice.

      This specified location will be the default directory for all of the project files that are created during
      this tutorial. The project files and their associated folder locations appear under the Files view on the
      Project Schematic. To make the Files view visible, select View > Files from the main menu of ANSYS
      Workbench.

Now the project is ready for further processing. The following figure shows a standalone Mesh system on
the Project Schematic. Note the name of the project, StaticMixer, appears in the title bar of the ANSYS
Workbench application.




                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
126                                                    of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                              Creating a New Geometry in DesignModeler

Figure: The ANSYS Workbench Application




The Mesh system is composed of various cells. ANSYS Workbench provides visual indications of a cell's state
at any given time via icons on the right side of each cell. In Figure : The ANSYS Workbench Application (p. 127),
Geometry and Mesh cells are shown with a blue question mark (?), indicating that cells need to be set up
before continuing the analysis. See Understanding Cell States for a description of various cell states.

Adding Geometry to the Project
A geometry can be added to the project in the following ways:

 •    Importing an Existing Geometry (p. 127)
 •    Creating a New Geometry in DesignModeler (p. 127)

If you want to create a new geometry manually, proceed to the section Creating a New Geometry in Design-
Modeler (p. 127).

Importing an Existing Geometry
This section describes how to import an existing geometry file StaticMixer.agdb into the project.

      Note

      If you do not have this file, then see Getting CAD Files for CFX-Mesh Tutorials (p. 120) for details.

 1.    On Project Schematic, right-click Geometry cell in the Mesh system and select Import Geometry >
       Browse. In the Open dialog box, select StaticMixer.agdb from your Samples directory.

       The geometry is included in the project and the Geometry cell appears in an up-to-date state.
 2.    Now proceed to the section Mesh Generation.

Creating a New Geometry in DesignModeler
This section describes how to create a new geometry using DesignModeler.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               127
Tutorial 1: Static Mixer

 1.    On the Project Schematic, right-click Geometry cell in the Mesh system and select New Geometry to
       create geometry within DesignModeler.

       DesignModeler loads along with a pop-up window, prompting you to set a desired length unit.
 2.    Select Meter.

            Note

            If you have previously set the default unit by selecting either Always use project unit or
            Always use selected unit in DesignModeler, the units pop-up window will not appear.

            To access the units pop-up window upon subsequent openings of DesignModeler, open
            the Options dialog box by selecting Tools > Options from DesignModeler's main menu.
            In the Options dialog box, select DesignModeler > Units and set Units > Display Units
            Pop-up Window to Yes. For details, see Units in the DesignModeler Help.


            Note

            If you are using the Parasolid file supplied for this tutorial, see Tutorials Requiring Modifications
            When Importing CAD Files (p. 121).


The following section provides an overview of geometry creation features available in DesignModeler that
will help you become familiar with its operation.

Overview of DesignModeler
The DesignModeler application is arranged into the following main areas, also marked in the figure below:

 •    The top area contains various menus and toolbars
 •    The top-left area contains the Tree Outline and Sketching Toolboxes

      The following figure shows DesignModeler in a Modeling Mode with the Tree Outline. Click on the
      Sketching tab to access Sketching Toolboxes.
 •    The bottom-left area contains the Details View
 •    The right hand side contains the Graphics Window




                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
128                                                    of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                      Tree Outline and Sketching Toolboxes

Figure: The DesignModeler Application




Tree Outline and Sketching Toolboxes
DesignModeler has two main modes of operation: Modeling and Sketching. You will have to switch between
them as you build your model. Initially, DesignModeler loads using Modeling Mode, displaying the tree
structure under Tree Outline, as shown in Figure : The DesignModeler Application (p. 129). The area covered
by Tree Outline is replaced by Sketching Toolboxes when you switch from Modeling to Sketching. To
switch between the two modes, simply click on the Modeling or Sketching tab as appropriate.

The Sketching Mode supports five Sketching toolboxes to create 2D sketches: Draw, Modify, Dimensions,
Constraints and Settings. The Modeling mode enables you to create 3D models, for example, by extruding
or revolving profiles from your 2D sketches.

The Tree Outline shows all of the features of the geometry and their current state in a tree structure. When
DesignModeler is first opened, only the three default planes (XYPlane, ZXPlane, and YZPlane) are present,
together with an entry that shows you that there are currently 0 Parts, 0 Bodies. As you perform geometry
creation operations, the structure of the tree will expand to show these. The geometry operations such as
Extrude and Revolve are applied from the top of the tree downwards. For example, in Figure : The Tree
Outline (p. 129), Extrude2 is the first operation, followed by Revolve2.

Figure: The Tree Outline




In the Tree Outline, the symbols to the left of each item show the state of that particular item. The following
table describes the meaning of these symbols:


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                  129
Tutorial 1: Static Mixer

Sym- Meaning
bol
         Everything is OK.
         The item is suppressed, i.e., not taking any effect (it can be unsuppressed later).
         Something is wrong with the item, e.g., you tried to generate it before you had fully specified it,
         or you modified one of the features above it that makes the specifications of the item invalid.
         (You can see the error messages by right-clicking on the object and selecting Show Errors and
         Warnings.)
         The item needs to be generated or re-generated (because changes to the settings have been
         made since it was last generated).
         The sketch will remain visible even when not selected.
         The Body has been hidden (made invisible).


Details View
The Details View shows the details for the selected object. It can be used to edit the details (including the
name of the object) by simply typing over the information to be updated. When DesignModeler is first
opened, no object is selected, so the Details View is blank as shown in Figure : The DesignModeler Applica-
tion (p. 129).

Graphics Window
The Graphics window displays the geometry. Some examples of commonly used geometry manipulations
using mouse buttons are listed below:

 •    To rotate the geometry, click and hold down the middle mouse button and move the mouse over the
      Graphics window.
 •    To bring up a context sensitive menu, click the right mouse button over the Graphics window. This
      menu includes various options for manipulating the model as well as other options which are particular
      to what geometry operation you are performing or what objects are selected.
 •    To put the model into a particular view, you can use the Triad that is displayed at the bottom right
      corner of the Graphics window: click on one of the axes or on the cyan-colored ball to rotate the
      model.
 •    To view the entire model, right-click over the Graphics window and select Zoom to Fit.
 •    To zoom in to a selected area: click and hold down the right mouse button, drag the mouse to enclose
      the required area in a box and release the button. The Graphics window will refresh and zoom in to
      your selected area.

As you progress through this tutorial, the section Model Manipulation in DesignModeler (p. 135) will introduce
more ways to manipulate the model.

Recovering from Mistakes
You are certain to make mistakes as you build up your geometry, so it is important to know how to recover
from these.




                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
130                                                    of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Creating the Solid

If you are in Sketching Mode, then the Undo button in the Undo/Redo toolbar towards the top of the window
can be used to undo sketching operations. The Back button, accessed by right-clicking over the Graphics
window can be used to undo the selection of (for example) the last point in a polyline, whilst sketching.

If you are in Modeling Mode, and you have not yet generated your feature (such as Extrude) you can either
just make further changes in the Details View, or you can delete it by right-clicking on its name in the tree
view and selecting Delete.

After generating a feature, you can delete it by selecting it in the tree view and using Delete on the right
mouse menu. For example, if you have generated a feature such as Extrude and then realize that you selected
the wrong sketch to define it, you will need to use the Edit Selections feature. This is accessed by selecting
right-clicking over the name of the feature in the tree view and selecting Edit Selections. You will then be
able to edit the selections by using the Details View as usual.

Creating the Solid
You need to start creating the Static Mixer geometry by creating a sketch to make the main body of the
mixer.
 1.   Click ZXPlane in the Tree Outline found in the top left of the screen.
 2.   Click on the Sketching tab found below the tree view to work on the sketch.

Each sketch is created in a plane. By selecting the ZXPlane immediately before going into sketching mode,
you ensure that the sketch you are about to create is based on the ZXPlane.

Before starting to create your sketch, it helps to set up a grid of lines on the plane in which the sketch will
be drawn. The presence of the grid allows the precise positioning of points when the Snap option is enabled.

 1.   In the Sketching tab, click Settings to open the Settings toolbox.
 2.   Click Grid and select Show in 2D and Snap.
 3.   Click Major Grid Spacing and set it to 1.
 4.   Click Minor-Steps per Major and set it to 2.
 5.   You now need to zoom in to see the effect of changing Minor-Steps per Major. Click the right mouse
      button to the top left of the plane center in the Graphics window and drag a box across it to zoom
      into the middle of the grid. When you release the mouse button the model will be magnified to show
      the selected area.




You now have a grid of squares with the smallest squares being 50 cm across. Because Snap is enabled,
you will only be able to select points that are on this grid to build your geometry, and this can often help
to position objects correctly.

 1.   Select the Draw toolbox from the Sketching tab.
 2.   Click Polyline and then create the shape shown below as follows:


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                             131
Tutorial 1: Static Mixer

      a.   Click on the grid in any of the positions where one of the points from the shape needs to be
           placed.
      b.   Then click on each successive point to make the shape.
      c.   If you click on the wrong point, just click with the right mouse button over the Graphics window
           and select Back from the menu to undo the point selection.
      d.   To close the polyline after selecting the last point, click with the right mouse button to bring up
           a menu and select Closed End.

      The information of the new sketch, Sketch1, appears in the Details View. Note that the longest straight
      line (4 m long) in the diagram below is along the Z-axis (located at x = 0 m).




You will now create the main body of the mixer by revolving the new sketch around the Z-axis.

 1.   Select Revolve            from the 3D Features toolbar, located above the Graphics window.
 2.   Details of the Revolve operation are shown in the Details View at the bottom left of the window. Leave
      the name of the Revolve as the default, Revolve1.
 3.   The Base Object is the name of the sketch to be revolved. It defaults to the sketch which you have
      just created, Sketch1, so this setting does not need to be changed.
 4.   The Axis for the rotation does not have a default setting. In the Graphics window, click on the grid
      line which runs along the Z-axis and then click Apply in the Details View. You should find that the
      text next to Axis now changes to Selected. If instead it changes to Not Selected with a yellow back-
      ground, click on the text Not Selected and then try selecting the axis again in the Graphics window,
      remembering to press Apply in the Details View after you have selected it.
 5.   Leave Operation set to Add Material since you need to create a solid. The other options allow you
      to modify existing solids and manipulate multiple solid situations.
 6.   The sketch needs to be revolved by a full 360 degrees. Ensure that Angle is set to 360 degrees. Leave
      the other settings as default.
 7.   To activate the revolve operation, you need to click Generate . This can be selected from the menu
      which appears when you click with the right mouse button almost anywhere in the window, or from
      the 3D Features toolbar towards the top of the window.

After generation, you should find you have a solid as shown below.




                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
132                                                    of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Creating the Solid




Now, you need to create the two side pipes. This involves creating and extruding two new sketches. To
make it easier to see the grid when creating the sketches, the first step is to make the solid invisible for
now.

 1.   In the tree view, click the plus sign next to 1 Part, 1 Body to expand the tree structure.
 2.   Right-click Solid and select Hide Body.
 3.   Select the ZXPlane in the tree view again, and create a new sketch based on this plane by using the
      New Sketch        button on the Active Plane/Sketch toolbar, which is located above the Graphics window.
 4.   Select the Sketching tab.
 5.   Create a circle as shown in the figure below:
      a.   Select the Draw toolbox.
      b.   Select Circle, click on the grid to mark the center of the circle and then drag the mouse to define
           the radius.




Now, you need to extrude this sketch to make the first side-pipe.

 1.   Select Extrude        from the 3D Features toolbar, located above the Graphics window.
 2.   In the Details View at the bottom left of the window, change Direction to Reversed, in order to extrude
      in the opposite direction to the plane normal.
 3.   Change the Depth to 3 m and press Enter to set this value. The rest of the settings can be left as their
      default. The Add Material setting will mean that material is added to the existing solid, rather than a
      new solid being created.
 4.   To activate the extrude operation, you need to click Generate                                        as before.

In order to see the result of this, you will have to make the solid visible again:

 1.   In the tree view, right-click Solid and select Show Body.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                             133
Tutorial 1: Static Mixer

 2.   Click and hold the middle mouse button over the middle part of the Graphics window and drag the
      mouse around to rotate the model. Check that the Solid looks like the figure below when rotated into
      a viewing position so that the side-pipe is clearly visible.




 3.   Right-click Solid and select Hide Body.

To create the other side pipe, the same operations are used.

 1.   Select the ZXPlane in the tree view again, and create a new sketch based on this plane by using the
      New Sketch            button on the Active Plane/Sketch toolbar, which is located above the Graphics window.
 2.   Select the Sketching tab.
 3.   Right-click over the Graphics window and select Isometric View to put the sketch back into a sensible
      viewing position. Then right-click again and select Zoom to Fit to zoom in on the sketch, if it appears
      too small.
 4.   From the Draw toolbox, select Circle and then create the second circle shown in the figure below:




 1.   Select Extrude            from the 3D Features toolbar.
 2.   In the Details View, set Direction to Normal, in order to extrude in the same direction as the plane
      normal.
 3.   Ensure that Depth is set to 3 m. Leave the other settings as default.
 4.   To activate the extrude operation, you need to click Generate                                            as before.
 5.   In the tree view, right-click Solid and then select Show Body.

The geometry is now complete.

 1.   From the DesignModeler's main menu , select File > Save Project to save the project.




                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
134                                                    of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                     Model Manipulation in DesignModeler

Model Manipulation in DesignModeler
Before moving on, practice using the mouse to manipulate the model in the Graphics window. This is essential
to be able to move the model into positions which are good for selecting or looking closely at particular
parts of the model.

 1.   Ensure that Rotate mode               is selected from the Rotation Modes toolbar at the top of the window.
 2.   Click and hold the middle mouse button over the middle part of the Graphics window and drag the
      mouse around to rotate the model. This is the most common way to move the model.
 3.   Now, move the mouse towards the top left of the Graphics window. As you get near to the top left,

      the cursor should change from        to       . If you now click and hold the middle mouse button with
      the new cursor showing, and drag the mouse around, you will be able to rotate the model about an
      axis which points out of the screen (“roll”).
 4.   There are two more types of rotations, also shown in the figure below. Drag the mouse towards the

      left edge of the Graphics window until the cursor changes to       . If you click and hold the middle
      mouse button with this cursor showing, then the rotation is constrained to be around a vertical axis
      in the plane of the screen. Similarly, if you drag the mouse towards the top edge of the Graphics

      window, the cursor changes to       . If you click and hold the middle mouse button with this cursor
      showing, then the rotation is constrained to be around a horizontal axis in the plane of the screen.

      The type of rotation modes available depends on the position of the cursor. The following figure illus-
      trates areas of the Graphics window which correspond to each type of rotation. Note that the circular
      region where you get free rotation will always fill the smallest dimension of the window.




 5.   Put the model back into the Isometric View by clicking on the cyan-colored ball in the Triad at the
      bottom right of the Graphics window.

The steps to zoom in on one of the pipe ends are outlined below:

 1.   Right-click on the Graphics window to the top left of the pipe end which is visible and drag a box
      across it. When you release the mouse button, the model will expand so that the contents of the box
      are visible across the whole Graphics window.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                135
Tutorial 1: Static Mixer




 2.   Try rotating the model. You will find that the model by default rotates around the model center, so
      the pipe end quickly moves out of view. You can change this as outlined below:
      •   Bring the pipe end back into view, and click once with the left mouse button on the pipe end.
          DesignModeler will place a small red sphere where you clicked, and then the model is repositioned
          so that the small red sphere moves to the middle of the Graphics window. If you now try rotation,
          you will find that the model rotates around the small red sphere, not the model center, so the pipe
          end is always in view.
      •   To change back to rotating around the model center, click once with the left mouse button anywhere
          in the Graphics window that is away from the model itself.
 3.   Zoom out again by holding down the Shift key on the keyboard, pressing the middle mouse button
      and dragging the mouse downwards. You can zoom in by dragging the mouse upwards instead. An
      alternative way of enabling the Zoom functionality is to select Zoom     from the Rotation Modes
      toolbar. Once this is enabled, zooming in and out is done by clicking and dragging with the left mouse
      button. If Zoom mode is selected, then most of the ways that you just tried rotating the model are
      no longer available; you must select Rotate mode                                     again to use them.

There are two more useful ways to manipulate the model in the Graphics window.

 1.   Pan (or Translate) the model by holding down the Ctrl key on the keyboard, pressing the middle mouse
      button and dragging the mouse around. An alternative way of enabling the Pan functionality is to
      select Pan mode              from the Rotation Modes toolbar. Once this is enabled, panning is done by
      clicking and dragging with the left mouse button. Again, you must reselect Rotate mode                                             to use
      most of the different rotation methods.
 2.   Finally, center the model in the Graphics window and resize it so that it is all visible by selecting Zoom
      to Fit     from the Rotation Modes toolbar.

In the rest of this tutorial and all of the subsequent tutorials, you should use the functionality described
above to manipulate the model in any way which is convenient.

Once you are familiar with DesignModeler, close DesignModeler by selecting File > Close DesignModeler
from the main menu and return to the Project Schematic. Now the Geometry cell appears in an up-to-date
state.

Mesh Generation
Launching CFX-Mesh
The next step after you have created the geometry is to generate a mesh using CFX-Mesh.

 1.   On the Project Schematic, right-click Mesh cell in the Mesh system and select Edit to launch the
      Meshing application.


                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
136                                                    of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                   Launching CFX-Mesh

     If you have configured your global settings to ensure that CFX-Mesh is loaded automatically, the
     Meshing application will load followed by CFX-Mesh. Otherwise, if only the Meshing application appears,
     continue with the following step.
2.   Launch CFX-Mesh from the Meshing application by following one of the methods outlined below:

     Figure: The Meshing Application




     •   Launching from the Meshing Options panel

         This method is applicable only for generating a new mesh. Once CFX-Mesh has been closed and
         if you want to re-edit your mesh in CFX-Mesh in a subsequent attempt, see other two ways described
         below this method.
         a.   In the Meshing application, if the Meshing Options panel to the right of the viewer is not
              visible, expand Model in the Outline tree view and select Mesh. Then click on the Options
              button from the toolbar. The Meshing Options panel appears.
         b.   On the Meshing Options panel, set Mesh Method to CFX-Mesh.
         c.   (Optional) To set your global settings such that CFX-Mesh is loaded automatically whenever
              you choose to create a new mesh, ensure that Set Meshing Defaults is selected.
         d.   Click OK. CFX-Mesh now loads.
     •   Launching from the Outline tree view
         a.   In the tree view, expand Model and right-click on Mesh.
         b.   Select Edit in CFX-Mesh.

              This results in CFX-Mesh method to be assigned to the whole geometry and CFX-Mesh loads.
     •   Launching by Creating a Meshing Method
         a.   In the Outline tree view, expand Model and right-click on Mesh.
         b.   Select Insert > Method.



                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                             137
Tutorial 1: Static Mixer

          c.   Clicking anywhere on the geometry in the Graphics window and then click Apply in the Details
               View next to Geometry.
          d.   In the Details View, set Definition > Method to CFX-Mesh.
          e.   In the Outline tree view, right-click CFX-Mesh Method and select Edit in CFX-Mesh to load
               CFX-Mesh.

      Anytime you choose to edit a mesh by launching CFX-Mesh from within the Meshing application, the
      Mesh cell on the Project Schematic will become out-of-date and will require updating from within the
      Project Schematic. For details on how to update the Mesh cell, see Updating the Mesh Cell State.

Overview of the CFX-Mesh Interface
The CFX-Mesh interface is designed to have the same look and feel as DesignModeler. In particular, this
means that you can use the same mouse controls to manipulate the model.

Figure: The CFX-Mesh Interface




One important difference between DesignModeler and CFX-Mesh is in the order of the items in the tree
structure. In DesignModeler, the Tree Outline shows items in the order that they were created, and the order
affects the final geometry. In the Tree View of CFX-Mesh, the order of the items does not have an influence
on the final mesh. The items of the same type are grouped together, independent of when they were created.

You will notice that various items are already present in CFX-Mesh under the Tree View; these are the default
items and contain default settings. Some of the symbols next to items in the tree structure have slightly
different implications in CFX-Mesh than they did in DesignModeler. In CFX-Mesh, the meanings are as follows:

Basic       Description                                                             Hidden Sym-                  Suppressed              Preview
Sym-                                                                                bols a                       Symbols b               Group Sym-
bols                                                                                                                                     bols c
            An item without any symbol is valid.                                                                 The item and
                                                                                                                 its status sym-
                                                                                    This symbol in-              bol become              This symbol
                                                                                    dicates that                 gray on sup-            indicates that
                                                                                    the Region is                pressing.               the Preview
                                                                                    valid and hid-                                       Group is valid
                                                                                    den.                                                 and hidden.

                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
138                                                    of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                               Overview of the CFX-Mesh Interface

Basic        Description                                                            Hidden Sym-                  Suppressed              Preview
Sym-                                                                                bols a                       Symbols b               Group Sym-
bols                                                                                                                                     bols c
             Check mark: Everything is valid but the
             item has been automatically updated by
             CFX-Mesh and it is recommended to verify
             the changes.

             Example: This may occur if you have per-
             formed a geometry update that has resul-
             ted in a face that no longer exists. If that
             face was being used in the location list for
             any mesh feature, then it will be removed
             automatically as part of the update and
             CFX-Mesh marks the affected mesh feature
             with this status symbol.
             Padlock: Everything is valid but the item is
                     ,
             “locked” i.e., editing of this feature is restric-
             ted in some way. In general, items which are                           Example: The
             locked cannot be deleted, and most cannot                              Default 2D Re-
             be renamed or have their locations changed.                            gion is given
                                                                                    this symbol
                                                                                    when it cannot
                                                                                    be deleted or
                                                                                    renamed.
             Exclamation: This means that there is
             something invalid about the definition of
             the item or one of its sub-items that will                                                          This symbol
             also be marked with the same symbol. Of-                                                            indicates that
             ten this will be because no required selec-                                                         the item is
             tion has been made.                                                                                 suppressed
                                                                                                                 and will be
                                                                                                                 invalid when
                                                                                                                 it is unsup-
                                                                                                                 pressed.
             The item is locked and invalid. You must make the item valid before you can mesh again. In
             the case of a locked Virtual Edge, all you can do is do is delete it; in most other cases you must
             edit the location list to make it valid.

             See the description of the locked symbol                              above.
             This symbol indicates that an item contains associated sub-items. Left-click on the symbol to
             expand the item and display its contents.
             This symbol indicates that an item contains associated sub-items. Left-click on the symbol to
             collapse the item so that none of its sub-items are visible in the tree.
a
  Hidden Symbols: They apply to Regions when an item has been hidden in the Graphics window. As such, the item cannot be selected in
the Graphics window; however, the item is not suppressed and will still be meshed (although the mesh can be displayed on the item only
when the item is visible in the viewer).The symbols are paler versions of the basic symbols and their meanings correspond.
b
  Suppressed Symbols:The item and its status symbol become gray on suppressing.The suppressed item becomes inactive and is not included
in the mesh.You must unsuppress an object before you can edit or delete it.
c
  Preview Group Symbols:They apply to Preview Groups when the mesh has not been generated or the generated mesh is out-of-date, i.e.,
it does not reflect the current mesh settings.To generate an up-to-date mesh for the Preview Group, right-click over its name and select

                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                       of ANSYS, Inc. and its subsidiaries and affiliates.                                            139
Tutorial 1: Static Mixer

Generate This Surface Mesh.To generate an up-to-date mesh on all Preview Groups, right-click Preview in the Tree View and select Gen-
erate All Surface Meshes.

The surface and volume mesh is controlled by various features that you can access in CFX-Mesh. The type
of controls available depends on the mesher used. By default, you are using the Delaunay Surface Mesher
for surface meshing and Advancing Front Volume Mesher for volume meshing.

In this first tutorial, you will only set up the most basic features for controlling the mesh generation. Only
the length scale of the mesh will be specified.

Setting up the Regions
The first step is to define some regions on the geometry. Composite 2D Regions are created from the solid
faces (primitive 2D Regions) of the geometry. Composite 2D Regions can be used in CFX-Pre to assign
boundary conditions, such as inlets and outlets, to the problem. It is not a requirement of that you create
such regions; however, grouping faces into Composite 2D Regions in CFX-Mesh will make selection of regions
easier in CFX-Pre. This tutorial uses an inlet boundary condition at the entrance to each of the two side
pipes, an outlet boundary condition on the end of the funnel outlet and a wall boundary condition for the
remaining surfaces.

      Note

      There is an important distinction between primitive 2D Regions and the underlying solid faces
      that applies when the model has more than one solid. This is explained in "Tutorial 10: Heating
      Coil" (p. 201) under Mesh Generation (p. 206).

If you look at the Tree View, you can see that under Regions, one Composite 2D Region is defined already,
called Default 2D Region. This region will always contain all of the faces of the model that you have not
explicitly assigned to another Composite 2D Region.

Create the Composite 2D Region for the first inlet:

 1.    Right-click Regions in the Tree View.
 2.    Select Insert > Composite 2D Region.
 3.    A new object, Composite 2D Region 1, is inserted under Regions in the Tree View. In the Details
       View, there will be two buttons, Apply and Cancel, next to Location. This means that you are ready
       to select the face from the Graphics window.

             Tip

             You can rotate the model during face selection by holding down the middle mouse button
             and moving the mouse over the geometry.


 4.    In the Graphics window, click on the circular face at the end of the side pipe that is at the position
       with the lowest value of the Y-coordinate. This will turn green to show that it has been selected, as in
       the figure below.




                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
140                                                    of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Setting up the Mesh




 5.   Click Apply in the Details View. The face will turn red indicating that the region has been successfully
      created.
 6.   Change the name of the region to in1: right-click over the name, select Rename and then type over
      the existing name.

Create the second inlet:

 1.   Right-click Regions in the Tree View.
 2.   Select Insert > Composite 2D Region.
 3.   A new object, Composite 2D Region 1, is inserted under Regions in the Tree View. In the Graphics
      window, click on the circular face at the end of the side pipe with the highest value of the Y-coordinate.
 4.   Click Apply in the Details View.
 5.   Change the name of the region to in2 by right-clicking over the existing name.

Create the region for the outlet:

 1.   Right-click Regions in the Tree View and select Insert > Composite 2D Region.
 2.   Select the circular face at the bottom of the mixer vessel, with the lowest value of the Z-coordinate.
 3.   Click Apply in the Details View.
 4.   Change the region name to out.

It is not necessary to create a fourth Composite 2D Region for the walls of the static mixer. Any remaining
faces that are not explicitly assigned to a Composite 2D Region are automatically assigned to the 2D Region
named Default 2D Region. You can use this region in CFX-Pre to define the location of your wall boundary
condition.

Setting up the Mesh
You will set a single size for all elements in this tutorial. The next tutorial will improve upon this coarse mesh.

 1.   Click Default Body Spacing in the Tree View, which is contained in Mesh > Spacing.
 2.   In the Details View, change Maximum Spacing to 0.3 m. This is a coarse length scale for this model,
      but is reasonable for a first run to generate an approximate solution and to test that the model is
      working correctly.
 3.   Press Enter on the keyboard to set this value.

The remaining settings will be left as their default.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                              141
Tutorial 1: Static Mixer

Generating the Surface Mesh
It is not necessary to create a surface mesh within CFX-Mesh, since if it has not been created explicitly it will
be generated automatically when you create the volume mesh. However, in many of these tutorials, you
will create the surface mesh first, in order to demonstrate the effect of various mesh settings. It is generally
a good idea to check the surface mesh before creating the volume mesh as it allows you to ensure that all
settings result in the desired effect.

You will now view the surface mesh to see the effect of the chosen length scale.

 1.   Click plus sign next to Preview in the Tree View to expand the tree.
 2.   Right-click Default Preview Group and select Generate Surface Meshes. The Default Preview Group
      always contains all faces in the geometry, so the mesh will be generated everywhere.

During the generation of the surface mesh, the progress will be displayed in the status bar at the bottom
of the CFX-Mesh window.

      Note

      You can modify the way that the mesh is displayed by clicking on Preview in the Tree View and
      changing the options shown in the Details View. For example, by changing the Display Mode
      you can switch to display the mesh in Wire Mesh rather than with solid faces. Simply click on
      the name Default Preview Group to redisplay the surface mesh using the new settings.




Generating the Volume Mesh
To generate the volume mesh, right-click Mesh in the Tree View and select Generate Volume Mesh.

During the generation of the volume mesh, the progress will be displayed in the status bar at the bottom
of the CFX-Mesh window. When the volume mesh is complete, the status bar displays the message that
operation has completed successfully and you will be able to take control of the user interface again.

This completes the mesh generation. Now save the project, close CFX-Mesh and the Meshing application,
and return to the Project Schematic as outlined in the following steps:

 1.   Save the project by selecting File > Save from CFX-Mesh's main menu.
 2.   Close the CFX-Mesh interface by selecting File > Close CFX-Mesh.

      This step closes CFX-Mesh and the Meshing application appears.
 3.   Now, close the Meshing application by selecting File > Close Meshing from the Meshing application's
      main menu.
 4.   Return to the Project Schematic. Now the Mesh cell appears in an up-to-date state.

                           Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
142                                                    of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                    Generating the Volume Mesh

The volume mesh generated above can be used for performing the flow analysis using the ANSYS CFX
software. This can be achieved by adding a CFX system as a downstream connection to the Mesh system
containing the generated mesh. On the Project Schematic, right-click Mesh cell in the existing Mesh system
and select Transfer Data To New > CFX from the menu.

A CFX system linked to the Mesh system will be added to the Project Schematic as shown below.




The Mesh cell indicates that an update is required. Right-click the Mesh cell and select Update.

In the CFX system, right-click Setup cell and select Edit from the menu to open the mesh in the ANSYS CFX
software. For details on performing an analysis with ANSYS CFX software, see Analysis Systems in the ANSYS
Workbench Help.

This finishes the Static Mixer tutorial. You can exit from ANSYS Workbench by selecting File > Exit from the
main menu.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                      143
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
144                               of ANSYS, Inc. and its subsidiaries and affiliates.
Tutorial 2: Static Mixer (Refined Mesh)




This tutorial modifies the mesh and geometry for the static mixer model created in "Tutorial 1: Static Mix-
er" (p. 125), and assumes that you have access to the project files created as part of that example. The following
geometry and meshing features are illustrated:

 •    Modifying an existing mesh setup
 •    Inflation
 •    Geometry update.

Modifying the Mesh Generation
Opening the Existing Project
This section outlines the steps to open the project that was created in "Tutorial 1: Static Mixer" (p. 125) and
saving it as StaticMixerRef.wbpj.

 1.    Open ANSYS Workbench.

       The Project Schematic appears with an Unsaved Project.
 2.    From ANSYS Workbench's main menu, select File > Open and open the project file StaticMix-
       er.wbpj that was created in Tutorial 1.
 3.    Now select File > Save As to open the Save As dialog box.
 4.    Select a new working directory for the refined static mixer project and save the project as Static-
       MixerRef.wbpj.

       Note the name of the project, StaticMixerRef, appears in the title bar of the ANSYS Workbench applic-
       ation.

Launching CFX-Mesh
 1.    On the Project Schematic, right-click Mesh cell in the Mesh system and select Edit to launch the
       Meshing application.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               145
Tutorial 2: Static Mixer (Refined Mesh)

 2.   In the Outline tree view of the Meshing application, expand Model and right-click Mesh and select
      Edit in CFX-Mesh to load CFX-Mesh.

Modifying the Mesh Settings in CFX-Mesh
The first step is to create a refined mesh size over the whole geometry.

 1.   In the Tree View, select Model > Mesh > Spacing > Default Body Spacing.
 2.   In the Details View, change Maximum Spacing to 0.2 m. This is a smaller length scale for the model
      than set previously (0.3 m).
 3.   Press Enter on the keyboard to set this value.

The next step is to create an Inflated Boundary on the walls of the mixer. Creating inflated boundaries gen-
erates prismatic elements from the surface by inflating triangular elements into the solid. As a result, near
the wall boundaries there will be layers of flat prismatic (wedge-shaped) elements which provide a smaller
mesh length scale in the direction perpendicular to the wall. This provides better resolution of the velocity
field near the wall, where it changes rapidly.

Inflation can greatly improve accuracy, particularly in a model with a high aspect ratio, such as a long narrow
pipe, or in a model where turbulence is significant. Inflation should always be used when you are interested
in lift, drag or pressure drop in the model.

Away from the wall boundaries, the mesh elements will be tetrahedral as they were in Tutorial 1.

First, you will set the parameters used to control the inflation process, and then you will create the Inflated
Boundary itself.

 1.   Click Inflation in the Tree View.
 2.   In the Details View, set Number of Inflated Layers to 5. This will give five layers of prism elements.
 3.   Set Expansion Factor to 1.3. This controls how fast the thickness of the prism elements grows in
      successive layers away from the wall.
 4.   Leave the other settings as their default values.
 5.   In the Tree View, right-click Inflation and select Insert > Inflated Boundary.
 6.   Click Default 2D Region under Regions in the Tree View to select the faces which are in the default
      2D region for the Inflated Boundary. Click Apply in the Details View. The text should change to read
      1 Composite.
 7.   Set Maximum Thickness to 0.2 m.

This creates an Inflated Boundary that uses all the faces in the Default 2D Region. If you later change the
2D Region settings so that the Default 2D Region contains different faces, the Inflated Boundary will auto-
matically update to always use the faces in the Default 2D Region at the time when the mesh is generated.

Generating the Surface Mesh
You will now have a look at the surface mesh to see the effect of the chosen length scale and the inflation,
compared to the mesh you generated for the previous example. You can use the existing Preview Group to
display the surface mesh.

 1.   Right-click Preview > Default Preview Group and select Generate Surface Meshes.



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
146                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                  Further Geometry Modification




You should be able to see that this mesh is finer and thus has more surface elements then the mesh you
generated in the first example. Also, note that there are triangular prism elements near the walls of the
mixer vessel, the edges of which can be seen when you look at the mesh on the two inlets or the outlet.

Generating the Volume Mesh
Now generate the volume mesh by right-clicking Mesh in the Tree View and selecting Generate Volume
Mesh.

This completes the mesh generation. Now save the project by selecting File > Save from the CFX-Mesh's
main menu and return to the Project Schematic without closing CFX-Mesh.

      Note

      Do not close CFX-Mesh at this time as the last part of this tutorial, Updating the Geometry in CFX-
      Mesh (p. 150), requires CFX-Mesh to be open to demonstrate how to update the geometry in CFX-
      Mesh. If you have accidently closed CFX-Mesh at this point, you need to open CFX-Mesh, as outlined
      in Tutorial 1, and then return to the Project Schematic.

From this point, this tutorial continues by modifying the geometry in order to illustrate how to set dimensions
on geometry objects and how to use the updated geometry in CFX-Mesh. The setting of dimensions is es-
sential when creating geometry features with dimensions not as simple fractions of the model units, and
thus cannot use the grid for positioning the points and lines in the sketches. If you do not wish to continue
with this tutorial, then from the Project Schematic select File > Exit to quit ANSYS Workbench.

Further Geometry Modification
In this section, you will change the radius of the inlet pipes to 0.4 m from the initial 0.5 m, without using
the grid to position the circle. You will then extend the outlet pipes.

 1.   On the Project Schematic, double-click Geometry cell in the Mesh system.
 2.   Once DesignModeler has opened, expand the ZXPlane and then select Sketch2 in the Tree View,
      noting which circle it contains. Click the Sketching tab.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                      147
Tutorial 2: Static Mixer (Refined Mesh)


           Note

           If you used the supplied geometry file StaticMixer.agdb to create the project for pre-
           vious tutorial then skip the next three steps, because the supplied geometry file already
           contains the dimension specified for radius.


 3.   Click Dimensions on the Sketching tab to open the Dimensions toolbox.
 4.   Click Radius and then select the circle which forms Sketch2 from the Graphics window.
 5.   Click somewhere in the Graphics window to choose where the label for this dimension will be placed.
      Its location does not affect the model in any way, and is purely for display purposes.
 6.   If you now look in the Details View at the bottom left of the screen, you will find a section headed
      Dimensions, which contains the radius R1, set to 0.5 m. For now, change the radius to be 0.4 m .
 7.   Click Generate        to activate the change.

You will see that both of the side pipes now have a reduced radius as required. The radius of both the pipes
changed simultaneously as the property of AutoConstraints is turned on by default. This automatically detects
dimensions which are equal and constrains them to be equal such that when one changes, the other does
also. See the DesignModeler Help for more details.

You have now explicitly defined the dimensions of the inlet pipe radii and can easily change it if you change
the geometry or make a mistake when originally specifying the radius. Whenever you are asked in later tu-
torials to create a geometry object of a particular size, you can either set up the grid to enable precise pos-
itioning of the geometry, or create the geometry at approximately the right size and then use the Dimensions
toolbox to specify the exact dimensions.

You can now extend the outlet pipe. The first part of the extension requires a Revolve operation. However,
you need to revolve the end surface of the existing outlet pipe, which is currently not defined as a sketch
or plane, so you must first construct the appropriate plane from which to revolve.

 1.   Create a new plane by using the New Plane                              button on the Active Plane/Sketch toolbar, located
      above the Graphics window.
 2.   In the Details View, set Type to be From Face and Subtype to be Outline Plane.
 3.   In the Details View, click in the box next to Base Face. There will now be two buttons, Apply and
      Cancel, which indicates that you are ready to select the face from the Graphics window.
 4.   In the Graphics window, click on the circular face at the end of the outlet pipe, which is at the position
      with the lowest value of the Z-coordinate. Click Apply in the Details View.
 5.   Click Generate        to create the plane.

The Revolve operation requires the specification of a rotation axis. Since this rotation will not be around any
of the main coordinate axes, a sketch containing a single line to act as the required axis will be created.

 1.   Select the new plane (Plane4) in the Tree View, and create a new sketch based on this plane by using
      the New Sketch           button on the Active Plane/Sketch toolbar located above the Graphics window.
 2.   Select the Sketching tab.
 3.   Click Settings in the Sketching tab to open the Settings toolbox.
 4.   Click Grid and select Show in 2D and Snap.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
148                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                   Further Geometry Modification

 5.   Click Major Grid Spacing and set it to 1.
 6.   Click Minor-Steps per Major and set it to 2.
 7.   From the Draw toolbox, select Line and then create a line which is parallel to the Y-axis and is posi-
      tioned at x = 2 m. You can use the grid settings to position this line. The length of the line and the
      exact position of its end points are not important since it is only going to be used to define a rotation
      axis.
 8.   Select Revolve        from the 3D Features toolbar.
 9.   In the Details View, click next to Base Object and then click on the name of the plane that you have
      just created (Plane4) in the Tree View. Click Apply in the Details View.
 10. In the Details View, click next to Axis and then click on the name of the sketch that you have just
     created (Sketch4) in the Tree View. Click Apply in the Details View.
 11. Set Angle to 60 degrees.
 12. Click Generate         to create the revolve.




One more operation is needed to add another straight section of pipe to the outlet. This follows a very
similar procedure to the one that you have just used to create the first extension.

 1.   Create a new plane by using the New Plane                              button on the Active Plane/Sketch toolbar, which is
      located above the Graphics window.
 2.   In the Details View, set Type to be From Face and Subtype to be Outline Plane.
 3.   In the Details View, click in the box next to Base Face. There will now be two buttons, Apply and
      Cancel, which indicates that you are ready to select the face from the Graphics window.
 4.   In the Graphics window, click on the circular face at the end of the newly revolved pipe section, which
      is in the position with the lowest value of the Z-coordinate.
 5.   Click Generate        to create the plane.
 6.   Select Extrude        from the 3D Features toolbar.
 7.   In the Details View, click next to Base Object and then click on the name of the plane that you have
      just created (Plane5) in the Tree View. Click Apply in the Details View.
 8.   Set Depth to 2 m.
 9.   Click Generate        to create the extrusion.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                      149
Tutorial 2: Static Mixer (Refined Mesh)




This finishes the geometry modification. Leave DesignModeler open and return to the CFX-Mesh setup.

Updating the Geometry in CFX-Mesh
In this section you will update the modified geometry in CFX-Mesh.

      Note

      If the CFX-Mesh interface is not open or has been closed accidently, you need to open CFX-Mesh,
      as outlined in Launching CFX-Mesh (p. 136).

      Upon launching CFX-Mesh at this time from the Project Schematic, a message will appear
      prompting you to read the upstream data. Click No, because this tutorial will demonstrate how
      to update the modified upstream geometry from within CFX-Mesh in the steps outlined below.

 1.   In CFX-Mesh, right-click Geometry in the Tree View. Select Update Geometry and click Yes in the
      dialog box to continue with the update.

      The Graphics window will refresh to show the new geometry, with the thinner inlet pipes and the
      longer outlet. Also, the Tree View will be updated to account for the fact that the original face for the
      end of the outlet pipe is no longer there that new faces on the sides and end of the new section of
      pipe have been added.

      Notice that the Tree View now shows that you have an invalid setup: various items show red exclam-
      ation marks . The problem is that the specification for the 2D Composite Region out is invalid since
      the face it was applied to no longer exists.
 2.   Click out in the Tree View. Select the circular face at the bottom of the mixer vessel, with the lowest
      value of the Z-coordinate.
 3.   Click Apply in the Details View.

      The model setup is now valid - the red status symbols have all gone from the Tree View.

      When you do a Geometry Update, any new faces are automatically added to the Default Preview Group
      and to the Default 2D Region. This means that you do not need to update Inflated Boundary 1 to
      include any new faces because it was set up to use the Default 2D Region as its location and the new
      faces will have been automatically added to this region.

The geometry has been successfully updated and the CFX-Mesh setup is ready to re-mesh. At this point you
can create a new surface or volume mesh.

When you are finished working in CFX-Mesh, close CFX-Mesh and the Meshing application, and return to
the Project Schematic. You can exit from ANSYS Workbench by selecting File >Exit from the main menu. If
you are asked to save the project, ensure that you do not overwrite your existing files created before the
geometry modification.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
150                                                of ANSYS, Inc. and its subsidiaries and affiliates.
Tutorial 3: Process Injection Mixing Pipe




This tutorial shows how to create a simple pipe junction, using the Sweep operation in DesignModeler to
create the pipe profile. The following geometry and meshing features are illustrated:

 •    Face spacing, for refining the mesh on a particular face
 •    Inflation
 •    Full surface mesh generation, to preview the full surface mesh.

Geometry Creation
Creating the Project
 1.    Open ANSYS Workbench and add a standalone Mesh system on the Project Schematic. Save it as In-
       jectMixer.wbpj. For details, see Creating the Project in ANSYS Workbench (p. 126).
 2.    Now add geometry to the project by using one of the following methods:
       •   If you want to skip the geometry creation part of this tutorial, use the supplied file InjectMix-
           er.agdb to import geometry into the project. Once the geometry has been added, the Geometry
           cell appears in an up-to-date state. For details, see Can I Skip the Geometry Creation? (p. 120).

           Now proceed to the section Mesh Generation in this tutorial.
       •   If you want to create the geometry manually, continue with the following instructions.
 3.    On the Project Schematic, right-click Geometry cell in the Mesh system and choose New geometry
       to open DesignModeler, specifying the units as meters.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               151
Tutorial 3: Process Injection Mixing Pipe


           Note

           If you have previously set the default unit by selecting either Always use project unit or
           Always use selected unit in DesignModeler, the units pop-up window will not appear.

           To access the units pop-up window upon subsequent openings of DesignModeler, open
           the Options dialog box by selecting Tools > Options from DesignModeler's main menu.
           In the Options dialog box, select DesignModeler > Units and set Units > Display Units
           Pop-up Window to Yes. For details, see Units in the DesignModeler Help.


           Note

           If you are using the Parasolid file supplied for this tutorial, see Tutorials Requiring Modifications
           When Importing CAD Files (p. 121).



Creating the Main Pipe
To create the main pipe, you will use the Sweep operation. Sweep requires the use of two sketches: one
defines the profile to be swept (in this case, a circle) and the other defines the path through which the
profile is swept. The profile will be created first.

 1.   Create a new plane as follows. Select XYPlane from the Tree Outline and click on New Plane   from
      the Active Plane/Sketch toolbar, near the top of the ANSYS Workbench window. Clicking on XYPlane
      first, ensures that the new plane is based on the XYPlane.
 2.   In the Details View, set Transform 1 (RMB) to Offset Z, and set the Value of the offset to -4 m.
 3.   Click on Generate          to create the plane.
 4.   Create a new sketch as follows. Select Plane4 from the Tree Outline and then click on New Sketch
         from the Active Plane/Sketch toolbar, near the top of the ANSYS Workbench window. Clicking on
      the plane first ensures that the new sketch is based on Plane4.
 5.   On the Sketching tab open the Settings toolbox and select Grid > Show in 2D and Snap.
 6.   Set Major Grid Spacing to 1 m and Minor-Steps per Major to 2.
 7.   Zoom in on the center of the grid, so that you can see the gridlines clearly. You can do this by holding
      down the right-mouse button and dragging a box over the desired viewing area.
 8.   On the Sketching tab open the Draw toolbox and select Circle. Draw a circle of radius 0.5 m, centered
      on X = 0 m, Y = -2 m. The grid settings that you have just set up will help you to position the circle
      and set its radius correctly.




Creating the Path




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
152                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                Creating the Side Pipe

 1.   On the Modeling tab select YZPlane, then click New Sketch                                         to create a new sketch based on the
      YZPlane.
 2.   On the Sketching tab open theSettings toolbox and select Grid > Show in 2D and Snap.
 3.   Set Major Grid Spacing to 1 m and Minor-Steps per Major to 2.
 4.   In the Draw toolbox, select Line to draw two straight lines on the sketch, as shown in the picture below.
      For reference, the coordinates of the endpoints of the lines are (Y = -2 m, Z = -4 m), (Y = -2 m, Z = 0
      m) for the horizontal line and (Y = 0 m, Z = 2 m), (Y = 4 m, Z = 2 m) for the vertical line.
 5.   In the Draw toolbox select Arc by Center and click once on the origin (center of the Arc shown in
      the picture below). Now select one of the end points of the arc, and then move the mouse round to
      the other end point and click on it to draw the quarter-circle. If the wrong part of the arc is drawn
      (that is, a 270 degree segment instead of a 90 segment), click Undo from the Undo/Redo toolbar and
      try again, making sure that after you click on the first end point, that you move the mouse in the
      correct direction for the arc that is to be drawn.




Making the Pipe Itself

 1.   Select Sweep       from the 3D Features toolbar.
 2.   Set the Profile to be Sketch1: click on Sketch1 in the Tree Outline and then click on Apply in the
      Details View at the bottom-left of the screen.
 3.   Set the Path to Sketch2: click on the Not selected text next to Path, click on Sketch2 in the Tree
      Outline, and then click Apply.
 4.   Click on Generate          to create the pipe.




Creating the Side Pipe
 1.   Create a new plane based on the ZXPlane: as before, first make ZXPlane active by clicking on it, then
      use New Plane         to create the plane based upon it.
 2.   In the Details View, set Transform 1 (RMB) to Offset Global Z, and set the Value of the offset to 2
      m.
 3.   Set Transform 2 to Offset Global Y and Value of the offset to -3 m.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                             153
Tutorial 3: Process Injection Mixing Pipe

 4.   Click on Generate           to create the plane.
 5.   With the new plane selected in the Tree Outline , create a New Sketch                                             .
 6.   On the Sketching tab open the Draw toolbox and select Circle to create the circle centered on the
      origin with a radius of 0.15 m. Create the circle initially with any convenient radius, and then open the
      Dimensions toolbox and select Radius to specify the radius more precisely, as described in "Tutorial
      1: Static Mixer" (p. 125) under Geometry Creation (p. 126).
 7.   Select Extrude        from the 3D Features toolbar.
 8.   Set Base Object to be the new sketch (Sketch3), and set Operation to Add Material.
 9.   Set Direction to Normal and Extent Type to Fixed. Set Depth to 3 m.
 10. Click on Generate            to create the side-pipe.

Note that the extrusion of Sketch3 has to reach the main pipe body, but that it does not matter if it extends
into the body. It is possible to extrude To Next, which means that the extrusion will stop when it meets
another geometry object, but the net effect would be no different than using the Fixed extent.

The geometry is now complete. From the DesignModeler's main menu, select File > Save Project to save
the project and return to the Project Schematic. Now the Geometry cell appears in an up-to-date state.

Mesh Generation
Launching CFX-Mesh
On the Project Schematic, right-click Mesh cell in the Mesh system and select Edit to launch the Meshing
application.

If you have configured your global settings to ensure that CFX-Mesh is loaded automatically, the Meshing
application will load followed by CFX-Mesh.

      Note

      You can configure the settings under Tools > Options to open CFX-Mesh automatically
      whenever you choose to create a new mesh. For details on how to perform this one-time setup,
      see Setting CFX-Mesh as the Default Method for Meshing (p. 119).


Setting up the Regions
Create the region for the side inlet:

 1.   Right-click over Regions in the Tree View and select Insert > Composite 2D Region.
 2.   Select the circular face at the end of the small side pipe. Click on Apply in the Details View.
 3.   Right-click the new region in the Tree View and select Rename. Change the name of the region to
      side inlet.

Create the region for the main inlet by repeating the instructions for creating the side inlet, however, with
the following differences:

 1.   You will select the circular face at the end of the main pipe that has the lowest Z-coordinate.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
154                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                     Generating the Surface Mesh

 2.   The Composite 2D Region will be called main inlet.

Create the region for the outlet as previously, but with these differences:

 1.   You will select the circular face at the other end of the main pipe with the highest Y-coordinate.
 2.   The Composite 2D Region will be called outlet.

Setting up the Mesh
Set the Maximum Spacing:

 1.   In the Tree View select Mesh > Spacing > Default Body Spacing.
 2.   In the Details View, change Maximum Spacing to 0.25 m and press Enter to set this value.

It is desirable to have a reasonably fine mesh in the region of the side pipe, since the features of the flow
in this region are likely to be smaller than the Maximum Spacing that you just set. To do this, you will set
a Face Spacing to concentrate nodes and elements in this region. You can specify how quickly the mesh
elements grow as you move away from the selected face using an expansion factor.

Face Spacings act like sources, determining the size and distribution of elements in the region around that
face. They affect both the triangular surface mesh and the volume mesh. It is also possible to create Controls,
which have a similar effect but are applied to points, lines or triangles instead of faces.

In this tutorial, you will define a Face Spacing on the exterior of the side pipe to control the size of the ele-
ments generated in the vicinity.

 1.   Right-click on Spacing and select Insert > Face Spacing.
 2.   Select the cylindrical face of the side pipe. Click on Apply in the Details View.
 3.   In the Details View, set Option to Constant, and set Constant Edge Length to 0.05 m. This sets the
      mesh length scale for the Face Spacing.
 4.   Set the Radius of Influence to 0.0 m. The mesh control is applied only to the surface and not to a
      volume surrounding the surface.
 5.   Set the Expansion Factor to 1.2. This specifies how quickly the mesh elements grow as you move
      away from the face. As you move away, each element will be approximately 1.2 times as big as the
      previous one in the region in which the expansion takes place, until the mesh length scale reaches
      the maximum spacing of 0.25 m, which was set in the last section.

Generating the Surface Mesh
You will now have a look at the surface mesh to see the effect of the chosen length scale.

 1.   Click on the plus sign next to Preview in the Tree View to open it up.
 2.   Right-click over Default Preview Group and select Generate Surface Meshes.

You should be able to see that the mesh is finer around the side pipe than it is elsewhere in the geometry.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                       155
Tutorial 3: Process Injection Mixing Pipe




Setting up Inflation
The velocity gradient near the pipe wall surface can vary significantly, so it is advisable to apply inflation in
these areas.
 1.   Click on Inflation in the Tree View.
 2.   In the Details View, check that Number of Inflated Layers is set to 5.
 3.   Leave the other settings at their default values.
 4.   In the Tree View, right-click on Inflation and select Insert > Inflated Boundary.
 5.   Click on Default 2D Region in the Tree View to select the faces that are in the Default 2D Region for
      the Inflated Boundary. Click on Apply in the Details View.
 6.   Leave Maximum Thickness at the default setting.

Generating the Volume Mesh
Finally, you can generate the volume mesh by right-clicking Mesh in the Tree View and selecting Generate
Volume Mesh.

This completes the mesh generation. Now save the project by selecting File > Save from CFX-Mesh's main
menu and return to the Project Schematic.

You can exit from ANSYS Workbench by selecting File > Exit from the main menu.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
156                                               of ANSYS, Inc. and its subsidiaries and affiliates.
Tutorial 4: Circular Vent




This tutorial creates the geometry and mesh for a simple chimney stack. The following geometry and
meshing features are illustrated:
 •    Controls, for refining the mesh along a line
 •    Inflation
 •    Preview Groups, for previewing part of the surface mesh.

Geometry Creation
Creating the Project
 1.    Open ANSYS Workbench and add a standalone Mesh system on the Project Schematic. Save it as
       CircVent.wbpj. For details, see Creating the Project in ANSYS Workbench (p. 126).
 2.    Now add geometry to the project by using one of the following methods:
       •   If you want to skip the geometry creation part of this tutorial, use the supplied file CircVent.agdb
           to import geometry into the project. Once the geometry has been added, the Geometry cell appears
           in an up-to-date state. For details, see Can I Skip the Geometry Creation? (p. 120).

           Now proceed to the section Mesh Generation in this tutorial.
       •   If you want to create the geometry manually, continue with the following instructions.
 3.    On the Project Schematic, right-click Geometry cell in the Mesh system and select New geometry to
       open DesignModeler, specifying the units as meters.

            Note

            If you have previously set the default unit by selecting either Always use project unit or
            Always use selected unit in DesignModeler, the units pop-up window will not appear.

            To access the units pop-up window upon subsequent openings of DesignModeler, open
            the Options dialog box by selecting Tools > Options from DesignModeler's main menu.
            In the Options dialog box, select DesignModeler > Units and set Units > Display Units
            Pop-up Window to Yes. For details, see Units in the DesignModeler Help.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               157
Tutorial 4: Circular Vent


            Note

            If you are using the Parasolid file supplied for this tutorial, see Tutorials Requiring Modifications
            When Importing CAD Files (p. 121).



Creating the Solid
The geometry consists of a cylindrical pipe, placed in the center of a cylindrical region.

 1.   With the XYPlane selected in the Tree Outline, create a New Sketch                                             .
 2.   Use Circle from the Draw toolbox on the Sketching tab to draw a circle in the new sketch, centered
      at the origin and with radius 10 m.

If you immediately extruded this circle, you would get a cylinder which consisted of three faces: circular top,
circular bottom and the curved cylindrical face. However, you will need to apply a boundary condition in
the CFD simulation to only half of the curved cylindrical face. The only way to do that effectively is to create
the cylindrical face in two parts. This means that you will need to modify the circle before extruding.

 1.   Select Construction Point at Intersection from the Draw toolbox. This is located at the bottom of
      the list.
 2.   Select the Y-axis and then select the circle somewhere near where it intersects the Y-axis. You should
      find that a point appears at the intersection.
 3.   Now select the Y-axis again, and select the circle somewhere near where the other intersection of it
      and the Y-axis occur. A second construction point should appear.




 4.   Select Split from the Modify toolbox of the Sketching tab. Right-click over the Graphics window and
      select Split Edge at All Points.
 5.   Click on the circle to perform the split.
 6.   Select Extrude         from the 3D Features toolbar.
 7.   Set Base Object to be the new sketch (Sketch1), and set Operation to Add Material. Set Depth to
      be 10 m.
 8.   Set Merge Topology? to No. This stops DesignModeler from optimizing the surfaces created by
      combining them where possible, which would prevent the splits in the circle from having any effect.
 9.   Click on Generate            to create the cylinder.

You will now cut material from this cylinder to form the vent itself.

 1.   With the XYPlane selected in the Tree Outline, create another New Sketch                                                  .
 2.   Use Circle from the Draw toolbox of the Sketching tab to draw a circle in the new sketch, centered
      at the origin and with radius 1 m.

                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
158                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                Setting up the Regions

 3.   Select Extrude        from the 3D Features toolbar.
 4.   Set Base Object to be the new sketch (Sketch2), and set Operation to Cut Material.
 5.   Set Depth to be 5 m, and click on Generate                              to cut the pipe out of the large cylindrical region.

The geometry is now complete. From the DesignModeler's main menu, select File > Save Project to save
the project and return to the Project Schematic. Now the Geometry cell appears in an up-to-date state.

Mesh Generation
Launching CFX-Mesh
On the Project Schematic, right-click Mesh cell in the Mesh system and select Edit to launch the Meshing
application.

If you have configured your global settings to ensure that CFX-Mesh is loaded automatically, the Meshing
application will load followed by CFX-Mesh.

      Note

      You can configure the settings under Tools > Options to open CFX-Mesh automatically
      whenever you choose to create a new mesh. For details on how to perform this one-time setup,
      see Setting CFX-Mesh as the Default Method for Meshing (p. 119).


Setting up the Regions
Create the region for the wind inlet:

 1.   Create a Composite 2D Region called Wind.
 2.   Select the large curved face with the lowest X-coordinates. Click on Apply in the Details View.

Create the region for the opening to the atmosphere:

 1.   Create a Composite 2D Region called Atmosphere.
 2.   Select the other large curved face with the highest X-coordinate and the top round surface with the
      highest Z-coordinate. Click on Apply in the Details View.

Create the region for the vent opening to the atmosphere:

 1.   Create a Composite 2D Region called Vent.

      Select the small circular face at the top of the vent to apply it to.
 2.   Click over the axes in the bottom right corner of the Graphics window in the position shown in the
      picture below. As you move the cursor into this position, the black “-Z”-axis will appear (it is not shown
      by default). Click this axis.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                            159
Tutorial 4: Circular Vent

      This viewing position allows you to see the bottom of the geometry and to look up the vent itself to
      see the small circular face at the top of the vent without it being behind another face. You can now
      select the face directly.
 3.   Click Apply to set the location.

Setting up the Mesh
Set the Maximum Spacing:

 1.   Click on Default Body Spacing in the Tree View, which is contained in Mesh > Spacing.
 2.   In the Details View, change Maximum Spacing to 2.0 m, and press Enter on the keyboard to set this
      value.

Create inflated surfaces for the vent and ground surfaces:

 1.   Click on Inflation in the Tree View.
 2.   In the Details View, set Number of Inflated Layers to 4.
 3.   Leave the other settings as their default values.
 4.   In the Tree View, right-click on Inflation and select Insert > Inflated Boundary.
 5.   Select the faces for the boundary. The two surfaces which it should be applied to are the side of the
      vent and the bottom of the large cylinder with the lowest Z-coordinates.
 6.   Set Maximum Thickness to 0.2 m.

Create a Control in the center of the vent to refine the mesh in this region of the simulation. You will use
a Line Control, which refines the mesh in the region around a line.

Point, Line and Triangle Controls all make use of the Point Spacing object. This defines a set of spacing values,
which can be applied to the various Controls as desired.

 1.   Right-click on Controls in the Tree View, and select Insert > Point Spacing.
 2.   In the Details View, set Length Scale to 0.33 m. Set Radius of Influence to 1.0 m, and Expansion
      Factor to 1.15.
 3.   Right-click on Controls in the Tree View, and select Insert > Line Control.
 4.   In the Details View, there will now be two buttons, Apply and Cancel. Click on Cancel without selecting
      anything in the Graphics window, and then right-click in the same place and select Edit. Enter 0 0 0
      to set the coordinates of the first Point.
 5.   Set the coordinates of the second Point to be 0 0 4 in the same way.
 6.   You want the specified Point Spacing to apply to both points, so leave Spacing Definitions set to
      Uniform.
 7.   Click in the box next to Spacing, and then click on Point Spacing 1 in the Tree View to select the
      appropriate Point Spacing for the Control. Press Apply to complete the selection.
 8.   In order to better see the inside of the vent, click on Geometry in the Tree View, and in the Details
      View, set Transparency to 80 %.

If you ensure that the new Line Control is selected in the Tree View, and look at the vent in the Graphics
window, you should be able to see where the Control has been created, as shown below. The line itself
should be clearly visible, and the two spheres at each end show the Radius of Influence.



                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
160                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                    Generating the Volume Mesh




Generating the Surface Mesh
To get a clear view of how the Control affects the mesh, it is convenient to generate just part of the surface
mesh.

 1.   Right-click over Preview in the Tree View, and select Insert > Preview Group.
 2.   Change the name of the preview group to Ground.
 3.   For Location, select the large circular face with a hole at the bottom of the geometry with the lowest
      Z-coordinate.
 4.   Now right-click over the preview group Ground in the Tree View, and select Generate This Surface
      Mesh. The surface mesh will be generated on the corresponding face.




Generating the Volume Mesh
Finally, you can generate the volume mesh by right-clicking Mesh in the Tree View and selecting Generate
Volume Mesh.

This completes the mesh generation. Now save the project by selecting File > Save from CFX-Mesh's main
menu and return to the Project Schematic.

You can exit from ANSYS Workbench by selecting File > Exit from the main menu.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                      161
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
162                               of ANSYS, Inc. and its subsidiaries and affiliates.
Tutorial 5: Blunt Body




This tutorial creates the geometry and mesh for a simulation of flow over a vehicle body shape. Due to the
symmetry of both the geometry and the flow pattern, only half of the body needs to be modeled. The fol-
lowing geometry and meshing features are illustrated:

 •    Face Spacing, for refining the mesh on a particular face
 •    Inflation
 •    Proximity, for refining the volume mesh where two faces are close together
 •    Preview Groups, for previewing part of the surface mesh.

Geometry Creation
Creating the Project
 1.    Open ANSYS Workbench and add a standalone Mesh system on the Project Schematic. Save it as
       BluntBody.wbpj. For details, see Creating the Project in ANSYS Workbench (p. 126).
 2.    Now add geometry to the project by using one of the following methods:
       •   If you want to skip the geometry creation part of this tutorial, use the supplied file BluntBody.ag-
           db to import geometry into the project. Once the geometry has been added, the Geometry cell
           appears in an up-to-date state. For details, see Can I Skip the Geometry Creation? (p. 120).

           Now proceed to the section Mesh Generation in this tutorial.
       •   If you want to create the geometry manually, continue with the following instructions.
 3.    On the Project Schematic, right-click Geometry cell in the Mesh system and select New geometry to
       open DesignModeler, specifying the units as meters.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               163
Tutorial 5: Blunt Body


           Note

           If you have previously set the default unit by selecting either Always use project unit or
           Always use selected unit in DesignModeler, the units pop-up window will not appear.

           To access the units pop-up window upon subsequent openings of DesignModeler, open
           the Options dialog box by selecting Tools > Options from DesignModeler's main menu.
           In the Options dialog box, select DesignModeler > Units and set Units > Display Units
           Pop-up Window to Yes. For details, see Units in the DesignModeler Help.


           Note

           If you are using the Parasolid file supplied for this tutorial, see Tutorials Requiring Modifications
           When Importing CAD Files (p. 121).



Creating the Body
To create the body shape, you will create a sketch and then extrude it. A Cut Material operation will then
be used to shape the rounded end of the body.

 1.   With the ZXPlane selected in the Tree Outline, create a New Sketch                                              .
 2.   Use Rectangle from the Draw toolbox of the Sketching tab to draw a rectangle as shown below (note
      the orientation and position of the axes which appear as dotted lines). The required dimensions are:
      H1 = 1.44 m, V2 = 5.22 m.




 3.   Select Fillet from the Modify toolbox of the Sketching tab, and enter 0.5 for the Radius in the box
      that opens to the right of the word Fillet.
 4.   Select the two corners of the geometry that are on the Z-axis, to create the two fillets, as shown below.




 5.   Select Chamfer from the Modify toolbox, and enter 1.11 for the Length in the box which opens to
      the right of the word Chamfer.
 6.   Select the top right corner of the geometry to create the chamfer, as shown below.




                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
164                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Creating the Body




 7.   Use Angle from the Dimensions toolbox to specify the angle between the chamfer and the top of
      the sketch to be 25 degrees, as shown below. If the wrong angle is displayed just after you click on
      the second edge, then before you click to position the dimension, right-click and select Alternate
      Angle until the correct angle is displayed. After you have selected both of the edges which form the
      angle, remember to click once to position the label before typing the angle, 25 degrees, into the Di-
      mensions box in the Details View.




 8.   Use Length from the Dimensions toolbox to specify the length of the slanted edge to be 1.11, as
      shown below.




The sketch is now complete, and can be extruded to form the body.

 1.   Select Extrude        from the 3D Features toolbar.
 2.   Set Base Object to be the new sketch, and set Operation to Add Material. Set Direction to Reversed.
 3.   Set Depth to be 0.9725 m, and click Generate                                to create the solid.

The front end of the blunt body is already rounded; however, more material needs to be cut away from it
to get the correct shape.

 1.   With the XYPlane selected in the Tree View, create a New Sketch                                           .
 2.   Click Look At Face/Plane/Sketch        to move the model to get a good view of the new sketch. This
      icon will always place the currently-selected object (a plane, face or sketch) in the center of the
      Graphics view, and rotate the model so that you are viewing the object perpendicularly (or, in the case
      of a non-planar face, so that you get a reasonable view of it). Right-click on the Graphics view and
      drag a box over the solid to zoom into it.
 3.   You need to create the sketch shown in the picture below. One way to do this is as follows:
      a.   Select Sketching > Draw > Polyline to draw two straight lines of the approximate length. After
           you have clicked to place the third point (at the end of the second line), right-click and select
           Open End to finish the polyline.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                            165
Tutorial 5: Blunt Body

      b.   Select Constraints > Equal Length and then click on the two straight lines. This ensures that
           they will always remain the same length, so if one changes, the other one will also change.
      c.   Select Draw > Arc by Tangent to draw the quarter-circle, then select the two end points of the
           polyline. If the wrong part of the arc is being drawn (that is, a 270 degree segment instead of a
           90 segment), just before you click on the second end point, right-click and select Reverse to
           correct it.
      d.   Use Vertical and Radius from the Dimensions toolbox to fix the two dimensions shown. The
           values required are: V1 = 0.9725 m, R2 = 0.5 m.




 4.   Select Extrude          from the 3D Features toolbar.
 5.   Set Base Object to be the new sketch (Sketch2), and set Operation to Cut Material.
 6.   Set Depth to be 1.5 m, and click Generate                              to cut away the material.

The end of your blunt body should now look the same as in the picture below.




Creating the Containing Box
The next step is to create the box around the blunt body to form the region for the fluid flow simulation.
To stop the new solid from merging with the blunt body, you must first freeze it, and give it a name to
identify it more easily later on.

 1.   In the Tree Outline, click on the plus sign next to 1 Part, 1 Body and select Solid from the tree under-
      neath this entry. In the Details View, you will now see the information relating to the body. Click Solid
      in the Details View, and change it to Blunt Body. Pressing Enter on the keyboard will let the name
      change take effect.
 2.   Select Tools > Freeze from the main menu to freeze the body.
 3.   With the ZXPlane selected in the Tree Outline, create a New Sketch                                              .
 4.   Select Sketching > Draw > Rectangle to draw a rectangle as shown below. Note that the rectangle
      extends below the bottom of the body (below the XYPlane). The required dimensions are: V5 = 12.39
      m, V6 = 17.61 m, H7 = 4.75 m, H8 = 0.25 m.




                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
166                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                Setting up the Regions




 5.   Select Extrude        from the 3D Features toolbar.
 6.   Set Base Object to be the new sketch (Sketch3), and set Operation to Add Material.
 7.   Set Direction to Reversed and Extent Type to Fixed. Set Depth to be 5.15 m, and click Generate
         to create the solid.

You can now cut out the blunt body from the containing box, to leave just the region of interest for the
CFD simulation.

 1.   Select Create > Body Operation from the main menu.
 2.   Set Type to Cut Material and Bodies to the blunt body. To select the blunt body, you can click Blunt
      Body in the Tree Outline, under 2 Parts, 2 Bodies.
 3.   Click Generate        to remove the blunt body from its containing box.

The geometry is now complete. From the DesignModeler's main menu, select File > Save Project to save
the project and return to the Project Schematic. Now the Geometry cell appears in an up-to-date state.

Mesh Generation
Launching CFX-Mesh
On the Project Schematic, right-click Mesh cell in the Mesh system and select Edit to launch the Meshing
application.

If you have configured your global settings to ensure that CFX-Mesh is loaded automatically, the Meshing
application will load followed by CFX-Mesh.

      Note

      You can configure the settings under Tools > Options to open CFX-Mesh automatically
      whenever you choose to create a new mesh. For details on how to perform this one-time setup,
      see Setting CFX-Mesh as the Default Method for Meshing (p. 119).


Setting up the Regions
Create the region for the inlet:

 1.   Create a Composite 2D Region called Inlet.
 2.   Select the rectangular face of the solid with the lowest X-coordinate to apply it to.

Create the region for the outlet:

 1.   Create a Composite 2D Region called Outlet.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                            167
Tutorial 5: Blunt Body

 2.   Select the rectangular face of the solid with the highest X-coordinate to apply it to.

Create the region for the top free-slip wall:

 1.   Create a Composite 2D Region called Free1.
 2.   Select the rectangular face of the solid with the highest Z-coordinate to apply it to.

Create the region for the side free-slip wall:

 1.   Create a Composite 2D Region called Free2.
 2.   Select the rectangular face of the solid with the lowest Y-coordinate to apply it to.

Create the region for the symmetry plane:

 1.   Create a Composite 2D Region called SymP.
 2.   Select the rectangular face of the solid with the highest Y-coordinate to apply it to.

It is a good idea to create a separate region on the surface of the blunt body for visualization purposes and
for setting mesh controls.

 1.   Create a Composite 2D Region called Body.
 2.   You need to select the nine faces of the blunt body to apply this to. This can be done using Box Select:
      whilst holding down the left mouse button, drag a box across the body surfaces, as shown in the
      picture below, to select them. All the surfaces which are fully enclosed in this box will be selected.
      Press Apply in the Details View to accept the selection.




Setting up the Mesh
Set the Maximum Spacing:

 1.   Click Default Body Spacing in the Tree View, which is contained in Mesh > Spacing.
 2.   In the Details View, change Maximum Spacing to 0.8 m, and press Enter on the keyboard to set this
      value.

It is desirable to have a reasonably fine mesh around the surfaces of the blunt body. You can create a Face
Spacing to concentrate nodes and elements in this region.

 1.   Right-click Spacing and select Insert > Face Spacing.
 2.   Select the Composite 2D Region Body by clicking on its name in the Tree View. Click Apply in the
      Details View.
 3.   In the Details View, set Option to Constant, and set the Constant Edge Length to 0.15 m. This sets
      the mesh length scale for the Face Spacing.
 4.   Set the Radius of Influence to 0.0 m, and Expansion Factor to 1.2.

                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
168                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                    Generating the Surface Mesh

You can use Inflation to produce a thin layer of prismatic elements around the body external surface and
along the ground.

 1.   Click Inflation in the Tree View. In the Details View, set Number of Inflated Layers to 5.
 2.   Set Expansion Factor to 1.3.
 3.   In the Tree View, right-click Inflation and select Insert > Inflated Boundary.
 4.   For Location, select both Body and Default 2D Region from the Tree View. Hold down the Ctrl key
      in order to select the second of these.
 5.   Set Maximum Thickness to 0.1 m.

Generating the Surface Mesh
Obtain a view of the surface mesh over the surface of the blunt body using a Preview Group:

 1.   Right-click Preview in the Tree View, and select Insert > Preview Group. Change the name of the
      Preview Group to Body.
 2.   For Location, select the Composite 2D Region Body from the Tree View.
 3.   Now right-click the Preview Group Body in the Tree View, and select Generate This Surface Mesh.
      The surface mesh will be generated on just the corresponding faces.

Next, take a look at the mesh on the symmetry plane:

 1.   Right-click Preview in the Tree View, and select Insert > Preview Group. Change the name of the
      Preview Group to SymP.
 2.   For Location, select the Composite 2D Region SymP from the Tree View.
 3.   Now right-click the Preview Group SymP in the Tree View, and select Generate This Surface Mesh.
      The surface mesh will be generated on just the corresponding faces.
 4.   Click the green Y-axis in the triad at the bottom right of the Graphics view to put the geometry into
      a good viewing position to inspect this mesh, and click the Preview Group SymP in the Tree View to
      display it.
 5.   Zoom into the region of mesh near the back of the Blunt Body (as shown in the picture below), using
      the right mouse button to drag a box to define the required viewing area.




If you look at the inflation layers between the Body and the Ground (bottom), then you will see that there
was not enough space for the mesher to add the full five layers of inflation (you may need to zoom in more
to be able to see this). To see why this happens, display the mesh as it was before the inflated layers were
generated.

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                       169
Tutorial 5: Blunt Body

 1.   Click Preview in the Tree View, and in the Details View, set Display Mesh to Mesh Before Inflation.
      Re-display the Preview Group SymP by clicking on its name in the Tree View.




You can now see that the gap between the Body and the ground is only about one to two elements thick,
given the mesh spacing around the Body. Since the total height of the Inflation Layers would be approximately
one element thick on each side of the gap, this explains why there is not enough room for the full 5 layers
of inflation that you set.

To avoid this problem without having to explicitly set a Face Spacing in the location of the small gap, you
can use Surface Proximity. Surface Proximity is a meshing feature that detects close surfaces, such as the
base of the body and the ground, and then refines the mesh so that a minimum number of mesh elements
span the gap. The default number of elements across the gap is 4, and this is the minimum recommended
when both faces have inflation, such as in this case.

You can turn on Surface Proximity as follows:

 1.   Click Proximity in the Tree View.
 2.   Set Surface Proximity to Yes and Elements Across Gap to 4.

Surface Proximity will attempt to add elements so that there will be four elements across the gap. However,
the SymP face uses the Default Face Spacing, which has set a minimum edge length of around 0.08 m. Since
the gap is only around 0.25 m, this is too restrictive and will prevent Surface Proximity from adding elements
evenly.

 1.   Select the Default Face Spacing under Spacing in the Tree View.
 2.   In the Details View, set the Minimum Edge Length to 0.01 m.
 3.   Regenerate the mesh on the Preview Group SymP by right-clicking on its name in the Tree View and
      selecting Generate This Surface Mesh.




                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
170                                                  of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                     Generating the Volume Mesh




You will see that more elements now span the gap. The surface mesher has detected the close proximity
of the two surfaces and refined the mesh in this region, leading to elements of a higher quality.

Surface Proximity is an automatic method that produces higher quality meshes for many geometries. However,
you should always check the size of the mesh produced, as it can dramatically increase the number of nodes.
In some cases it is important to use a minimum edge length to prevent over-refinement of the mesh; see
Surface Proximity in the CFX-Mesh Help for more details.

Set the Preview options back to show the inflated layers:

 1.   Click Preview in the Tree View, and in the Details View, set Display Mesh to Mesh After Inflation.
      Re-display the Preview Group SymP by clicking on its name in the Tree View.




You can now see that the full five layers of inflation are present.

Generating the Volume Mesh
Finally, you can generate the volume mesh by right-clicking Mesh in the Tree View and selecting Generate
Volume Mesh.

This completes the mesh generation. Now save the project by selecting File > Save from CFX-Mesh's main
menu and return to the Project Schematic.

You can exit from ANSYS Workbench by selecting File > Exit from the main menu.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                      171
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
172                               of ANSYS, Inc. and its subsidiaries and affiliates.
Tutorial 6: Butterfly Valve




This tutorial creates the geometry and mesh for a butterfly valve in a pipe. The following geometry and
meshing features are illustrated:
 •    Parasolid import of the valve geometry
 •    Splitting the geometry along a line
 •    Curvature-sensitive meshing
 •    Face Spacing, for refining the mesh on a particular face
 •    Inflation
 •    Proximity, for refining the volume mesh when two faces are close together
 •    Preview Groups, for previewing part of the surface mesh.

This tutorial requires you to have a copy of the Parasolid file PipeValve.x_t. If you do not have this file,
download it from http://www.ansys.com/dm_how_tos/cm_pipevalve.exe (you will need to execute the
downloaded file to extract the required Parasolid file).

Geometry Creation
Creating the Project
 1.    Open ANSYS Workbench and add a standalone Mesh system on the Project Schematic. Save it as
       PipeValve.wbpj. For details, see Creating the Project in ANSYS Workbench (p. 126).
 2.    Now add geometry to the project by using one of the following methods:
       •   If you want to skip the geometry creation part of this tutorial, use the supplied file PipeValve.ag-
           db to import geometry into the project. Once the geometry has been added, the Geometry cell
           appears in an up-to-date state. For details, see Can I Skip the Geometry Creation? (p. 120).

           Now proceed to the section Mesh Generation in this tutorial.
       •   If you want to create the geometry manually, continue with the following instructions.
 3.    On the Project Schematic, right-click Geometry cell in the Mesh system and select New geometry to
       open DesignModeler, specifying the units as millimeters.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               173
Tutorial 6: Butterfly Valve


            Note

            If you have previously set the default unit by selecting either Always use project unit or
            Always use selected unit in DesignModeler, the units pop-up window will not appear.

            To access the units pop-up window upon subsequent openings of DesignModeler, open
            the Options dialog box by selecting Tools > Options from DesignModeler's main menu.
            In the Options dialog box, select DesignModeler > Units and set Units > Display Units
            Pop-up Window to Yes. For details, see Units in the DesignModeler Help.


            Note

            If you are using the Parasolid file supplied for this tutorial, see Tutorials Requiring Modifications
            When Importing CAD Files (p. 121).



Setting up the Valve Geometry
The first step is to import the valve geometry.

 1.   Select File > Import External Geometry File... from the main menu.
 2.   In the file browser that appears, open the file PipeValve.x_t. If you do not have this file, refer to
      the introduction to this tutorial for details on where to find it.
 3.   Click on Generate            to import the valve.

The valve is imported with its flat faces parallel to the ZXPlane. For the simulation, the valve needs to be
tilted at an angle of 35 degrees, so the next step is to move it. In DesignModeler, the way to move a body
is to move it from one plane to another. You will need to create the new plane, and then use a Body Oper-
ation to transform the valve.

 1.   With the ZXPlane selected, create a New Plane                                .
 2.   In the Details View, set Transform 1 to Rotate about Global X, and set the Value of the rotation to
      -35 degrees.
 3.   Click on Generate            to create the plane.
 4.   Select Create > Body Operation from the main menu.
 5.   Set Type to Move and select the valve as Bodies. To select the valve, you can click on it in the
      Graphics window.
 6.   Set Source Plane to ZXPlane and Destination Plane to Plane4.
 7.   Click on Generate            to move the valve.
 8.   Click on ZXPlane to show the original plane, so that you can see where the valve has moved.




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
174                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Creating the Pipe




Creating the Pipe
You now need to create the pipe which surrounds the valve, in which the fluid flows. To stop the new solid
from merging with the valve, you must first freeze the valve solid. You will also give it a name to identify it
more easily later on.

 1.   In the Tree Outline, click on the plus sign next to 1 Part, 1 Body and then select Solid from the tree
      underneath this entry. In the Details View, you will now see the information relating to the body. Click
      on Solid, and change it to Valve. Pressing Enter on the keyboard will let the name change take effect.
 2.   Select Tools > Freeze from the main menu to freeze the valve.
 3.   With the XYPlane selected, create a new plane                              .
 4.   In the Details View, set Transform 1 to Offset Z, and set the Value of the offset to -100 mm.
 5.   Click on Generate           to create the plane. You may need to zoom out from the valve geometry to see
      the new plane.
 6.   With the new plane (Plane5) selected, create a New Sketch                                       .
 7.   Use Circle from the Draw toolbox of the Sketching tab to draw a circle in the new sketch, centered
      at the origin and with radius 20 mm.
 8.   Select Extrude        from the 3D Features toolbar.
 9.   Set Base Object to be the new sketch (Sketch1), and set Operation to Add Material.
 10. Set Depth to be 200 mm, and click on Generate                                   to create the pipe.

You can now subtract the solid material in the valve from the pipe, which will leave a valve-shaped hole in
the pipe. The remaining solid is the volume in which fluid flows and is ready to be set up in simulation.

 1.   Select Create > Body Operation from the main menu.
 2.   Set Type to Cut Material and Bodies to the valve. To select the valve, you can click on Valve in the
      Tree Outline, under 2 Parts, 2 Bodies.
 3.   Click on Generate           to remove the valve material from the pipe.

Although it is not easy to see, the pipe now has a valve-shaped hole in it.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                            175
Tutorial 6: Butterfly Valve




Splitting the Solid
Since this model exhibits symmetry about the YZPlane, you can divide it in two using a slice operation, and
then run the simulation on only one half, to reduce the computing resources required. The slice operation
can only be used on geometry which is frozen.

 1.   Select Tools > Freeze from the main menu.
 2.   Create a new sketch based on Plane5.
 3.   Use Line from the Draw toolbox of the Sketching tab to draw a single vertical line in the new sketch,
      along the Y-axis. The exact dimensions of the line are not important but the line must extent above
      the top of the geometry (Y = 20 mm) and below the bottom of the geometry (Y = -20 mm).
 4.   Select Extrude          from the 3D Features toolbar.
 5.   Set Base Object to be the new sketch (Sketch2), and set Operation to Slice Material.
 6.   Set Depth to be 200 mm, and click on Generate                                   to split the pipe.
 7.   Select Create > Body Operation from the main menu.
 8.   Set Type to Delete and Bodies to the half of the pipe which has positive X-coordinates, by clicking
      on it in the Graphics window.
 9.   Click on Generate            to remove the unwanted half of the pipe.




The geometry is now complete. From the DesignModeler's main menu, select File > Save Project to save
the project and return to the Project Schematic. Now the Geometry cell appears in an up-to-date state.

Mesh Generation
Launching CFX-Mesh
On the Project Schematic, right-click Mesh cell in the Mesh system and select Edit to launch the Meshing
application.


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
176                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Setting up the Mesh

If you have configured your global settings to ensure that CFX-Mesh is loaded automatically, the Meshing
application will load followed by CFX-Mesh.

      Note

      You can configure the settings under Tools > Options to open CFX-Mesh automatically
      whenever you choose to create a new mesh. For details on how to perform this one-time setup,
      see Setting CFX-Mesh as the Default Method for Meshing (p. 119).


Setting up the Regions
Create the region for the inlet:

 1.   Create a Composite 2D Region called inlet.
 2.   Select the semi-circular face of the pipe with the lowest Z-coordinate to apply it to.

Create the other regions:

 1.   Create a Composite 2D Region called outlet on the semi-circular face of the pipe with the highest Z-
      coordinate.
 2.   Create a Composite 2D Region called symP on the plane with the highest X-coordinate.
 3.   Create a Composite 2D Region called pipe wall on the semi-cylindrical pipe wall.

The remaining faces which form the valve, will be grouped into the Default 2D Region.

Setting up the Mesh
Set the Maximum Spacing:

 1.   Click on Default Body Spacing in the Tree View, which is contained in Mesh > Spacing.
 2.   In the Details View, change Maximum Spacing to 4.5 mm, and press Enter on the keyboard to set
      this value.

A fine mesh is required around the hinge of the valve and at the top and bottom of the valve plate. In this
tutorial, you will use curvature-sensitive meshing. Using this utility, the mesh will automatically be refined
in regions where the edges of the surfaces have a large curvature.

 1.   Click on Default Face Spacing in the Tree View, which is contained in Mesh > Spacing. This is a Face
      Spacing object which is applied to all faces which do not have a Face Spacing explicitly defined.
 2.   Set Option to Angular Resolution and set the Angular Resolution to 18 degrees. The mesh will be
      refined wherever two adjacent surface mesh faces make an angle of more than the number of degrees
      set by the Angular Resolution setting.
 3.   Set Minimum Edge Length to 0.5 mm. This prevents over-refinement in areas which have a very large
      curvature.
 4.   Set Maximum Edge Length to 4.5 mm and leave the other parameters set to the default settings.

The Face Spacing settings above will produce a fine mesh around the highly-curved parts of the valve. You
will also need to create another Face Spacing parameter to increase the mesh density in the region near
the valve hinge, where the faces are flatter and therefore not refined by the Angular Resolution setting.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                              177
Tutorial 6: Butterfly Valve

The four faces which are required for the location are the large flat faces of the valve. Since these can be
difficult to select, the following method is recommended:

 1.   In order to better see the faces of the valve, click on Geometry in the Tree View, and then in the Details
      View, set Transparency to 40 %.
 2.   Right-click on Spacing and select Insert > Face Spacing.
 3.   Put the model into the isometric view by clicking on the cyan ball in the triad at the bottom right of
      the Graphics window. Zoom into the valve itself by holding down the Shift key on the keyboard and
      the middle mouse button, and moving the mouse over the Graphics window. Position your cursor
      over the top valve face as shown in the picture below.




 4.   Now click with the left mouse button as if you wanted to select this face. However, instead the symmetry
      plane is selected, since it is that face which is on top. Note that when you click, four rectangles appear
      in a stack at the bottom left of the Graphics window, as highlighted in the picture below.




 5.   The rectangles represent all of the faces which were under your cursor when you clicked. The top-most
      rectangle, at the left side of the stack, is outlined in red to indicate that it is selected. You actually
      wanted to select the next face down, which is represented by the second rectangle from the left. Click
      on this rectangle to select the top face of the valve.




 6.   Select the three flat faces on the other side of the valve by holding down Ctrl and clicking on them.
      You may need to rotate the model slightly to make it possible to select all three.




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
178                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                     Generating the Surface Mesh




 7.   Click Apply in the Details View. You should see that the text next to Location now reads 4 2D Regions.
 8.   In the Details View, set Option to Constant, and set the Constant Edge Length to 2 mm.
 9.   Set the Radius of Influence to 0.0 m, and Expansion Factor to 1.3.

This tutorial uses Surface Proximity to automatically refine the mesh where two faces are close to each
other without intersecting.

 1.   Click on Proximity in the Tree View.
 2.   Set Surface Proximity to Yes and change Elements Across Gap to 3.

In general, a value of 3 elements across a gap is not recommended when you want to produce a high
quality mesh. A small value is used in this case to minimize the size of the mesh for the tutorial.

Set up Inflated Boundaries on the walls:

 1.   Click on Inflation in the Tree View. In the Details View, set Number of Inflated Layers to 5.
 2.   Set Expansion Factor to 1.35. This is a large expansion factor. Often, a value of 1.2 is acceptable.
 3.   Change Inflation Option > Option to First Layer Thickness, and set the First Prism Height to 0.5
      mm.

      The pipe wall is to be modeled as a rough wall with an equivalent sand grain roughness of 0.2 mm.
      To maintain the validity of the assumptions used in modeling rough walls, it is important that the
      thickness of the first element of the wall is not much smaller than the equivalent roughness height.
      In general, a value equal to the roughness height is recommended, which would be 0.2 mm here. It
      is also important that the mesh length scale does not increase dramatically in the transition from the
      last inflation layer to the rest of the volume mesh. The value chosen here for the first prism height,
      combined with the high expansion factor, allows the elements in the inflation layers to expand to a
      reasonable size before the transition to the rest of the volume mesh. To produce a good mesh for this
      geometry, a much smaller Maximum Spacing is required, allowing a First Prism Height of 0.2 mm to
      be used and a smooth transition from the last inflation layer to the bulk volume mesh.
 4.   In the Tree View, right-click on Inflation and select Insert > Inflated Boundary.
 5.   For Location, select both pipe wall and Default 2D Region from the Tree View. Hold down the Ctrl
      key in order to select the second of these.

Generating the Surface Mesh
Next, take a look at the mesh on the pipe wall:

 1.   Right-click over Preview in the Tree View, and select Insert > Preview Group. Change the name of
      the Preview Group to pipe wall.
 2.   For Location, select the Composite 2D Region pipe wall from the Tree View.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                       179
Tutorial 6: Butterfly Valve

 3.   Right-click over the Preview Group pipe wall in the Tree View, and select Generate Surface Mesh.
      The surface mesh will only be generated on the corresponding faces.
 4.   Click over the axes in the bottom right corner of the Graphics window in the position shown in the
      picture below. As you move the cursor into this position, the black “-X”-axis will appear (it is not shown
      by default). This will put the geometry into a good position for viewing the mesh.




Notice how the nodes are concentrated around the valve.

Generating the Volume Mesh
Finally, you can generate the volume mesh by right-clicking Mesh in the Tree View and selecting Generate
Volume Mesh.

This completes the mesh generation. Now save the project by selecting File > Save from CFX-Mesh's main
menu and return to the Project Schematic.

You can exit from ANSYS Workbench by selecting File > Exit from the main menu.




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
180                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
Tutorial 7: Catalytic Converter




This tutorial shows how to create the geometry and mesh for the inlet pipe and flange for a catalytic con-
verter. The following geometry and meshing features are illustrated:

 •    The Skin/Loft operation to extrapolate between sketch profiles
 •    Sketch Instances (copying and pasting an entire sketch)
 •    Inflation.

Geometry Creation
Creating the Project
 1.    Open ANSYS Workbench and add a standalone Mesh system on the Project Schematic. Save it as
       CatConv.wbpj. For details, see Creating the Project in ANSYS Workbench (p. 126).
 2.    Now add geometry to the project by using one of the following methods:
       •   If you want to skip the geometry creation part of this tutorial, use the supplied file CatConv.agdb
           to import geometry into the project. Once the geometry has been added, the Geometry cell appears
           in an up-to-date state. For details, see Can I Skip the Geometry Creation? (p. 120).

           Now proceed to the section Mesh Generation in this tutorial.
       •   If you want to create the geometry manually, continue with the following instructions.
 3.    On the Project Schematic, right-click Geometry cell in the Mesh system and select New geometry to
       open DesignModeler, specifying the units as centimeters.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               181
Tutorial 7: Catalytic Converter


           Note

           If you have previously set the default unit by selecting either Always use project unit or
           Always use selected unit in DesignModeler, the units pop-up window will not appear.

           To access the units pop-up window upon subsequent openings of DesignModeler, open
           the Options dialog box by selecting Tools > Options from DesignModeler's main menu.
           In the Options dialog box, select DesignModeler > Units and set Units > Display Units
           Pop-up Window to Yes. For details, see Units in the DesignModeler Help.


           Note

           If you are using the Parasolid file supplied for this tutorial, see Tutorials Requiring Modifications
           When Importing CAD Files (p. 121).



Creating the Sketches for the Inlet Flange
The first geometry operations are to create four sketches to define the profile of the inlet flange. Two of the
sketches are circles, and the other two consist of a more elongated shapes constructed from eight edges
(lines and curves). You will then use the Skin/Loft operation to connect the sketches. This operation requires
that all sketches have the same number of edges. The two circles will be constructed with eight edges and
have an orientation that gives the smoothest connecting surface when the Skin/Loft operation is applied.

 1.   With the XYPlane selected, click New Sketch                             .
 2.   On the Sketching tab open the Settings toolbox and select Grid > Show in 2D and Snap. Set Major
      Grid Spacing to 1 cm and Minor-Steps per Major to 2.
 3.   Open the Draw toolbox and select Circle to create a circle centered at the origin that has a radius of
      2.5 cm.
 4.   To break the circle into eight segments, open the Modify toolbox and select Split, then right-click on
      the Graphics window and select Split Edge into n Equal Segments.
 5.   Back on the Sketching tab, next to where you clicked on Split, you will now find a box that enables
      you to specify how many segments to break the circle into. Set it to 8 and select the circle in the
      Graphics window to perform the Split operation.

To re-orient the circle to give a smoother final surface, you will rotate it by 22.5 degrees.

 1.   Select Move from the Modify toolbox. In the two boxes that appear, set the rotation angle r to be
      22.5 degrees and leave the scale factor f unchanged.
 2.   Select all eight segments by clicking on each of them in turn.
 3.   Right-click over the Graphics window and select End/Use Plane Origin as Handle. This tells Design-
      Modeler that you have finished selecting the edges to copy, and that you want to use the origin of
      the plane as a reference point for the rotation and paste actions which follow.
 4.   Right-click in the Graphics window and select Rotate by r Degrees to perform the rotation. You will
      not see any effect of this yet because it is applied only when you paste the circle into its new position.
 5.   Right-click again and select Paste at Plane Origin. You should see the original circle move round by
      22.5 degrees. No translation took place since you pasted the reference point (the origin of the
      plane/center of the circle) back at the Plane Origin.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
182                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                 Creating the Sketches for the Inlet Flange

 6.   Right-click again and select End.




The second sketch (Sketch2) is the second circle, placed in a different plane and made slightly bigger. Rather
than constructing it from scratch and having to perform the Split and Move as you did for Sketch1, you will
just copy it from Sketch1.

 1.   On the Modeling tab, with the XYPlane selected, create a New Plane                                             .
 2.   In the Details View, set Transform 1 (RMB) to Offset Z, and set the Value of the offset to 1 cm.
 3.   Click on Generate         to create the plane.
 4.   Right-click on Plane4 in the Tree Outline and select Insert > Sketch Instance. A Sketch Instance is
      just a copy of an ordinary sketch.
 5.   In the Tree Outline, select Sketch 1; in the Details View, click the Apply button beside Base Sketch
      to set the base sketch to be Sketch1.
 6.   Set Scale to 1.05.
 7.   Click on Generate         to create the Sketch Instance.
 8.   To be able to see both sketches, right-click on each in turn in the Tree Outline, and select Always
      Show Sketch.

You should now be able to see that both sketches are clearly offset from each other, with the second being
slightly larger then the first.

The next sketch (Sketch3) is a different shape constructed of straight edges and quarter-circles.

 1.   With the XYPlane selected, create a New Plane                             .
 2.   In the Details View, set Transform 1 to Offset Z, and set the Value of the offset to 5 cm.
 3.   Click on Generate         to create the plane.
 4.   On the Sketching tab open the Settings toolbox and select Grid > Show in 2D and Snap. Set Major
      Grid Spacing to 5 cm and Minor-Steps per Major to 5.
 5.   Click on Look At Plane/Face/Sketch       to move the image in order to see the new plane. Zoom in
      a little by holding down the Shift key on the keyboard, pressing the middle mouse button and dragging
      the mouse upwards.
 6.   Select tools from the Draw toolbox on the Sketching tab to construct the shape shown below. For
      reference, the shape is 20 cm long and 12 cm high, and is orientated with the X-axis along the long
      axis of the shape.
      a.   Use Line to draw the four straight edges.


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                   183
Tutorial 7: Catalytic Converter

      b.     Use Arc by Tangent to draw the four quarter-circles. In each case, select the two end points of
             the arc. If the wrong part of the arc is being drawn (i.e. a 270 degree segment instead of a 90
             segment) just before you click on the second end point, then right-click and select Reverse to
             correct it.




 7.   Click on Generate            to create the Sketch Instance.

Sketch4 is just a copy of Sketch3.

 1.   On the Modeling tab with the XYPlane selected, create a New Plane                                                 .
 2.   In the Details View, set Transform 1 (RMB) to Offset Z, and set the offset to 6 cm.
 3.   Click on Generate            to create the plane.
 4.   Right-click on Plane6 in the Tree Outline and select Insert > Sketch Instance.
 5.   In the Tree Outline, select Sketch3; in the Details View, click Apply beside Base Sketch to set Sketch3
      as the base sketch for Sketch4.
 6.   Set Scale to 1.05.
 7.   Click on Generate            to create the Sketch Instance.
 8.   To see all four sketches, right-click on the last two sketches in turn in the Tree Outline and select Always
      Show Sketch.

Creating the Inlet Flange
Having created all four profiles, you can now create the solid that connects them by using the Skin/Loft
operation.

 1.   Click on the blue Z-axis in the triad at the bottom right of the Graphics window to put the geometry
      into a good viewing position for the selection.
 2.   Select Skin/Loft          from the 3D Features toolbar.
 3.   Either:
      •     Select the four profiles from the Graphics window by selecting the four edges shown in the picture
            below. You will need to hold down the Control key while selecting the second and subsequent
            edges. Select the edges in the correct order by taking the inside one first and then working outwards:
            the order of the profiles is important because the Skin/Loft operation will make a surface that
            smoothly interpolates between them in the order which you specify.

      or:
      •     Select the four profiles from the Graphics window by holding down the left mouse button and
            placing the cursor in approximately the middle of the center circle. While still holding down the
            left button, move the mouse slowly outwards towards the top left of the model view. As you pass
            over each sketch, it is selected and the edge that you passed the cursor over is highlighted. This


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
184                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                            Creating the Inlet Flange

         automatically selects the sketches in the correct order (from inside to outside), which is important
         because the Skin/Loft operation will make a surface which smoothly interpolates between them
         in the order which you specify.




 4.   Click on Apply after selecting the four profiles.

You will now be able to see gray lines connecting the vertices of the four profiles. The gray lines may be in
slightly different places, depending on exactly which edges you created first for each sketch. These lines are
called guide lines, and give you a preview of how the Skin/Loft operation will connect these vertices. Unfor-
tunately, the gray lines in the picture above indicate that the wrong vertices are being connected: if you
went ahead and created the solid without fixing this, the resulting shape would be very twisted. The correct
way to join the vertices is shown in the picture below.




Unless your vertices happen to be connected like the ones in the picture above, you will need to fix the
problem, as described below.

 1.   Right-click and select Fix Guide Line.
 2.   Select different edges on the sketches until the gray lines look correct.

Now continue to specify the settings for the Skin/Loft operation.

 1.   In the Details View for the Skin/Loft, set Merge Topology? to Yes. If you leave it as the default (No),
      then the solid that is created has 26 surfaces (a planar surface from the edges in Sketch1, a planar
      surface from the edges in Sketch4, and 24 surfaces for the smooth curved surfaces interpolated between
      the profiles). If you were to put a mesh onto this solid, you would have to use a small mesh size to
      get a good quality mesh on and near the smallest surfaces. However, if you choose to Merge Topology
      directly in DesignModeler, the resulting solid only has three surfaces: the smooth curved surface is
      created in one piece rather than 24 pieces. This solid can be meshed more evenly, even when using
      a coarser mesh size.
 2.   Click on Generate          to create the Skin/Loft.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                            185
Tutorial 7: Catalytic Converter

The solid should look like the picture below when appropriately orientated. See the notes below if the solid
does not look correct or if you get error messages when you generate it.




If your solid is not correct, try the following:

 •    Check that each of the four sketches has exactly eight edges, particularly if you get messages about
      profiles not having an equal number of edges. You can easily do this by selecting each sketch in the
      Tree Outline and reading the number of edges in the sketch from the Details View.
 •    Check that you have selected the profiles in the right order, particularly if you get messages about self-
      intersecting geometry. You can check the order by viewing the Details View for the Skin/Loft; the profiles
      are listed in the order of selection. Only the order 1-2-3-4 or 4-3-2-1 will allow the solid to be generated
      correctly. If your profiles are in the wrong order, then fix this as follows:
      1.   Right-click on Skin1 in the Tree Outline and select Edit Selections.
      2.   In the Details View, right-click on the name of the profile which is in the wrong order (e.g. Profile2),
           and use the commands Move to Top, Move up, Move down, and Move to Bottom to change
           the position of the profile.
      3.   Click on Generate             to modify the Skin/Loft.
 •    If you create a solid that is twisted, check that the guide lines are correct: see above for details.
 •    If your solid is generated but looks to be the wrong shape, you will have to check that each profile is
      correctly positioned, and that the planes you created (Plane4, Plane5 and Plane6) have the correct offsets
      and are all based on the XYPlane. You should also check that you have selected all four profiles and
      have not missed one.

Creating the Inlet Pipe
You can now create the inlet pipe that attaches to the flange that you have just created. The pipe consists
of two sections: a curved section and an extruded straight section.

The curved section of the pipe is a Revolve operation based on Sketch1. However, you need to create a line
to act as the axis for the rotation first.

 1.    With the XYPlane selected, create a New Sketch                                .
 2.    On the Sketching tab open the Draw toolbox and select Line to draw a line that is parallel to the Y-
       axis, at X = 15 cm. The length of the line is unimportant.
 3.    Select Revolve        from the 3D Features toolbar.
 4.    Set Base Object to Sketch1 and Axis to the line which you have just drawn.
 5.    Set Direction to Reversed and Angle to 45 degrees.
 6.    Click on Generate           to revolve the inlet pipe.



                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
186                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                Setting up the Regions




Finally, you can extrude to make the straight section of the pipe. However, you need to extrude from the
end surface of the pipe, which isn't currently defined as a sketch or plane, so first you need to construct the
appropriate plane.

 1.   Create a New Plane            .
 2.   Set Type to be From Face and Subtype to be Outline Plane.
 3.   Set Base Face to be the end of the pipe section which you have just created. This can be selected
      directly by clicking on it in the Graphics window.
 4.   Click on Generate           to create the plane.
 5.   Select Extrude        from the 3D Features toolbar.
 6.   Set Base Object to be the plane that you have just created (Plane7) and Depth to 10 cm.
 7.   Click on Generate           to create the extrusion.

The geometry is now complete. From the DesignModeler's main menu, select File > Save Project to save
the project and return to the Project Schematic. Now the Geometry cell appears in an up-to-date state.

Mesh Generation
Launching CFX-Mesh
On the Project Schematic, right-click Mesh cell in the Mesh system and select Edit to launch the Meshing
application.

If you have configured your global settings to ensure that CFX-Mesh is loaded automatically, the Meshing
application will load followed by CFX-Mesh.

      Note

      You can configure the settings under Tools > Options to open CFX-Mesh automatically
      whenever you choose to create a new mesh. For details on how to perform this one-time setup,
      see Setting CFX-Mesh as the Default Method for Meshing (p. 119).


Setting up the Regions
In this case, two 2D Regions are required, one on the end of the pipe to allow an Inlet or Outlet Boundary
Condition to be applied and a second on the end of the flange to allow an Interface to be created between
the flange and catalyst housing.


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                            187
Tutorial 7: Catalytic Converter

 1.   Create a Composite 2D Region called PipeEnd on the circular face at the end of the pipe: In the Tree
      View, right-click Regions > Insert > Composite 2D Region. Click on the circular face, then in the Details
      View click Apply. In the Tree View, right-click the new Composite 2D Region and rename it PipeEnd.
 2.   Create a Composite 2D Region called FlangeEnd on the planar face at the end of the flange (this has
      the highest Z-coordinate): In the Tree View, right-click Regions > Insert > Composite 2D Region. Click
      on the planar face, then in the Details View click Apply. In the Tree View, right-click the new Composite
      2D Region and rename it FlangeEnd.

The remaining faces are grouped into the Default 2D Region.

Setting up the Mesh
Set the Maximum Spacing:

 1.   In the Tree View select Mesh > Spacing > Default Body Spacing .
 2.   In the Details View, change Maximum Spacing to 1.0 cm, then press Enter.

You can use Inflation to produce a thin layer of prismatic elements along the walls of the converter.

 1.   In the Tree View, click on Inflation. In the Details View, set Number of Inflated Layers to 5.
 2.   Leave the rest of the parameters at their default values.
 3.   In the Tree View, right-click on Inflation and select Insert > Inflated Boundary.
 4.   For Location, select Default 2D Region from the Tree View.
 5.   Set Maximum Thickness to 0.5 cm.

Generating the Volume Mesh
Finally, you can generate the volume mesh by right-clicking Mesh in the Tree View and selecting Generate
Volume Mesh.

This completes the mesh generation. Now save the project by selecting File > Save from CFX-Mesh's main
menu and return to the Project Schematic.

You can exit from ANSYS Workbench by selecting File > Exit from the main menu.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
188                                                of ANSYS, Inc. and its subsidiaries and affiliates.
Tutorial 8: Annulus




This is a very simple example which shows how to mesh a two-dimensional geometry. The following geometry
and meshing features are illustrated:

•    Inflation
•    Extended Layer Growth for Inflation
•    Extruded 2D meshing.

Geometry Creation
Creating the Project
1.    Open ANSYS Workbench and add a standalone Mesh system on the Project Schematic. Save it as
      NonNewton.wbpj. For details, see Creating the Project in ANSYS Workbench (p. 126).
2.    Now add geometry to the project by using one of the following methods:
      •   If you want to skip the geometry creation part of this tutorial, use the supplied file NonNewton.ag-
          db to import geometry into the project. Once the geometry has been added, the Geometry cell
          appears in an up-to-date state. For details, see Can I Skip the Geometry Creation? (p. 120).

          Now proceed to the section Mesh Generation in this tutorial.
      •   If you want to create the geometry manually, continue with the following instructions.
3.    On the Project Schematic, right-click Geometry cell in the Mesh system and select New geometry to
      open DesignModeler, specifying the units as foot.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               189
Tutorial 8: Annulus


             Note

             If you have previously set the default unit by selecting either Always use project unit or
             Always use selected unit in DesignModeler, the units pop-up window will not appear.

             To access the units pop-up window upon subsequent openings of DesignModeler, open
             the Options dialog box by selecting Tools > Options from DesignModeler's main menu.
             In the Options dialog box, select DesignModeler > Units and set Units > Display Units
             Pop-up Window to Yes. For details, see Units in the DesignModeler Help.


             Note

             If you are using the Parasolid file supplied for this tutorial, see Tutorials Requiring Modifications
             When Importing CAD Files (p. 121).



Creating the Solid
 1.   With the XYPlane selected, create a New Sketch                                 .
 2.   Use Grid from the Settings toolbox of the Sketching tab to select Show in 2D and Snap.
 3.   Set Major Grid Spacing to 0.5 ft and Minor-Steps per Major to 4.
 4.   Use Circle from the Draw toolbox of the Sketching tab to create a circle centered on the origin with
      a radius of 0.5 ft.
 5.   Use Circle again to create another circle centered on X = 0 ft, Y = 0.125 ft, with a radius of 0.75 ft.
 6.   Select Extrude         from the 3D Features toolbar.
 7.   Set Base Object to be the sketch that you have just created (Sketch1) and Depth to 0.1 ft.
 8.   Click on Generate            to create the solid.

The geometry is now complete. From the DesignModeler's main menu, select File > Save Project to save
the project and return to the Project Schematic. Now the Geometry cell appears in an up-to-date state.

Mesh Generation
Launching CFX-Mesh
On the Project Schematic, right-click Mesh cell in the Mesh system and select Edit to launch the Meshing
application.

If you have configured your global settings to ensure that CFX-Mesh is loaded automatically, the Meshing
application will load followed by CFX-Mesh.

      Note

      You can configure the settings under Tools > Options to open CFX-Mesh automatically
      whenever you choose to create a new mesh. For details on how to perform this one-time setup,
      see Setting CFX-Mesh as the Default Method for Meshing (p. 119).


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
190                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Setting up the Mesh

Setting up the Regions
Create the 2D Regions:

 1.   Create a Composite 2D Region called rotwall on the inner wall, which will subsequently be rotating
      in the CFD simulation.
 2.   Create a Composite 2D Region called SymP1 on the planar face with the lowest Z-coordinate.
 3.   Create a Composite 2D Region called SymP2 on the planar face with the highest Z-coordinate.

Setting up the Mesh
Set the Maximum Spacing:

 1.   Click on Default Body Spacing in the Tree View, which is contained in Mesh > Spacing.
 2.   In the Details View, change Maximum Spacing to 0.02 ft, and press Enter on the keyboard to set this
      value. If you are using geometry which has come from the Parasolid import route, use the value 0.006
      m.

This mesh will be used to simulate the flow of a non-Newtonian fluid in ANSYS CFX, with its viscosity de-
pending upon the shear strain. A fine mesh is required on the inner and outer radius walls to resolve the
shear layers and accurately predict the viscosity variation in the boundary layer regions. You will use inflation
to create layers of prismatic elements on the Wall boundaries. For this tutorial, you will use the First Layer
Thickness option, which allows you to set the height of the first prism layer (i.e. the one which actually
touches the edge of the geometry). Successive prism layers are then added, each one of thickness equal to
the thickness of the previous layer multiplied by the Expansion Factor, until the height of the next prism
layer is approximately equal to its width/length. Since the last layer of prisms have approximately unit aspect
ratio (side lengths approximately equal), the transition between the prism elements and the tetrahedral
elements is smoother using this option. When the First Layer Thickness option is enabled, the Number of
Inflated Layers is used as a maximum number of layers rather than an actual number of layers.

In addition, this tutorial will use the Extended Layer Growth parameter. This is only available when the
First Layer Thickness option is selected, and it allows extra prism layers to be added beyond the point
where unit aspect ratio prisms are reached. Each of these extra layers is of the same thickness as the previous
layer, so that unit aspect ratio is maintained. Prisms continue to be added until either the Number of Inflated
Layers is reached or the prism layers begin to collide with each other or with the geometry boundaries.

The Extended Layer Growth option is being used here to ensure that as much of the geometry as possible
is filled with prisms. This results in a smoother flow pattern for a coarser mesh since the flow is mostly
aligned with the prism layers.

 1.   Click on Inflation in the Tree View. In the Details View, set Number of Inflated Layers to 40.
 2.   Set Expansion Factor to 1.3.
 3.   Set Inflation Option > Option to First Layer Thickness and set First Prism Height to 0.0012 ft or
      0.00037 m for Parasolid geometry.
 4.   Ensure that Extended Layer Growth is set to Yes.
 5.   In the Tree View, right-click on Inflation and select Insert > Inflated Boundary.
 6.   For Location, select Default 2D Region and rotwall from the Tree View.
 7.   Expand the Preview item in the Tree View, right-click over Default Preview Group, and select Generate
      Surface Meshes. You should be able to see that the prism layers almost fill the geometry.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                              191
Tutorial 8: Annulus

Setting up the Extruded 2D Mesh
CFX-Mesh has an Extruded 2D mesh capability which can be used to mesh two-dimensional geometries
(such as this one) or to extrude a mesh on one face through a specified translation to form an extruded
mesh consisting of triangular prisms and hexahedra. In each case, the geometry is created as a normal 3D
geometry. Once you activate the Extruded 2D Meshing capability, you must specify a Periodic Pair which
can be either translational or rotational: this identifies two sets of faces which map onto each other by the
specified transformation. When you mesh, the surface mesh (including Inflation) is generated as usual.
However, instead of volume meshing in the normal manner, all the mesh apart from the mesh on one
nominated set of faces (Location 1) is removed, and the mesh on Location 1 is swept through the transform-
ation specified for the Periodic Pair, giving the 2D or extruded mesh.

In order to set up the Extruded 2D mesh, you must first activate the capability, and then create an Extruded
2D Periodic Pair to define the direction of the extrusion.

 1.   Click on Options in the Tree View. In the Details View, set Meshing Strategy to Extruded 2D Mesh.
 2.   Set Number of Layers to 1. This will give a mesh which is just one layer thick along the Z-axis, so that
      the flow is truly two-dimensional. Higher values for the number of layers would give you an extruded
      mesh which could be used for three-dimensional flow, such as a pipe mesh with elements all aligned
      along the pipe direction.

After you have selected the Extruded 2D Mesh option, a new item will appear in the Tree View: Extruded
Periodic Pair. At first this shows as being invalid because the locations have not yet been specified.

 1.   Click on Extruded Periodic Pair.
 2.   For Location 1, select SymP1 from the Tree View.
 3.   For Location 2, select SymP2 from the Tree View.
 4.   Leave Periodic Type > Option set to Translational.
 5.   Since the sketches which were used to produce this geometry in DesignModeler consist entirely of
      circles which have no vertices, CFX-Mesh is unable to determine the translation vector automatically,
      and you must enter this in the boxes which appear. Set Translation Along X Axis to 0 ft, Translation
      Along Y Axis to 0 ft, and Translation Along Z Axis to 0.1 ft or 0.03048 m for Parasolid geometry.

Previewing the Surface Mesh
Next, take a look at the mesh which is produced.

 1.   Right-click over Default Preview Group, and select Generate Surface Meshes.
 2.   In order to view the mesh clearly, right-click over Preview in the Tree View, and select Insert > Preview
      Group. For Location, select Default 2D Region, rotwall, and SymP2 from the Tree View.
 3.   Click on Preview in the Tree View, and in the Details View, set Display Mode to Wire Mesh, Face
      Color Mode to Uniform, and Uniform Color to a dark color (double-click on the existing color to
      bring up a color selector).
 4.   Now click on Preview Group 1 in the Tree View to make it visible again.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
192                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                    Generating the Volume Mesh




You will be able to see that on the two curved surfaces, there are no triangles in the surface mesh. Instead,
the mesh on these faces consists of quad elements (four-sided elements) produced by extruding the mesh
from SymP1 to SymP2.

Generating the Volume Mesh
Finally, you can generate the volume mesh by right-clicking Mesh in the Tree View and selecting Generate
Volume Mesh.

This completes the mesh generation. Now save the project by selecting File > Save from CFX-Mesh's main
menu and return to the Project Schematic.

You can exit from ANSYS Workbench by selecting File > Exit from the main menu.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                      193
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
194                               of ANSYS, Inc. and its subsidiaries and affiliates.
Tutorial 9: Mixing Tube




This is a simple example which shows how to add extra surfaces to a model which can then be used for
boundary conditions. The picture above shows the geometry: the three circular holes will be used in the final
CFD simulation to inject the reactants to be mixed. They must exist as distinct surfaces to allow the inlet
boundary conditions to be defined in the simulation. The following geometry and meshing features are il-
lustrated:

 •    Imprint Surfaces, to add surfaces for boundary conditions
 •    Curvature-sensitive meshing
 •    Inflation
 •    Stretch, to reduce the number of elements along one axis
 •    Preview Groups, to view part of the surface mesh

Geometry Creation
Creating the Project
 1.    Open ANSYS Workbench and add a standalone Mesh system on the Project Schematic. Save it as Re-
       actor.wbpj.
 2.    Now add geometry to the project by using one of the following methods:
       •   If you want to skip the geometry creation part of this tutorial, use the supplied file Reactor.agdb
           to import geometry into the project. Once the geometry has been added, the Geometry cell appears
           in an up-to-date state. For details, see Can I Skip the Geometry Creation? (p. 120).

           Now proceed to the section Mesh Generation in this tutorial.
       •   If you want to create the geometry manually, continue with the following instructions.
 3.    On the Project Schematic, right-click Geometry cell in the Mesh system and select New geometry to
       open DesignModeler, specifying the units as millimeters.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               195
Tutorial 9: Mixing Tube


           Note

           If you have previously set the default unit by selecting either Always use project unit or
           Always use selected unit in DesignModeler, the units pop-up window will not appear.

           To access the units pop-up window upon subsequent openings of DesignModeler, open
           the Options dialog box by selecting Tools > Options from DesignModeler's main menu.
           In the Options dialog box, select DesignModeler > Units and set Units > Display Units
           Pop-up Window to Yes. For details, see Units in the DesignModeler Help.


           Note

           If you are using the Parasolid file supplied for this tutorial, see Tutorials Requiring Modifications
           When Importing CAD Files (p. 121).



Creating the Solid
The first step is to create the solid for the mixing tube.

 1.   With the XYPlane selected, create a New Sketch                                .
 2.   Use Rectangle from the Draw toolbox of the Sketching tab to create a rectangle which extends from
      0 < X < 60 mm and -10 mm < Y < -4 mm.
 3.   Select Revolve         from the 3D Features toolbar.
 4.   Set the axis for the rotation as follows. First, click on the line which forms the bottom of the rectangle
      (Y = -10 mm), and then click on Apply in the Details View.
 5.   Set Direction to Both - Symmetric and Angle to 15 degrees.
 6.   Click on Generate           to create the solid.

Notice that the curved surface of the solid consists of just one surface, as can be seen by clicking on it.




Breaking up the Curved Surface
You need to break up this surface so that the three circular holes are created as separate surfaces. To do
this, you will create a sketch containing the three circles, and then Extrude with Imprint Surfaces to effectively
project the circles onto the full curved surface.

 1.   With the ZXPlane selected, create a New Sketch                                .
 2.   Use Circle from the Draw toolbox of the Sketching tab to create three circles in this sketch, as shown
      below. The circles each have radius 0.75 mm, and their centers are positioned on the X-axis at 5 mm,


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
196                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                  Breaking up the Curved Surface

      15 mm and 25 mm from the Z-axis, respectively. First draw the circles in approximately the right pos-
      ition.
 3.   Now use Equal Radius from the Constraints toolbox of the Sketching tab to set two of the circles
      to have the same radius. Repeat to set the third circle to have the same radius as one of the other
      two.
 4.   Click on Dimensions in the Sketching tab to open the Dimensions toolbox.
 5.   Click on Radius and then select the first circle from the Model View.
 6.   Click somewhere in the Model View to choose where the label for this dimension will be placed. Its
      location does not affect the model in any way and is purely for display purposes.
 7.   If you now look in the Details View at the bottom left of the screen, you will find a section headed
      Dimensions, which contains the radius R1. Set this to be 0.75 mm. The other circles will automatically
      take the same radius.

      Note that if you happen to draw the circles sufficiently close to having an equal radius, then Design-
      Modeler will apply an Auto Constraint to the circles, constraining their radii to be equal. If this happens
      and you try to set the radius of both circles explicitly, then you will see a warning: “New dimension
      makes model over-constrained.” when you try to dimension the radius of the second or subsequent
      circle. If you do see this warning, then click OK to clear the warning and then right-click over the
      Graphics window and select Cancel. You will not need to set a dimension on this circle in this case:
      its radius will always be identical to the radius that you have already set.




Now you can create the Extrude.

 1.   Select Extrude        from the 3D Features toolbar.
 2.   Set Base Object to be the new sketch (Sketch2), and set Operation to Imprint Faces.
 3.   Set Direction to Reversed, Extent Type to be To Faces, and select the curved surface as the Target
      Face.
 4.   Click on Generate           to break up the surface.

You should now find that if you click on the curved surface of the solid, it consists of four separate surfaces:
the three circles and the remainder.




The geometry is now complete. From the DesignModeler's main menu, select File > Save Project to save
the project and return to the Project Schematic. Now the Geometry cell appears in an up-to-date state.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                      197
Tutorial 9: Mixing Tube


Mesh Generation
Launching CFX-Mesh
On the Project Schematic, right-click Mesh cell in the Mesh system and select Edit to launch the Meshing
application.

If you have configured your global settings to ensure that CFX-Mesh is loaded automatically, the Meshing
application will load followed by CFX-Mesh.

      Note

      You can configure the settings under Tools > Options to open CFX-Mesh automatically
      whenever you choose to create a new mesh. For details on how to perform this one-time setup,
      see Setting CFX-Mesh as the Default Method for Meshing (p. 119).


Setting up the Regions
Create the 2D Regions:

 1.   Create a Composite 2D Region called InWater on the nearly-triangular face with the lowest X-coordinate.
 2.   Create a Composite 2D Region called InAcid on the circular face nearest to the InWater 2D Region
      which you have just created. The circle is part of the curved face of the reactor.
 3.   Create a Composite 2D Region called InAlkali on the two remaining circular faces.
 4.   Create a Composite 2D Region called out on the nearly-triangular face with the highest X-coordinate.
 5.   Create a Composite 2D Region called sym1 on the planar face with the higher Z-coordinates.
 6.   Create a Composite 2D Region called sym2 on the planar face with the lower Z-coordinates.

Setting up the Mesh
Set the Maximum Spacing:

 1.   Click on Default Body Spacing in the Tree View, which is contained in Mesh > Spacing.
 2.   In the Details View, change Maximum Spacing to 0.6 mm, and press Enter on the keyboard to set
      this value.

A fine mesh is required around the circular inlets. In this tutorial, you will use curvature-sensitive meshing.
Using this utility, the mesh will automatically be refined in regions where the edges of the surfaces have a
large curvature.

 1.   Click on Default Face Spacing in the Tree View, which is contained in Mesh > Spacing. This is a Face
      Spacing object which is applied to all faces which do not have a Face Spacing explicitly defined.
 2.   Set the Angular Resolution to 18 degrees. The mesh will be refined wherever two adjacent surface
      mesh edges make an angle of more than the number of degrees set by the Angular Resolution setting.
 3.   Set Minimum Edge Length to 0.15 mm. This prevents over-refinement in areas which have a very
      large curvature.
 4.   Set Maximum Edge Length to 0.6 mm and leave the other parameters to the default settings.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
198                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                     Generating the Volume Mesh

Generating the Surface Mesh
To see the effects of curvature-sensitive meshing, preview the surface mesh on the wall of the reactor.

 1.   Right-click over Preview in the Tree View, and select Insert > Preview Group. Change the name of
      the Preview Group to wall.
 2.   For Location, select the curved surface of the geometry with the highest Y-coordinate.
 3.   Now right-click over the Preview Group wall in the Tree View, and select Generate This Surface Mesh.
      The surface mesh will be generated on just the corresponding faces.
 4.   Zoom into the area around the three circular inlets by clicking with the right mouse button and
      dragging a zoom box over the area required.




You will see that the mesh has been automatically refined around the three inlets.

Setting up Stretch and Inflation
Since the geometry is long and thin, it is appropriate to generate a stretched mesh to expand the mesh
elements in the X-direction. In practice, the geometry is expanded by the specified factors, meshing takes
place and then the geometry is contracted back to its original size. This results in fewer elements along the
length of the reactor without affecting how many elements are present in a cross-section of the tube.

 1.   Click on Stretch in the Tree View.
 2.   Set Stretch in X to 0.5 and leave the other stretch factors set to 1.
 3.   Regenerate the mesh by right-clicking on the Preview Group wall and selecting Generate This Surface
      Mesh.




It is a good idea to put inflation on the reactor wall.

 1.   Click on Inflation in the Tree View. In the Details View, set Number of Inflated Layers to 5.
 2.   Set Expansion Factor to 1.3. Leave the rest of the parameters as their default values.
 3.   In the Tree View, right-click on Inflation and select Insert > Inflated Boundary.
 4.   For Location, select the curved surface of the geometry with the highest Y-coordinate.
 5.   Set Maximum Thickness to 0.6 mm.

Generating the Volume Mesh
Finally, you can generate the volume mesh by right-clicking Mesh in the Tree View and selecting Generate
Volume Mesh.

This completes the mesh generation. Now save the project by selecting File > Save from CFX-Mesh's main
menu and return to the Project Schematic.

You can exit from ANSYS Workbench by selecting File > Exit from the main menu.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                      199
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
200                               of ANSYS, Inc. and its subsidiaries and affiliates.
Tutorial 10: Heating Coil




This tutorial creates the geometry and mesh for a heating coil, which consists of a solid copper coil in a
vessel containing liquid. Two solid bodies are required, one for the coil and one for the containing vessel.
The following geometry and meshing features are illustrated:

 •    The Sweep operation to create the coil
 •    Multiple solid bodies
 •    Body operations
 •    Face Spacing, to refine the mesh on a particular face
 •    Inflation
 •    Proximity
 •    Preview Groups, to view part of the surface mesh.

Geometry Creation
Creating the Project
 1.    Open ANSYS Workbench and add a standalone Mesh system on the Project Schematic. Save it as
       HeatingCoil.wbpj. For details, see Creating the Project in ANSYS Workbench (p. 126).
 2.    Now add geometry to the project by using one of the following methods:
       •   If you want to skip the geometry creation part of this tutorial, use the supplied file Heating-
           Coil.agdb to import geometry into the project. Once the geometry has been added, the Geometry
           cell appears in an up-to-date state. For details, see Can I Skip the Geometry Creation? (p. 120).

           Now proceed to the section Mesh Generation in this tutorial.
       •   If you want to create the geometry manually, continue with the following instructions.
 3.    On the Project Schematic, right-click Geometry cell in the Mesh system and select New geometry to
       open DesignModeler, specifying the units as meters.



                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                    of ANSYS, Inc. and its subsidiaries and affiliates.                               201
Tutorial 10: Heating Coil


           Note

           If you have previously set the default unit by selecting either Always use project unit or
           Always use selected unit in DesignModeler, the units pop-up window will not appear.

           To access the units pop-up window upon subsequent openings of DesignModeler, open
           the Options dialog box by selecting Tools > Options from DesignModeler's main menu.
           In the Options dialog box, select DesignModeler > Units and set Units > Display Units
           Pop-up Window to Yes. For details, see Units in the DesignModeler Help.


           Note

           If you are using the Parasolid file supplied for this tutorial, see Tutorials Requiring Modifications
           When Importing CAD Files (p. 121).



Creating the Profile and Path
You will use the Sweep action to create the coil which requires sketches to define the profile (the circle that
forms the cross-section for the coil) and the path around which it will be swept.

 1.   With the YZPlane selected, New Sketch                           to create a new sketch.
 2.   On the Sketching tab open the Settings toolbox and select Grid > Show in 2D and Snap. Set up the
      grid to have a Major Grid Spacing of 1 m and Minor-Steps per Major of 4.
 3.   Open the Draw toolbox and use Circle to create a circle centered on Y = 0.75 m, Z = 0.5 m with any
      convenient radius (that is, any radius that does not place the Y or Z axis as a tangent to the circle, as
      this would make the axis a constraint on the circle). Adjust the radius to 0.1 m by opening the Dimen-
      sions toolbox and using Radius: after clicking on Radius, click on the circle, then click slightly away
      from the circle. In the Details View, change the value of R1 to 0.1.
 4.   This tutorial will split the circle into two segments for reasons that will be explained later on. To break
      the circle into two pieces, open the Modify toolbox and select Split, then right-click in the Model View
      window and select Split Edge into n Equal Segments.
 5.   Back on the Sketching tab, next to where you clicked on Split, you will now find a box which allows
      you to specify how many segments to break the circle into. Set it to 2 and select the circle in the
      Model View window to perform the Split operation.
 6.   On the Modeling tab select the YZPlane, then click on New Sketch                                               to create Sketch2, based on
      the YZPlane as before.
 7.   On the Sketching tab open the Draw toolbox and select Line to create a single straight line along
      the Z-axis, from Z = 0.5 m to Z = 1.5 m.

Using Sweep to Make the Coil
 1.   From the 3D Features toolbar, select Sweep                              .
 2.   Set the Profile to be Sketch1: click on Sketch1 in the Tree Outline and then click on Apply in the
      Details View at the bottom-left of the screen.
 3.   Set the Path to Sketch2: click on the Not selected text next to Path, click on Sketch2 in the Tree
      Outline, and then click on Apply.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
202                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                         Extruding the Bottom End of the Coil

 4.   Set the Scale to 1.
 5.   Set the number of Turns to 2.
 6.   Click on Generate          to create the coil.




Extruding the Bottom End of the Coil
If you look at the geometry shown above, you will be able to see that the ends of the coil are extruded to
the edges of the container. However, the extrusion is not normal to the faces at the end of the coil: if you
were to extrude in the normal direction then the coil would look like the picture (a) below, whereas the
actual coil is shown in picture (b).




(a)                                   (b)

To create the extrusion in a direction that is not normal to the faces, you need to define a vector that gives
the direction for the extrude. You will create a vector to explicitly calculate the angle at which the extrusion
takes place in order to maintain the smooth gradient from the main coil into the extrusion. Straightforward
trigonometry shows that the angle between the path and the horizontal is 6.06 degrees:



 1.   With the ZXPlane selected, create a New Sketch                               .
 2.   On the Sketching tab open the Draw toolbox and select Line to create the line. To position it, place
      the first point at Z = 0 m, X = 0 m and then put the second point down at approximately the correct
      angle, as shown in the picture below. To orient the coil as shown in the picture, click on the green Y-
      axis arrow on the triad.
 3.   Now specify the exact angle as follows. Open the Dimensions toolbox and select Angle, then click
      on the X-axis, then on the line, and then on the X-axis again. If the wrong angle is displayed after you
      have selected the axis, then right-click and choose Alternate Angle until the correct angle is displayed.
      Click in the Model View window to position the angle label. Finally, type the angle, 6.06 degrees, into
      the Dimensions box in the Details View.

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                    203
Tutorial 10: Heating Coil




Use the Extrude operation:

 1.   From the 3D Features toolbar, select Extrude                              .
 2.   Set Base Object to be Sketch1, and set Operation to Add Material.
 3.   Right-click in the Tree Outline on Sketch3, and select Always Show Sketch. Click on Direction Vector
      to change it from just being None (Normal), then click on the single line in Sketch3 that defines the
      direction vector. Click Apply in the Details View. The text should now read 2D Edge.
 4.   Set Depth to be 1.2 m and Merge Topology? to No. Click on Generate                                                    to extrude the bottom
      end of the coil.

Extruding the Top End of the Coil
The actions above will be repeated to extrude the top part of the coil. However, there is no existing sketch
to extrude from; instead, you will create a new plane from the top circular end of the coil to use for this
purpose.

 1.   Create a New Plane            .
 2.   Set Type to be From Face and Subtype to be Outline Plane.
 3.   Set Base Face to be the circular face at the top of the coil. Hold down the middle-mouse button (or
      the mouse wheel) and drag the coil so that you can see the circular face. Click on Not selected, then
      click on the circular face in the Model View window, the click Apply.
 4.   Click on Generate           to create the plane.

Use the Extrude operation again:

 1.   From the 3D Features toolbar, select Extrude                              .
 2.   Set Base Object to be Plane4, and set Operation to Add Material.
 3.   Click on Direction Vector to change it from just being None (Normal). Click on the single line in
      Sketch3 that defines the direction vector, which is the same as for the previous Extrude. Click Apply
      in the Details View. The text should now read 2D Edge.
 4.   Set Direction to Reversed, Depth to 1.2 m, and Merge Topology? to No. Click on Generate                                                  to
      extrude the top end of the coil.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
204                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                            Creation of the Container

Trimming the Ends of the Coil
Now trim the ends of the coil as follows.

 1.   With the XYPlane selected, create a New Sketch                                .
 2.   Click the Look at face icon to orient the drawing.
 3.   On the Sketching tab open the Draw toolbox and select Circle to draw two circles in the new sketch.
      Both should be centered on the origin, and their radii should be exactly 1 m and at least 1.5 m respect-
      ively.
 4.   Select Extrude        from the 3D Features toolbar.
 5.   Set Base Object to be the new sketch, and set Operation to Cut Material.
 6.   Set Depth to be 2 m, and click on Generate                              to remove the ends of the pipes.

Creation of the Container
The next step is to create the container around the coil. DesignModeler has an Enclosure feature that allows
the easy creation of a cylindrical enclosure around a solid body and generates the cylinder automatically;
however, this only works if the solid body is not required to touch the edges of the enclosure. In this case,
the ends of the coil will touch the sides of the container, so although the Enclosure feature can be used,
you will have to construct the cylinder manually first.

The first steps are to freeze the coil, so that it is not affected by the next geometry creation actions, and to
give it a name, so that it can easily be identified later.

 1.   Select Tools > Freeze.
 2.   In the Tree Outline, click on the plus sign next to 1 Part, 1 Body and then select Solid from the tree
      underneath this entry. In the Details View, you will now see the information relating to the body. Click
      on the word Solid in this information, and change it to read Coil. Press Enter to have the name change
      take effect.
 3.   With the XYPlane selected, create a New Sketch                                .
 4.   On the Sketching tab open the Draw toolbox and select Circle to draw two circles in the new sketch.
      Both should be centered on the origin, and their radii should be exactly 1 m and 0.5 m respectively.
      Since a circle of radius of 1 m already exists in an earlier sketch, you may find that if you try to set the
      radius of the outer circle to be 1 m using the Dimensions toolbox, you get a warning: “New dimension
      makes model over-constrained.” This occurs if DesignModeler has applied Auto Constraints to your
      new circle, already constraining the radius to be 1 m to match the existing circle. If you do see this
      warning, then click OK to clear the warning and then right-click over the Model View window and
      select Cancel. You will not need to set a dimension on this circle in this case.
 5.   Select Extrude        from the 3D Features toolbar.
 6.   Set Base Object to be the new sketch, and set Operation to Add Material.
 7.   Set Depth to be 2.25 m, and click on Generate                                to create the container.
 8.   In the Tree Outline, under 2 Parts, 2 Bodies, click on Solid. In the Details View, click on Solid, and
      rename it to Container, then press Enter.

The next step is to cut the coil out from the container, using the Enclosure feature:


                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                           205
Tutorial 10: Heating Coil

 1.   From the main menu, select Tools > Enclosure.
 2.   Set Shape to User Defined.
 3.   Select the container as the User Defined Body. To select it, you can click on Container in the Tree
      Outline under 2 Parts, 2 Bodies, then click Apply.
 4.   Set Merge Parts? to Yes. This ensures that the final bodies are all in one part, and saves you from
      having to merge them into one part explicitly later on. The Merge Parts operation is able to operate
      more reliably if the surfaces that form the interface between the two parts are not just closed loops.
      This is the reason for breaking the circle in Sketch 1 into two separate pieces.
 5.   Click on Generate           to cut the coil out from the container.

This operation cuts a coil-shaped hole in the container, without deleting the coil, as required.

The geometry is now complete. From the DesignModeler's main menu, select File > Save Project to save
the project and return to the Project Schematic. Now the Geometry cell appears in an up-to-date state.

Mesh Generation
Launching CFX-Mesh
On the Project Schematic, right-click Mesh cell in the Mesh system and select Edit to launch the Meshing
application.

If you have configured your global settings to ensure that CFX-Mesh is loaded automatically, the Meshing
application will load followed by CFX-Mesh.

      Note

      You can configure the settings under Tools > Options to open CFX-Mesh automatically
      whenever you choose to create a new mesh. For details on how to perform this one-time setup,
      see Setting CFX-Mesh as the Default Method for Meshing (p. 119).


Setting up the Regions
Create the 2D Regions:

 1.   Create a Composite 2D Region called inflow on the large annular face with the lowest Z-coordinate:
      right-click on Regions and select Insert > Composite 2D Region. Right-click on Composite 2D Region
      and select Rename to change the name to inflow.
 2.   Create a Composite 2D Region called outflow on the large annular face with the highest Z-coordinate
      as above.

Finally, you need to create a Composite 2D Region on the coil itself. First, you need to understand an important
distinction between 2D Regions and solid faces that applies when there is more than one Solid Body present
in the model (which is what we have here: one solid is the coil, and the other is the container). Where two
Solid Bodies meet at a common face, there is just one face present in the geometry; however, there are two
2D Regions, as shown in the example below.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
206                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Setting up the Mesh




If your model has only one solid, then there is no difference between a face and 2D Region. If your model
has more than one solid, then all of the external faces will also be 2D Regions. However, two 2D Regions
will exist for every internal (shared) face.

So when you create the Composite 2D Region on the coil, you have to be very clear which side of the face
you want to select to include in the 2D Region. Since you are going to be applying Inflation to the 2D Region,
you need to select the 2D Regions on the container side of the faces, so that the Inflation grows into the
container (where you have fluid flow and need to resolve the boundary well) and not into the coil itself
(where there is only heat transfer and no particular need to resolve the boundary fields).

To make the selection easier and to ensure that you only pick 2D Regions on the container side and not the
coil side, you will first suppress the coil. This ensures that only the container faces can be picked.

 1.   Click on the plus sign next to Geometry in the Tree Outline to open it up. Click on the plus sign next
      to Part to show that the Part contains two bodies.
 2.   Click on the name of each body in turn: this highlights the appropriate body in the Graphics window.
 3.   Right-click Coil and select Hide. The Hide function stops the body from being displayed in the
      Graphics window and prevents you from selecting its faces; however, it will still be meshed. In this
      case, Hide makes selection of the required faces easier in the next step.
 4.   In the Tree View, right-click over Regions and select Insert > Composite 2D Region. Change its name
      to coil surface.
 5.   Click on the green Y-axis in the triad at the bottom right of the Graphics window to put the geometry
      into a good viewing position for the selection.
 6.   In order to better see the inside of the coil, click on Geometry in the Tree View, and in the Details
      View, set Transparency to 40 %.
 7.   Click back on the new Composite 2D Region in the Tree View, and then select all six of the coil faces,
      clicking Apply to finalize the selection. These can be most easily selected by using Box Select (drag a
      box across the Graphics window which encloses the whole of the coil but not the whole of the cylinder
      while holding down the left mouse button).

      If you appear to have only five or four faces making up the coil surface, then go back to your Design-
      Modeler tab and check that you set Merge Topology? to No for both of your Extrude operations. If
      you find that you did make a mistake in DesignModeler, then fix the problem in DesignModeler
      (making sure that you press Generate to apply the changes) and then in CFX-Mesh, right-click over
      Geometry in the Tree View and select Update Geometry to update the CFX-Mesh session to use the
      corrected geometry.
 8.   Note that the coil body is still hidden. Right-click on the Coil body and select Show.

Setting up the Mesh
Set the Maximum Spacing:

 1.   In the Tree View, select Mesh > Spacing > Default Body Spacing.
 2.   In the Details View, change Maximum Spacing to 0.1 m and press Enter.


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                              207
Tutorial 10: Heating Coil

 3.   Right-click on Spacing and select Insert > Face Spacing.
 4.   In the Details View, set Option to Constant, and set the Constant Edge Length to 0.07 m.
 5.   Set the Radius of Influence to 0.0 m, and Expansion Factor to 1.2.
 6.   For Location, select the Composite 2D Region coil surface from the Tree View and click Apply.

Note that the Composite 2D Region coil surface contains only one side of the coil faces, not both. However,
by setting a Face Spacing on this region, you are implicitly controlling the face spacing on both sides of the
coil face because the surface mesh on both sides of the faces must be identical.

Proximity will greatly improve the mesh for this tutorial. However, in order to keep the number of elements
down for tutorial purposes, the number of elements across the gap is reduced from the recommended
number 4 to 2.

 1.   In the Tree View, click Mesh > Proximity.
 2.   Set Surface Proximity to Yes and change Elements Across Gap to 2.

Create an Inflated Boundary on the coil:

 1.   In the Tree View, click on Inflation; in the Details View, set Number of Inflated Layers to 4.
 2.   Leave the rest of the parameters at their default values.
 3.   In the Tree View, right-click on Inflation and select Insert > Inflated Boundary.
 4.   For Location, select coil surface from the Tree View.
 5.   Set Maximum Thickness to 0.1 m.

Because only one side of the faces that form the boundary between the coil and container are contained
in coil surface, inflation will take place only on the container side of the faces.

Generating the Surface Mesh
You can visualize your inflation layer to see the effect of choosing only one side of the coil faces for Inflation.

 1.   Right-click over Preview > Default Preview Group, and select Generate Surface Meshes.

Your mesh should show that the inflated layers are all outside the coil. You may see that the inflation layers
do not go all the way round the coil ends; this is because the coil meets the container at a very shallow
angle and the inflator cannot easily fill the very narrow gap.

You may also find that the surface mesh generation process produces warnings about poor angles. This in-
dicates that the mesh is not of a high quality, and it is the result of meshing this geometry with over-coarse
length scales (in order to keep the solution time down for tutorial purposes).

Now create another inflated boundary on the wall of the container:

 1.   In the Tree View, right-click on Inflation and select Insert > Inflated Boundary.
 2.   For Location, select the outside and inside walls of the container (Ctrl-click on the large cylindrical
      face and the inner cylindrical face) from the Graphics window, then click Apply.
 3.   Set Maximum Thickness to 0.1 m.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
208                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                   Generating the Volume Mesh

Generating the Volume Mesh
Finally, you can generate the volume mesh by right-clicking Mesh in the Tree View and selecting Generate
Volume Mesh.

This completes the mesh generation. Now save the project by selecting File > Save from CFX-Mesh's main
menu and return to the Project Schematic.

You can exit from ANSYS Workbench by selecting File > Exit from the main menu.




                    Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                of ANSYS, Inc. and its subsidiaries and affiliates.                                      209
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
210                               of ANSYS, Inc. and its subsidiaries and affiliates.
Tutorial 11: Airlift Reactor




This tutorial creates the geometry and mesh for an airlift reactor or bubble column. The two figures above
show the geometry created in DesignModeler (left) and a schematic picture of the full geometry, not to
scale (right). In the CFD simulation, the air is input through a small ring sparger. It then rises up to the top
of the geometry and leaves the reactor. A thin draft tube helps to stabilize the rising plume of bubbles. The
full geometry is rotationally symmetric, so only a 30-degree segment needs to be modeled.

The draft tube will modeled as a “thin surface” (which has no thickness), and so it must be created as an
internal face of a separate body, which will need to be created in DesignModeler. The following geometry
and meshing features are illustrated:

 •    Multiple solid bodies
 •    Imprint Surfaces, to add surfaces for boundary conditions
 •    Face Spacing, to refine the mesh on a particular face.

Geometry Creation
Creating the Project
 1.    Open ANSYS Workbench and add a standalone Mesh system on the Project Schematic. Save it as
       BubbleColumn.wbpj. For details, see Creating the Project in ANSYS Workbench (p. 126).
 2.    Now add geometry to the project by using one of the following methods:
       •   If you want to skip the geometry creation part of this tutorial, use the supplied file Bubble-
           Column.agdb to import geometry into the project. Once the geometry has been added, the
           Geometry cell appears in an up-to-date state. For details, see Can I Skip the Geometry Creation? (p. 120).



                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               211
Tutorial 11: Airlift Reactor

          Now proceed to the section Mesh Generation in this tutorial.
      •   If you want to create the geometry manually, continue with the following instructions.
 3.   On the Project Schematic, right-click Geometry cell in the Mesh system and select New geometry to
      open DesignModeler, specifying the units as centimeters.

            Note

            If you have previously set the default unit by selecting either Always use project unit or
            Always use selected unit in DesignModeler, the units pop-up window will not appear.

            To access the units pop-up window upon subsequent openings of DesignModeler, open
            the Options dialog box by selecting Tools > Options from DesignModeler's main menu.
            In the Options dialog box, select DesignModeler > Units and set Units > Display Units
            Pop-up Window to Yes. For details, see Units in the DesignModeler Help.


            Note

            If you are using the Parasolid file supplied for this tutorial, see Tutorials Requiring Modifications
            When Importing CAD Files (p. 121).



Creating the Main Solid
The first step is to create the main solid.

 1.   With the XYPlane selected, create a New Sketch                                 .
 2.   Use Polyline from the Draw toolbox of the Sketching tab to create a closed polyline in the shape
      shown below (the Y-axis is vertical). To close the polyline, right-click over the Graphics window after
      you have selected the last point and select Closed End.




 3.   Use Circle from the Draw toolbox to create the circle shown in the diagram.
 4.   Use the Dimensions toolbox of the Sketching tab to add the dimension labels H1, H2, etc. shown in
      the picture. It does not matter if your labels do not have the same names as the ones in the picture.
                                                                                                       ,
      You will need to use the Horizontal, Vertical and Radius items from this toolbox to label the “H” “V”
      and “R” dimensions, respectively.
 5.   To ensure that the length of the bottom of the reactor is the same as the length of the top (H1), select
      Equal Length from the Constraints toolbox of the Sketching tab, and then select the top and bottom
      edges of the sketch. This ensures then when you set (or change) the dimension H1, both top and
      bottom of the reactor are affected.


                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
212                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                           Breaking the Sparger Surface to form the Inlet

 6.   Now use the table below to assign actual lengths to the dimensions listed in the Details View. Since
      the original sketch is not to scale, you will find that the geometry changes shape as you apply each
      one, particularly when you specify the bubble column height.

      Dimension name                                                                           Dimension label in picture            Length
                                                                                                       above
      Column radius                                                                                                H1                8.0 cm
      Distance between draft tube and outside of column                                                            H2                2.5 cm
      Distance between axis and sparger                                                                            H3                3.0 cm
      Height of column                                                                                              V4               77.0 cm
      Distance between top of draft tube and column top                                                             V5               3.5 cm
      Distance between bottom of draft tube and column base                                                         V6               3.5 cm
      Height of sparger above column base                                                                           V7               3.5 cm
      Radius of sparger                                                                                             R8               0.4 cm


Now you can use this sketch to create the solid body.

 1.   Select Revolve        from the 3D Features toolbar.
 2.   Set the axis for the rotation by clicking on the Y-axis and then clicking on Apply in the Details View.
 3.   Leave Direction set to Normal and Angle set to 30 degrees.
 4.   Click on Generate           to create the solid.

Breaking the Sparger Surface to form the Inlet
When the CFD simulation is run, the gas is injected through the top of the small circular hole, through a 74-
degree segment. Currently, the hole is defined with just one surface, so this must be broken to allow the
boundary conditions to be appropriately defined. The steps below explain how to modify the solid to achieve
this. All of this could have been done as part of the original construction of the solid, but this tutorial has
split the steps up to make it clear exactly what each step achieves.
 1.   The display will be clearer for the next step if you hide the solid for now: double-click on 1 Part, 1
      Body in the Tree Outline, right-click on Solid, and choose to Hide Body.
 2.   Select Sketch1 from the Tree Outline and go to the Modify toolbox of the Sketching tab.
 3.   Click on Split, and break the circle into two parts by clicking on it in approximately the positions shown
      in the picture below. The exact position of breaks does not matter for the moment, but make sure
      that you do not choose break points that are symmetrical about the vertical axis, i.e., the points should
      not be exactly at the highest or widest points of the circle.

      If you create points that are too symmetrical about the vertical axis, DesignModeler will automatically
      apply a constraint, which prevents you from positioning break points based on an angle of symmetry
      that is required later in the tutorial.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                     213
Tutorial 11: Airlift Reactor




Simply breaking the circle into two parts and regenerating the solid isn't enough to make the hole have
two surfaces. This is because by default, the Revolve operation has Merge Topology? set to Yes. This has
the effect of optimizing the topology of the resulting solid, which in this case means that the hole is always
created as just one surface.

 1.   Select the Revolve1 object from the Tree Outline.
 2.   Set Merge Topology? to No.
 3.   Click on Generate            to apply the changes to the solid.
 4.   Show the solid again by right-clicking on Solid in the Tree Outline, and choosing to Show Body.

You should now find that the hole in the solid has two faces as required.

The final step in the construction of this solid is to position the two breaks in the circle in the correct location.
As before, this could have been combined with the earlier steps, but it is clearer to separate it out for the
purposes of the tutorial. To position the breaks correctly, you will create a second sketch which is not used
to generate a solid directly but acts to constrain the breaks in the circle.

 1.   Hide the solid again by right-clicking on Solid in the Tree Outline, and choosing Hide Body.
 2.   With the XYPlane selected, create a New Sketch                                 .
 3.   Zoom into the circle from Sketch1 by clicking with the right mouse button somewhere near the circle
      and dragging a box over it whilst holding down the mouse button.
 4.   Use Line from the Draw toolbox of the Sketching tab to draw a vertical line with one endpoint at
      the center of the circle in Sketch1. You can make sure the line starts on the existing center point by
      ensuring that as you click the mouse button on it, a pink box appears around the center point. This
      indicates that you are choosing an existing point and not creating a new point. For the second point,
      move the cursor approximately vertically upwards and adjust it until a “V” appears next to the line. If
      you click whilst the “V” shape is present then the line is automatically constrained to be vertical. The
      length of the line does not matter, since you are only going to use it to define a symmetry axis.
 5.   Now draw two more lines, connecting each of the two vertices on the circle (where you split it) to the
      center of the circle. Again, you can make sure the lines start and finish on the existing points by ensuring
      that as you click the mouse button on the appropriate point, a pink box appears around the point.
 6.   The next step is to constrain the points so that they are symmetrically placed on each side of the
      vertical line. Select the Constraints toolbox of the Sketching tab, and click on Symmetry. Click first
      on the vertical line to pick the symmetry axis, and then click on the two straight lines to position them
      symmetrically.




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
214                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                         Creating the Second Solid

This moves the points in the Sketch2 to be symmetric about the vertical line. However, when you created
these points you defined them to be coincident points with the breaks in the circle in Sketch1, so this oper-
ation will also move the circle breaks in Sketch1 to be symmetric.

 1.   Select Angle from the Dimensions toolbox of the Sketching tab.
 2.   Set the angle between the two lines to be 74 degrees. If the wrong angle is displayed after you have
      selected the second line, then before you click to fix the label, right-click and choose Alternate Angle
      until the correct angle is displayed.




 1.   Click on Generate         to modify the solid.
 2.   Show the solid again by right-clicking on Solid in the Tree Outline, and choosing to Show Body.




Creating the Second Solid
Now what remains is to create the second solid, which fills in the gap on the outside of the reactor. If you
create another solid, the operation Add Material will add material to the first one rather than creating a
second solid as desired. The way to avoid this is to use Add Frozen instead of Add Material. The solid creation
operation, Extrude in this case, will add a new, separate solid. A frozen solid is not affected by most geometry
operations that follow, and will appear by default as slightly transparent.

To create the second solid, you first need to create a plane to extrude from.

 1.   Make sure that no faces are selected, and then create a New Plane                                         .
 2.   Set Type to From Face and check that Subtype is set to Outline Plane. If Subtype is already set to
      Tangent Plane, then you will not be able to change it: delete the new plane, make sure that no faces
      are selected (by clicking somewhere in the Model View window away from the geometry) and create
      a new plane instead.
 3.   For the Base Face, select the horizontal face at 3.5 cm above the bottom of the reactor - see the picture
      below - and then click on Apply in the Details View.
 4.   Click on Generate         to create the plane.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                          215
Tutorial 11: Airlift Reactor




 1.   Select Extrude           from the 3D Features toolbar.
 2.   Set Operation to Add Frozen.
 3.   Set Extent Type to To Faces. This will make the Extrude stop when it reaches the selected face(s).
 4.   Set the Target Face as the horizontal surface which is 3.5 cm below the top of the reactor
 5.   Click on Generate            to create the solid.




The Tree Outline should now show that you have display 2 Parts, 2 Bodies. In order to produce a single
mesh on the two bodies, they must be combined into one part.

 1.   From the Selection toolbar at the top of the window, turn on Select Bodies      . This means that you
      can only select Solid Bodies in the next operation, which helps to make the selection process easier.
 2.   In the Model View window, select one of the two Bodies by clicking on them with the left mouse
      button. Hold down the Ctrl key and then click on the other one in order to add to the original selection.
 3.   Right-click over the Model View window and select Form New Part.

The geometry is now complete. From the DesignModeler's main menu, select File > Save Project to save
the project and return to the Project Schematic. Now the Geometry cell appears in an up-to-date state.




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
216                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                              Setting up the Regions


Mesh Generation
Launching CFX-Mesh
On the Project Schematic, right-click Mesh cell in the Mesh system and select Edit to launch the Meshing
application.

If you have configured your global settings to ensure that CFX-Mesh is loaded automatically, the Meshing
application will load followed by CFX-Mesh.

      Note

      You can configure the settings under Tools > Options to open CFX-Mesh automatically
      whenever you choose to create a new mesh. For details on how to perform this one-time setup,
      see Setting CFX-Mesh as the Default Method for Meshing (p. 119).


Setting up the Regions
Create the 2D Regions:

 1.   Create a Composite 2D Region called Sparger on the top part of the small hole (the ring sparger).
 2.   Create a Composite 2D Region called Top on the very top face of the reactor (highest Y-coordinate).
 3.   Create a Composite 2D Region called Column on the column walls. You need to select five faces: the
      three parts of the outside wall (highest X-coordinate), the bottom face of the reactor (lowest Y-coordin-
      ate) and the bottom part of the small hole which forms the ring sparger.
 4.   Create a Composite 2D Region called Symmetry1 on the two faces which lie in the XYPlane.
 5.   Create a Composite 2D Region called Symmetry2 on the two faces which are directly opposite the
      faces used for Symmetry1.

Finally, create a Composite 2D Region on the internal face which will form the draft tube. In order to do
this, it is important to understand the difference between faces and 2D Regions when there are multiple
solids in the geometry, and how to use the selection rectangles. If you have not already done so, you are
advised to work through or at least read the meshing section of Tutorial 6: Butterfly Valve and the meshing
section of Tutorial 10: Heating Coil.

For the Composite 2D Region which comprises the draft tube, it is appropriate to include only one side of
the internal face. When you come to set up the Thin Surface boundary condition in CFX-Pre, the other side
of the face will then be automatically identified as the other side of the thin surface.

 1.   Right-click over Regions in the Tree View and select Insert > Composite 2D Region. Change its name
      to DraftTube.
 2.   Click on the cyan ball in the triad at the bottom right of the Graphics window to put the geometry
      into a good viewing position for the selection.
 3.   Place the cursor in the position shown in the picture below and click with the left mouse button.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                            217
Tutorial 11: Airlift Reactor




 4.   The selection rectangles will appear. The 2D Regions they correspond to are (from left to right): outside
      of the column, draft tube face (outside), draft tube face (inside), face from symmetry plane. Click on
      the second one from the left (draft tube face, outside), to select it.
 5.   Press Apply in the Details View. You should see that the text next to Location now reads 1 2D Region.

Setting up the Mesh
Set the Maximum Spacing:

 1.   Click on Default Body Spacing in the Tree View, which is contained in Mesh > Spacing.
 2.   In the Details View, change Maximum Spacing to 1.0 cm, and press Enter on the keyboard to set this
      value.

A maximum edge length of 1 cm will produce a coarse grid of about 4000-5000 nodes, suitable only for in-
structional and demonstrative uses. With the use of such a coarse mesh, the recirculation flow patterns in
the reactor cannot be resolved adequately and some difficulties in convergence may be expected. To create
a mesh that is appropriate for formal quantitative analysis of the airlift reactor in this tutorial, the maximum
edge length should be 0.5 cm or shorter. The resulting mesh will contain significantly more nodes.

Because the Default Face Spacing is set to use an Angular Resolution of 30 degrees, the mesh around the
sparger is automatically refined since the sparger has a high curvature.

Generating the Volume Mesh
Finally, you can generate the volume mesh by right-clicking Mesh in the Tree View and selecting Generate
Volume Mesh.

This completes the mesh generation. Now save the project by selecting File > Save from CFX-Mesh's main
menu and return to the Project Schematic.

You can exit from ANSYS Workbench by selecting File > Exit from the main menu.




                        Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
218                                                 of ANSYS, Inc. and its subsidiaries and affiliates.
Tutorial 12: Room with Air Conditioning




This tutorial creates the geometry and mesh for a room geometry, which can then be used in simulations
to determine the effectiveness of an air conditioning system. In the CFD simulation, the air is input through
a small vent in the roof of the room.

The following geometry and meshing features are illustrated:

 •    Imprint Surfaces, to add surfaces for boundary conditions
 •    Face Spacing, to refine the mesh on a particular face
 •    Inflation.

Geometry Creation
Creating the Project
 1.    Open ANSYS Workbench and add a standalone Mesh system on the Project Schematic. Save it as
       HVAC.wbpj. HVAC is an acronym for Heating, Ventilation and Air Conditioning. For details, see Creating
       the Project in ANSYS Workbench (p. 126).
 2.    Now add geometry to the project by using one of the following methods:
       •   If you want to skip the geometry creation part of this tutorial, use the supplied file HVAC.agdb
           to import geometry into the project. Once the geometry has been added, the Geometry cell appears
           in an up-to-date state. For details, see Can I Skip the Geometry Creation? (p. 120).

           Now proceed to the section Mesh Generation in this tutorial.
       •   If you want to create the geometry manually, continue with the following instructions.
 3.    On the Project Schematic, right-click Geometry cell in the Mesh system and select New geometry to
       open DesignModeler, specifying the units as meters.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                               219
Tutorial 12: Room with Air Conditioning


           Note

           If you have previously set the default unit by selecting either Always use project unit or
           Always use selected unit in DesignModeler, the units pop-up window will not appear.

           To access the units pop-up window upon subsequent openings of DesignModeler, open
           the Options dialog box by selecting Tools > Options from DesignModeler's main menu.
           In the Options dialog box, select DesignModeler > Units and set Units > Display Units
           Pop-up Window to Yes. For details, see Units in the DesignModeler Help.


           Note

           If you are using the Parasolid file supplied for this tutorial, see Tutorials Requiring Modifications
           When Importing CAD Files (p. 121).



Creating the Solid
The first step is to create the main solid, which is a simple box.

 1.   With the XYPlane selected, create a New Sketch                                .
 2.   Use Rectangle from the Draw toolbox of the Sketching tab to create a square which has one corner
      at the origin and another at X = 3.0 m, Y = 3.0 m.
 3.   Select Extrude        from the 3D Features toolbar.
 4.   Set Base Object to be the new sketch (Sketch1), and set Operation to Add Material.
 5.   Set Depth to be 2.5 m, and click on Generate                               to generate the solid.

Breaking the Faces to form the Boundary Conditions
The solid that you have just created has six rectangular faces. Some of these faces need breaking up, so that
the features such as windows, door and vents exist as separate faces of the solid. This can be done by using
Extrude with the Imprint Faces option.

Using this option requires sketches of the correct dimensions to be created first. However, when the Extrude
operation takes place, you cannot choose to have the Imprint Faces action only apply at a specified face; it
will apply at all faces between the sketch and the required face. For this reason, the sketches cannot be
created on the existing three planes since then they would always affect the faces of the solids which are
co-planar with these planes. This means that you need to start by creating a new plane.

 1.   With the XYPlane selected, click New Plane                            .
 2.   In the Details View, set Transform 1 to Offset Z, and set the Value of the offset to 1 m.
 3.   Click on    Generate to create the plane.
 4.   With the new plane (Plane4) selected, create a new sketch    . Use Rectangle from the Draw toolbox
      of the Sketching tab to create a rectangle which has one corner at X = 0.05 m, Y = 1.3 m and another
      at X = 0.15 m, Y = 1.7 m.
 5.   To do this first construct a rectangle in the approximate location.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
220                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                 Breaking the Faces to form the Boundary Conditions

 6.   In the Sketching toolbox under Dimensions choose Length/Distance.
 7.   Click on the side of the rectangle closest to the X-axis and then click on the X-axis itself. A label, L1,
      for this dimension will appear and can be placed anywhere on the grid (this does not affect the
      model in any way, it is purely for display purposes).
 8.   If you now look in the Details View at the bottom left of the screen, you will find a section headed
      Dimensions, which contains L1. Set this to 1.3 m.
 9.   Now click on the side of the rectangle closest to the Y-axis and then on the Y-axis itself. A label, L2,
      for this dimension will appear.
 10. In the Details View under Dimensions, there will now be a listing for L2. Set this to 0.05 m.

      Use this method to define the location of the other two sides of the rectangle.
 11. Select Extrude         from the 3D Features toolbar.
 12. Set Base Object to be the new sketch (Sketch2), and set Operation to Imprint Faces.
 13. Set Extent Type to To Next, and click on Generate                                   to break the top face.




Notice that in the figure above, the top face has been selected in order to show that it is in two parts.

These operations now need to be repeated to break the faces to form the windows and side vent.

 1.   With the ZXPlane selected, create a New Plane                               .
 2.   In the Details View, set Transform 1 to Offset Global Y, and set the Value of the offset to 1 m.
 3.   Click on    Generate to create the plane.
 4.   With the new plane (Plane5) selected, create a new sketch    . Use Rectangle from the Draw toolbox
      of the Sketching tab to create a rectangle which has one corner at X = 1.25 m, Z = 0.75 m and another
      at X = 1.75 m, Z = 1.75 m.
 5.   Use Rectangle from the Draw toolbox of the Sketching tab to create another rectangle, which has
      one corner at X = 2.05 m, Z = 0.15 m and another at X = 2.55 m, Z = 0.55 m.
 6.   Select Extrude        from the 3D Features toolbar.
 7.   Set Base Object to be the new sketch (Sketch3), and set Operation to Imprint Faces.
 8.   Set Direction to Reversed, Extent Type to be To Next, and click on                                             Generate to break a side
      face.




                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                          221
Tutorial 12: Room with Air Conditioning




 1.   With the YZPlane selected, create a New Plane                               .
 2.   In the Details View, set Transform 1 to Offset Z, and set the Value of the offset to 1 m.
 3.   Click on Generate           to create the plane.
 4.   With the new plane (Plane6) selected, create a New Sketch    . Use Rectangle from the Draw toolbox
      of the Sketching tab to create a rectangle which has one corner at Y = 1.25 m, Z = 0.75 m and another
      at Y = 1.75 m, Z = 1.75 m.
 5.   Select Extrude        from the 3D Features toolbar.
 6.   Set Base Object to be the new sketch (Sketch4), and set Operation to Imprint Faces.
 7.   Set Direction to Reversed and Extent Type to To Next, then click on Generate                                                   to break another
      side face.




Finally, you need to break one more face to make a face for the door. However, this time, the plane which
contains the sketch to be extruded must be outside the geometry. Otherwise, because the door reaches the
edge of the room, you will find that the rectangular (unbroken) face which shares an edge with the door
will be broken.

 1.   With the YZPlane selected, create a New Plane                               .
 2.   In the Details View, set Transform 1 to Offset Z, and set the Value of the offset to 4 m.
 3.   Click on Generate           to create the plane.
 4.   With the new plane (Plane7) selected, create a New Sketch    . Use Rectangle from the Draw toolbox
      of the Sketching tab to create a rectangle which has one corner at Y = 2.3 m, Z = 0.0 m and another
      at Y = 3.0 m, Z = 2.0 m.
 5.   Select Extrude        from the 3D Features toolbar.
 6.   Set Base Object to be the new sketch (Sketch5), and set Operation to Imprint Faces.

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
222                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                              Setting up the Regions

 7.   Set Direction to Reversed and Extent Type to To Next, and click on Generate                                                  to break the side
      face.




The geometry is now complete. From the DesignModeler's main menu, select File > Save Project to save
the project and return to the Project Schematic. Now the Geometry cell appears in an up-to-date state.

Mesh Generation
Launching CFX-Mesh
On the Project Schematic, right-click Mesh cell in the Mesh system and select Edit to launch the Meshing
application.

If you have configured your global settings to ensure that CFX-Mesh is loaded automatically, the Meshing
application will load followed by CFX-Mesh.

      Note

      You can configure the settings under Tools > Options to open CFX-Mesh automatically
      whenever you choose to create a new mesh. For details on how to perform this one-time setup,
      see Setting CFX-Mesh as the Default Method for Meshing (p. 119).


Setting up the Regions
Create the 2D Regions:

 1.   Create a Composite 2D Region called Inlet on the vent in the roof It is the small rectangular face
      contained in the plane with the highest Z-coordinate.
 2.   Create a Composite 2D Region called Roof on the remaining part of the roof with the highest Z-co-
      ordinate.
 3.   Create a Composite 2D Region called Window1 on the rectangular face which is cut out from the
      ZXPlane. This plane has two cutout rectangular faces, and you need the one which is taller and located
      at a higher Z-coordinate.
 4.   Create a Composite 2D Region called Window2 on the rectangular face which is cut out from the
      YZPlane.
 5.   Create a Composite 2D Region called VentOut on the smaller rectangular face which is cut out from
      the ZXPlane.
 6.   Create a Composite 2D Region called Floor on the rectangular face which is in the XYPlane.



                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                             223
Tutorial 12: Room with Air Conditioning

 7.   Create a Composite 2D Region called Door on the tall, thin rectangular face which is cut out from the
      face with the highest X-coordinate.

Setting up the Mesh
Set the Maximum Spacing:

 1.   Click on Default Body Spacing in the Tree View, which is contained in Mesh > Spacing.
 2.   In the Details View, change Maximum Spacing to 0.25 m, and press Enter on the keyboard to set this
      value.

This is a coarse length scale, suitable only for tutorial purposes. In order to better resolve the flow near the
inlet and outlet vents, Face Spacings will be applied to these regions to refine the mesh.

 1.   Right-click on Spacing and select Insert > Face Spacing.
 2.   In the Details View, set Option to Constant, and set the Constant Edge Length to 0.04 m.
 3.   Set the Radius of Influence to 0.0 m, and Expansion Factor to 1.3.
 4.   For Location, select Inlet from the Tree View.
 5.   Right-click on Spacing and select Insert > Face Spacing, to create another Face Spacing.
 6.   In the Details View, set Option to Constant, and set the Constant Edge Length to 0.1 m.
 7.   Set the Radius of Influence to 0.0 m, and Expansion Factor to 1.3.
 8.   For Location, select VentOut from the Tree View.

Setting up Inflation
It is a good idea to put inflation on the walls.

 1.   Click on Inflation in the Tree View. In the Details View, set Number of Inflated Layers to 5.
 2.   Set Expansion Factor to 1.2. Leave the rest of the parameters as their default values.
 3.   In the Tree View, right-click on Inflation and select Insert > Inflated Boundary.
 4.   For Location, select all of the Composite 2D Regions in the Tree View (including the Default 2D Region)
      except for Inlet and VentOut. The Details View should show 6 Composites after you have made the
      selection.
 5.   Set Maximum Thickness to 0.25 m.

Generating the Volume Mesh
Finally, you can generate the volume mesh by right-clicking Mesh in the Tree View and selecting Generate
Volume Mesh.

This completes the mesh generation. Now save the project by selecting File > Save from CFX-Mesh's main
menu and return to the Project Schematic.

You can exit from ANSYS Workbench by selecting File > Exit from the main menu.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
224                                               of ANSYS, Inc. and its subsidiaries and affiliates.
Tutorial 13: Can Combustor




This tutorial creates a mesh for a can combustor, which can be found in gas turbine engines. The geometry
is complex and consists of 5 separate solid bodies. It will be imported as a complete geometry from a
Parasolid file. The diagram above right shows the geometry schematically with part of the outer wall cut
away. The following geometry and meshing features are illustrated:

 •    Parasolid import
 •    Inflation.

This tutorial requires you to have a copy of the Parasolid file Combustor.x_t. If you do not have this file,
download it from http://www.ansys.com/dm_how_tos/cm_combustor.exe (you will need to execute the
downloaded file to extract the required Parasolid file).

Geometry Import
Creating the Project
 1.    Open ANSYS Workbench and add a standalone Mesh system on the Project Schematic. Save it as
       Combustor.wbpj. For details, see Creating the Project in ANSYS Workbench (p. 126).
 2.    Now add geometry to the project by using one of the following methods:
       •   If you want to skip the geometry creation part of this tutorial, use the supplied file Combustor.ag-
           db to import geometry into the project. Once the geometry has been added, the Geometry cell
           appears in an up-to-date state. For details, see Can I Skip the Geometry Creation? (p. 120).

           Now proceed to the section Mesh Generation in this tutorial.

                         Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                     of ANSYS, Inc. and its subsidiaries and affiliates.                               225
Tutorial 13: Can Combustor

      •   If you want to create the geometry manually, continue with the following instructions.
 3.   On the Project Schematic, right-click Geometry cell in the Mesh system and select New geometry to
      open DesignModeler, specifying the units as centimeters.

           Note

           If you have previously set the default unit by selecting either Always use project unit or
           Always use selected unit in DesignModeler, the units pop-up window will not appear.

           To access the units pop-up window upon subsequent openings of DesignModeler, open
           the Options dialog box by selecting Tools > Options from DesignModeler's main menu.
           In the Options dialog box, select DesignModeler > Units and set Units > Display Units
           Pop-up Window to Yes. For details, see Units in the DesignModeler Help.


           Note

           If you are using the Parasolid file supplied for this tutorial, see Tutorials Requiring Modifications
           When Importing CAD Files (p. 121).



Importing the Geometry
The geometry is imported complete, from a Parasolid file.

 1.   Select File > Import External Geometry File... from the main menu.
 2.   In the file browser which opens, locate and open the file Combustor.x_t.
 3.   Click on Generate          to import the combustor.

The Tree Outline should now show that you have 5 Parts, 5 Bodies. In order to produce a single mesh that
contains all of the bodies, rather than one mesh per body, the parts must be combined.

 1.   From the Selection toolbar at the top of the window, turn on Selection Filter: Bodies     . This means
      that you can only select Solid Bodies in the next operation, which helps to make the selection process
      easier.
 2.   In the Model View window, select all 5 bodies as follows:
      •   Click on Select Mode              and select Box Select from the drop-down menu.
      •   Whilst holding down the left mouse button, drag a box across the whole geometry to select all 5
          bodies. Once you have released the mouse button, the status bar found along the bottom of the
          ANSYS Workbench window, should change to show that you have selected 5 Bodies.
 3.   Right-click over the Graphics window and select Form New Part.

The Tree Outline should now show that you have 1 Part, 5 Bodies. The geometry does not need any further
modifications.

The geometry is now complete. From the DesignModeler's main menu, select File > Save Project to save
the project and return to the Project Schematic. Now the Geometry cell appears in an up-to-date state.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
226                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                               Setting up the Regions


Mesh Generation
Launching CFX-Mesh
On the Project Schematic, right-click Mesh cell in the Mesh system and select Edit to launch the Meshing
application.

If you have configured your global settings to ensure that CFX-Mesh is loaded automatically, the Meshing
application will load followed by CFX-Mesh.

      Note

      You can configure the settings under Tools > Options to open CFX-Mesh automatically
      whenever you choose to create a new mesh. For details on how to perform this one-time setup,
      see Setting CFX-Mesh as the Default Method for Meshing (p. 119).


Setting up the Regions
Create the 2D Regions:

 1.   Create a Composite 2D Region for the fuel inlet called fuelin on the six tiny faces on the cone near
      the bottom of the combustor. The easiest way to select them is as follows:
      a.   Click over the axes in the bottom right corner of the Graphics window in the position shown in
           the picture below. As you move the cursor into this position, the black “-Z”-axis will appear (it is
           not shown by default). This will put the geometry into a good position for picking the required
           faces.




      b.   Zoom into the geometry and select the six small faces which are shown in bright green in the
           picture below (note that the colors in your geometry may differ from the picture below).




 2.   Create a Composite 2D Region for the air inlet called airin on the eight faces at the very bottom of
      the geometry having the lowest Z-coordinate, as shown below.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                            227
Tutorial 13: Can Combustor

 3.   Create a Composite 2D Region for the secondary air inlet called secairin on the six small circular faces
      on the main body of the combustor. These introduce extra air to aid combustion.




 4.   Create a Composite 2D Region called out on the rectangular face with the highest Z-coordinate.
 5.   Right-click the Composite 2D Region called airin in the Tree View and select Hide.

      Look into the combustor inlet. You will see eight curved vanes surrounding the fuel inlet. Rotate the
      view slightly and note that every other vane passage is blocked by faces that are part of the Default
      2D Region. You will remove these faces from the Default 2D Region by defining a composite region
      for those faces.
 6.   Create a Composite 2D Region called internal faces. Set the location to the 8 primitive 2D regions
      that form both sides of the 4 faces that block the vane passages. You will need the selection rectangles
      to do this. For details, see Selection Tools (p. 12).




Setting up the Mesh
This is a complex geometry which will be used to run a simulation with complex physics. In order to keep
the computational time down for the purposes of the tutorial, a very coarse mesh will be used. If you wanted
to get accurate results on this geometry, a much finer mesh and a much larger solution time would be re-
quired.

Set the Maximum Spacing:

 1.   Click on Default Body Spacing in the Tree View, which is contained in Mesh > Spacing.
 2.   In the Details View, change Maximum Spacing to 1.6 cm, and press Enter on the keyboard to set this
      value.
 3.   Click on Default Face Spacing in the Tree View, which is contained in Mesh > Spacing.
 4.   In the Details View, set Option to Volume Spacing. This stops the surface mesh from being refined
      where the faces are highly-curved, which would add too many elements for this coarse tutorial mesh.
      The Volume Spacing setting simply uses the Default Body Spacing for the surface mesh spacing.


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
228                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                     Generating the Volume Mesh

Setting up Inflation
It is a good idea to put inflation on the walls.

 1.   Click on Inflation in the Tree View. In the Details View, set Number of Inflated Layers to 5.
 2.   Set Expansion Factor to 1.3. Leave the rest of the parameters at their default values.
 3.   In the Tree View, right-click on Inflation and select Insert > Inflated Boundary.
 4.   For Location, select Default 2D Region from the Tree View.
 5.   Set Maximum Thickness to 1.6 cm.

Generating the Volume Mesh
Finally, you can generate the volume mesh by right-clicking Mesh in the Tree View and selecting Generate
Volume Mesh.

This completes the mesh generation. Note that you may get a warning about poor quality volume elements
being present in the mesh. This is a result of setting up such a coarse mesh. If you wanted to get accurate
results in the CFD simulation, you would need to modify the mesh settings and regenerate the volume mesh
in order to improve the quality of the elements.

Now save the project by selecting File > Save from CFX-Mesh's main menu and return to the Project
Schematic.

You can exit from ANSYS Workbench by selecting File > Exit from the main menu.




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                      229
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
230                               of ANSYS, Inc. and its subsidiaries and affiliates.
Tutorial 14: CAD Cleanup and Meshing




This tutorial shows how to use CFX-Mesh with poor CAD. The geometry supplied is of very poor quality,
with bad faces and lots of short edges; however, these features of CFX-Mesh enable you to clean it up to
produce a good-quality mesh:

 •    CAD Check
 •    Virtual Faces
 •    Virtual Edges (both manual and automatic)
 •    Short Edge Removal.

This tutorial requires you to have a copy of the DesignModeler file CADMeshing.agdb. If you do not have
this file, download it from http://www.ansys.com/dm_how_tos/cm_cadmeshing.exe to your working directory
for this tutorial (you will need to execute the downloaded file to extract the required DesignModeler file).

Mesh Generation
Creating the Project
 1.    Open ANSYS Workbench and add a standalone Mesh system on the Project Schematic. Save it as
       CADMeshing.wbpj. For details, see Creating the Project in ANSYS Workbench (p. 126).
 2.    Now use the supplied file CADMeshing.agdb and import the geometry into the project. For details,
       see Importing CAD files for CFX-Mesh Tutorials (p. 120).
 3.    On the Project Schematic, right-click Mesh cell in the Mesh system and select Edit to launch the
       Meshing application.

       If you have configured your global settings to ensure that CFX-Mesh is loaded automatically, the
       Meshing application will load followed by CFX-Mesh.

            Note

            You can configure the settings under Tools > Options to open CFX-Mesh automatically
            whenever you choose to create a new mesh. For details, see Setting CFX-Mesh as the Default
            Method for Meshing (p. 119) for instructions on how to perform this one-time setup.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               231
Tutorial 14: CAD Cleanup and Meshing

Examining the Geometry
The first step is to inspect the geometry and see what features it has that will lead to a poor mesh.




The picture above shows the geometry, rotated to a suitable viewing position. The green highlights show
four very narrow faces: each of these will result in a very fine mesh as the narrow width is resolved. The blue
highlights show three faces that have very sharp points (including one which is also very narrow): these
faces will give a surface mesh with poor angles and may even make the meshing operations fail, depending
on factors such as the mesh length scale in the region of the point. In addition, many of the edges on these
faces are very short (not shown): these will cause regions of very fine mesh as the mesher is constrained to
put at least three vertices on every edge. Some of the edges are so short that you may find that the mesher
cannot generate a mesh with any reasonable length scale.

 1.   Zoom in to various parts of the geometry to see the various features highlighted in the picture.
 2.   Right-click on Geometry in the Tree View, and select Verify Geometry.

This runs the CAD-checking utility to have CFX-Mesh show certain geometry features that may cause the
mesher problems. Once the utility has finished, you should see four warnings or information messages under
Errors in the Messages window. These warn about different types of problematic features.

 1.   Click on Warning in the Messages window. This contains the text CAD model contains faces with
      small angles. You should be able to see that the face which the warning refers to is highlighted in
      the Graphics window. This is one of the faces which has already been identified as having a very sharp
      point. Zoom into this region of the geometry to see the face more clearly.
 2.   Click on the Information messages. One of these messages contains the text 6 potential sliver edge(s)
      have been found. Six very short edges are highlighted in green in the Graphics window, but they are
      so small that they are hard to spot. Zoom in to the region of the geometry highlighted in the picture
      below to find one of the short edges.




      The location of all six small edges are marked on the picture below. You can zoom in to each one of
      them to see how small they are. Note that some of these edges are so short that you will have to
      zoom in a long way to be able to see them.



                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
232                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                      Adding Virtual Faces and Virtual Edges




 3.   Another of the messages contains the text 38 potential sliver face(s) have been found.. This refers
      to two very narrow faces which have already been identified as a problem.
 4.   Finally, click on the last message in the list. This is just a summary of the checks. You will always get
      this message, even if no problems are found.

Next, you will attempt to create a surface mesh to see how the highlighted problems affect it.

 1.   Expand the Preview item in the Tree View, right-click over Default Preview Group, and select Generate
      Surface Meshes.

      A mesh is produced with numerous warning messages about poor quality triangles (triangles that are
      far from equilateral) and small internal angles. The mesh is of a poor quality and very patchy due to
      the very narrow faces and short edges. Although it might be tempting to try to create the mesh again
      with a smaller length scale to resolve the short edges better, in practice the very short edges mean
      that you would have to make such a large mesh that this would be impractical, and the narrow faces
      with small angles would still cause problems.
 2.   Click on the plus sign next to Default Preview Group in the Tree View, to expand it. Click on Mesh
      Statistics and check the Details View to see the mesh statistics. You should find that your surface
      mesh has around 8000-9000 triangles.

Adding Virtual Faces and Virtual Edges
The first steps in improving the geometry to allow it to mesh are to remove some of the narrow and pointed
faces and the very shortest edges. CFX-Mesh includes the ability to create a Virtual Face, which combines
several faces to make a single face and also (by default) combines any short edges that satisfy its criteria
into Virtual Edges. The mesher needs to mesh only the Virtual Faces and Virtual Edges and does not need
to separately mesh the constituent faces or any edges that are not on the border of the virtual face.

In order to illustrate the manual creation of Virtual Edges, you first turn off the automatic edge-merging fa-
cility:

 1.   From the menu bar select Tools > Options.
 2.   Expand the options tree and select Meshing > Meshing.
 3.   Under the sub-section Virtual Topology, set Merge Edges Bounding New Virtual Faces to No.
 4.   Click OK to apply the change.

Now zoom into the region of the geometry shown in the picture below. Note how the surface mesh has
been very distorted by the presence of the very narrow face (shown in brown in the picture).




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                   233
Tutorial 14: CAD Cleanup and Meshing




You will now merge the narrow face with its neighbor to eliminate it completely.

 1.   In the Tree View, right-click on Virtual Topology and select Insert > Virtual Face.
 2.   For Location, hold down the Ctrl key and click to pick the two faces highlighted in the picture below.




 3.   Click Apply in the Details View to confirm the selection.

Now, re-generate the surface mesh to see the effect of this.

 1.   Right-click over Default Preview Group in the Tree View, and select Generate Surface Meshes.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
234                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                     Adding Virtual Faces and Virtual Edges




The narrow face has now disappeared from the mesh and most of the small and distorted triangles that it
caused have also gone. However, there is still a short edge which used to form the edge of the narrow face,
and as a result there are still two poor triangles with very small angles. You may need to zoom in to see
these triangles.

Now create a Virtual Edge to remove this edge and the poor triangles.

 1.   In the Tree View, right-click on Virtual Topology and select Insert > Virtual Edge.
 2.   For Location, Ctrl-click to pick the two edges highlighted in the picture below.




 3.   Click Apply in the Details View to confirm the selection.

Now re-generate the surface mesh to see the effect of this.

 1.   Right-click over Default Preview Group in the Tree View, and select Generate Surface Meshes.




The distorted triangles have completely disappeared as the mesher no longer needs to resolve the short
edge. You will need to zoom out to see the triangles properly as they are so much larger than before.

Now that you have seen the effect of short edges and how to remove them manually, you will now see how
to remove them automatically. First turn on automatic edge merging again.


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                   235
Tutorial 14: CAD Cleanup and Meshing

 1.   From the menu bar, select Tools > Options.
 2.   Expand the options tree and select Meshing > Meshing.
 3.   Under the sub-section Virtual Topology, set Merge Edges Bounding New Virtual Faces to Yes.
 4.   Click on OK to apply the change.

You will need to delete both the Virtual Edge and the Virtual Face to see the effect of this setting because
it applies only when new Virtual Faces are created.

 1.   Right-click over Virtual Edge 1 in the Tree View and select Delete.
 2.   Right-click over Virtual Face 1 in the Tree View and select Delete.

      If you want, you can verify at this point that the surface mesh is poor again by regenerating it.

Now re-create the Virtual Face you made previously.

 1.   In the Tree View, right-click on Virtual Topology and select Insert > Virtual Face.
 2.   For Location, pick the two faces highlighted in the picture below.




 3.   Press Apply in the Details View to confirm the selection.

If you now inspect the Tree View, you should be able to see a new entry immediately below Virtual Face
1, that is, Virtual Edge 1. If you click on it to highlight it in the Graphics window, you can see that it corres-
ponds to the same Virtual Edge as you previously created manually. Now that automatic edge merging is
turned on, CFX-Mesh behaves intelligently and creates all the related Virtual Edges that it can each time it
creates a Virtual Face. Note that CFX-Mesh will not automatically merge edges that meet at an angle greater
than a certain tolerance (the default is 5 degrees) so that corners will be preserved. This tolerance can be
changed using Tools > Options and setting Meshing > CFX-Mesh Options > Virtual Topology > Automatic
Edge Merging Tolerance (Degrees).

You can now create several more Virtual Faces to remove the remaining narrow faces and corresponding
short edges.

 1.   In the Tree View, right-click on Virtual Topology and select Insert > Virtual Face.
 2.   For Location, start by picking the four narrow faces highlighted in the picture below (do not press
      Apply yet). These faces are most easily selected by using Box Select (drag a box with the left mouse
      button over each face in turn, holding down the Ctrl key for the second and subsequent faces).




                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
236                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                     Adding Virtual Faces and Virtual Edges




 3.   Now add a further fourteen faces to the selection, shown in the picture below.




 4.   Press Apply in the Details View to confirm the selection.
 5.   In the Tree View, right-click on Virtual Topology and select Insert > Virtual Face.
 6.   For Location, pick the narrow face highlighted in the picture below, using Box Select.




      Then add three more faces as shown in the next picture:




 7.   Press Apply in the Details View to confirm the selection.

Note that various Virtual Edges have been automatically created.

                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                   237
Tutorial 14: CAD Cleanup and Meshing

So far, all of the Virtual Faces you have created have merged faces that meet at a tangent; that is, the resulting
Virtual Face is smooth and contains no sharp corners. In this situation, there is no loss of accuracy resulting
from the creation of the Virtual Face. However, it is possible to create Virtual Faces that do contain sharp
corners: in the Virtual Face created below, two of the faces meet at right angles. Where this occurs, the
mesher effectively rounds off the corner and so the meshed geometry is only an approximation to the ori-
ginal geometry. You should merge faces into a non-smooth Virtual Face only where there is a small feature
present in the geometry that does not need to be included in the CFD simulation.

 1.   In the Tree View, right-click on Virtual Topology and select Insert > Virtual Face.
 2.   For Location, pick the narrow face highlighted in the picture below, using Box Select.




      Then add a second face as shown in the next picture:




 3.   Press Apply in the Details View to confirm the selection.
 4.   Right-click over Default Preview Group again and select Generate Surface Meshes. Zoom into the
      region of the mesh highlighted below.




Notice how the mesh in the region of the narrow face is not flat; the corner has been rounded off.

There are still two short edges where the ends of the narrow face used to be, which results in large numbers
of small mesh elements as the mesher resolves the short edges. These short edges could not be automatically
merged with another edge to form a Virtual Edge. The edge at the bottom (in the area highlighted in the
picture above) makes an angle of greater than 5 degrees with its neighbor so the corresponding Virtual


                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
238                                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                       Removing the Remaining Short Edges

Edge could have been created if this tolerance had been increased. However, the edge at the top cannot
be created as a Virtual Edge for reasons discussed in the next section.

Apart from these two small patches of fine and distorted mesh, the surface mesh is now much more uniform
and of a much higher quality due to the creation of the Virtual Faces and Edges.

Removing the Remaining Short Edges
The two remaining patches of fine mesh are due to the two remaining short edge. However, it is the top
patch of fine mesh (highest y-value) that causes the problem. Its topology is shown in the picture below:
edges are shown in blue and vertices in red.




You need to remove this short edge to eliminate the fine mesh that it forces the mesher to create. However,
you cannot do so by creating another Virtual Edge. A Virtual Edge can be created only from edges that share
the same faces, and there is no other edge that shares the same faces as this remaining short edge, as the
diagram above shows.

      Note

      It would have been easy to choose a different set of faces to be used in the construction of the
      last Virtual Face that would have avoided this problem; this tutorial has deliberately set up this
      problem edge in order to illustrate how it can be removed. Making a different Virtual Face may
      not always be possible in complex CAD where features may need to be preserved.

CFX-Mesh allows you to remove short edges using a second method: Short Edge Removal. Using this mech-
anism, short edges are removed by collapsing them to a single point. As a result (and unlike Virtual Edges),
this method cannot be used if the local mesh length scale is smaller than the length of the edges to be re-
moved, as it leads to the mesh becoming distorted (see the CFX-Mesh Help for more details). You need to
determine how long this edge is and compare it to the mesh length scale before using Short Edge Removal
to remove it.

Also, when using Short Edge Removal, you simply specify a length scale, and all edges in the geometry
which are shorter than this length scale are removed. It is therefore a good idea to make sure that before
you use it, you know exactly which edges will be removed.

Both of these things can be checked by using CAD Check again.

 1.   Click on the plus sign next to Geometry in the Tree View to open it up. Click on Verify Options.
 2.   In the Details View, you can set the parameters to be used by CAD Check to identify poor geometry.
      In this case, you are interested only in short edges. Set Short Edge Limit to 0.015 m to make CAD
      Check identify all of the edges shorter than this length.
 3.   Right-click over Geometry and select Verify Geometry to perform the CAD Check operation.
 4.   Once the CAD Check operation has finished, check the error messages in the Messages window.



                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                239
Tutorial 14: CAD Cleanup and Meshing

Note that the total number of warnings has decreased from when you ran CAD Check on the original geometry
(before creating Virtual Edges and Virtual Faces). There are no longer any warnings about CAD faces with
small angles or potential sliver faces, since all of these faces have been removed by the creation of Virtual
Faces. There is just one warning about short edges (plus the second warning which gives a summary of the
checks).

 1.   Click on the warning message about the short edges, and verify that the highlighted edges correspond
      to only the two edges which you have already identified as needing removal. This means that you can
      ask to remove all edges of less than 0.015 m from the geometry, knowing that it only affects the required
      edges. Since you are going to use a mesh length scale which is significantly larger than 0.015 m, the
      short edge can be safely removed using Short Edge Removal.
 2.   Under Geometry in the Tree View, click on Fix Options. In the Details View, set Remove Short Edges
      to Yes, and set Short Edge Tolerance [m] to 0.015 m.
 3.   Now regenerate the surface mesh by right-clicking over Default Preview Group and select Generate
      Surface Meshes. Once the meshing operation has finished, you should be able to see that the remaining
      patches of fine mesh have now disappeared.
 4.   Click on Mesh Statistics under Default Preview Group in the Tree View, and check the Details View
      to see the mesh statistics. You should find that your surface mesh has around 2000-2500 triangles.
      Removing the narrow faces and short edges has allowed you to create a good-quality mesh with far
      fewer triangles than previously.

Setting up the Finer Mesh
Set a finer Maximum Spacing (note that this should always remain above the 0.015 m that was set as the
limit for Short Edge Removal):

 1.   Click on Default Body Spacing in the Tree View, which is contained in Mesh > Spacing.
 2.   In the Details View, change Maximum Spacing to 0.05 m, and press Enter on the keyboard to set this
      value.
 3.   Click on Default Face Spacing in the Tree View, which is contained in Mesh > Spacing.
 4.   In the Details View, change Angular Resolution to 18 degrees.

Setting up Inflation
You will now add inflation onto the walls. First create a Composite 2D Region to allow the appropriate faces
to be selected more easily.

 1.   Create a Composite 2D Region called NoInflation on the faces highlighted in the picture below.




 2.   Click on Inflation in the Tree View. In the Details View, set Number of Inflated Layers to 5.
 3.   Set Expansion Factor to 1.3. Leave the rest of the parameters as their default values.


                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
240                                              of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                    Generating the Volume Mesh

 4.   In the Tree View, right-click on Inflation and select Insert > Inflated Boundary.
 5.   For Location, select Default 2D Region from the Tree View.
 6.   Set Maximum Thickness to 0.05 m.
 7.   Now regenerate the surface mesh to inspect the refined and inflated mesh. Right-click over Default
      Preview Group and select Generate Surface Meshes.

Generating the Volume Mesh
Finally, you can generate the volume mesh by right-clicking Mesh in the Tree View and selecting Generate
Volume Mesh.

This completes the mesh generation. Now save the project by selecting File > Save from CFX-Mesh's main
menu and return to the Project Schematic.

You can exit from ANSYS Workbench by selecting File > Exit from the main menu.




                     Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                 of ANSYS, Inc. and its subsidiaries and affiliates.                                      241
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
242                               of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                double-precision - storing the mesh and region in-
Index                                                                           formation , 101
                                                                                for point selection, 13
                                                                                mapping - between surface mesh and solid geometry
Symbols                                                                         , 37
2D
                                                                             creating
  generating an extruded 2D mesh, 87
                                                                                Composite 2D regions and Default 2D regions , 58
  selecting 2D regions and faces - See also regions, 57
                                                                                mesh - an overview, 1
3D
  using the advancing front and inflation for volume
  meshing, 87                                                                D
                                                                             Default 2D region
                                                                                description - See also regions, 58
A                                                                            defining
adding
                                                                                regions, 1
  guidelines for creating and adding - virtual face and
                                                                             degenerate geometry - See also geometry, 40
  virtual edge - See also checking; meshing; virtual to-
                                                                             Details View, 21
  pology, 47
                                                                             Display Units dialog
angular resolution
                                                                                accessing in DesignModeler, 128
  specifying the curvature for an edge or face in terms
                                                                             displaying - See also viewing, 22
  of an angle, 67
aspect ratio
  effects due to 2D extrusion options, 91                                    E
  effects due to inflation, 82                                               elements
                                                                                aspect ratio - controlling the size and distribution of
                                                                                elements , 75
B                                                                               aspect ratio and distribution for extruded mesh, 91
box select
                                                                                checking the mesh quality, 80
  specifying a location, 14
                                                                                distortion of interstitial elements, 80
                                                                             error messages
C                                                                               checking the undesirable geometry - See also geo-
CFX-Mesh                                                                        metry; meshing; troubleshooting, 41
   GUI - See also examples; features; tutorials, 5                           examples
   meshing features, 63                                                         creating a free floating thin surface, 36
   tutorials , 122                                                              creating a virtual edge, 51
checking                                                                        creating a virtual face, 48
   error messages - See also geometry; meshing;                                 creating an attached thin surface, 36
   troubleshooting, 41                                                          poorly-parameterized surfaces - circular parametric
   faces with high sliver factor, 43                                            surface, 39
   mesh quality, 80                                                             poorly-parameterized surfaces - cusps, 40
   parameterization face, 43                                                    poorly-parameterized surfaces - degenerate surfaces,
   parameterization quality, 43                                                 40
   sliver edge - locating short edges in the geometry,                          poorly-parameterized surfaces - distorting the
   42                                                                           square, 39
clearing                                                                        poorly-parameterized surfaces - uneven parametric
   removing the surface mesh from application's                                 lines, 39
   memory , 97                                                                  removing the short edges, 53
   user-defined settings using the File menu command,                        exporting
   6                                                                            mesh settings as a CCL file, 6
Composite 2D regions
   description - See also regions, 58                                        F
computation
                                                                             features
   of sliver factor, 43
                                                                                2D region groups, 122
coordinates

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                               243
Index

    advancing front surface mesher, 87                                          volume mesh, 3, 101
    advancing front volume mesher, 88                                         geometry
    advancing front with inflation 3D, 88                                       controlling the appearance, 46
    CAD check, 122                                                              creating 2D regions for thin surfaces , 37
    checking the undesirable geometry, 41                                       degenerate entities, 40
    curvature-sensitive meshing, 122                                            for CFX-Mesh , 1
    delaunay surface mesher, 87                                                 meshing the special topologies - faces of an inflated
    description of mesh controls, 68                                            boundary, 34
    extruded 2D meshing, 90, 122                                                meshing the special topologies - faces of solid bodies,
    face spacing, 122                                                           32
    geometry update, 122                                                        meshing the special topologies - solid bodies, 27
    global mesh scaling, 86                                                     modeling consideration for thin surfaces, 35
    inflation, 75, 122                                                          modeling guidelines to improve poorly-parameter-
    list of meshing functions to control mesh generation,                       ized surfaces, 37
    63                                                                          modifying and updating, 25
    listed - See also examples; tutorials, 122                                  requirements for meshing , 26
    meshing controls, 122                                                       sliver edge checking, 44
    Named Selections, 59                                                        suppressing items in the Tree View, 19
    parallel volume meshing, 88, 122                                            Verify Geometry - setting the tolerances and limits
    periodicity, 122                                                            for the geometry checking - See also checking, 43
    periodicity - generating the mesh for periodic                              verifying and updating the geometry using the
    boundary conditions, 72                                                     toolbar , 15
    preview groups, 122                                                       graphics window, 22
    proximity, 122                                                            GUI - See also toolbars; viewing, 5
    proximity - controlling the mesh refinement around                        guidelines
    edges and faces, 84                                                         selection of 2D regions and faces, 57
    short edge removal, 122                                                     specifying the mesh length scale, 115
    spacing - specifying the mesh length scale, 63                              to create virtual topology, 47
    specifying the meshing strategy, 87
    stretch, 122                                                              H
    stretch - expanding or contracting the mesh element,                      help
    83                                                                           context sensitive, 5
    surface meshing, 87                                                          GUI - an overview , 5
    virtual faces and edges, 122                                                 meshing features, 63
file formats                                                                  hiding
    .gtm, 101                                                                    objects, 20
    .mshdb, 101                                                               highlight
first layer thickness                                                            See also checking; tree view; viewing, 17
    inflation - specifying the height for the first prism
    layer, 77
fixing - See also geometry, 44
                                                                              I
flood select                                                                  inflation, 75
    specifying a location, 14                                                    consideration for the faces with thin gaps , 82
                                                                                 consideration for the inside walls of cylindrical pipes,
                                                                                 82
G                                                                                controlling the advanced mesh quality, 80
generate                                                                         creating an inflated boundary, 81
  surface mesh, 16                                                               list of available parameters to control inflation, 76
  surface meshes, 97                                                          interrupt
  volume mesh, 16                                                                description - See also toolbars, 16
generating
  preview group - selecting 2D regions, 97
  surface mesh, 2

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
244                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                    Index

L                                                                              inflation - first layer thickness, 77
length unit                                                                    inflation - total thickness , 79
   setting in DesignModeler, 128                                               parallel volume meshing - PVM distributed , 88
limits - See also tolerance, 43                                                parallel volume meshing - PVM local , 88
line control                                                                   setting the CFX-Mesh preferences for ANSYS Work-
   description, 70                                                             bench session, 103
location                                                                       setting the preferences using main menu, 7
   selecting multiple items, 12                                                settings to enable Named Selections, 59
   selection, 12                                                               Verify Geometry - setting the tolerances and limits
                                                                               for the geometry checking , 43
                                                                               y+, 77
M                                                                            overview, 1, 22
menus - description of menu items, 6                                           Details View, 21
merging                                                                        GUI, 5
  See also virtual topology, 48                                                Tree View, 17
mesh                                                                           tutorials, 119
  adaption - using ANSYS CFX-Pre , 3
  attributes - setting the length scale, 2
  generating volume mesh, 101                                                P
  generator - 3D meshing mode , 1                                            parameterization face checking - See also checking, 43
  generator - extrude 2D meshing mode, 1                                     periodic pair
  guidelines for mesh length scale, 115                                         extruded, 75
  mesh edge length - viewing the element size range                             specifying the parameters to define a periodic pair,
  , 14                                                                          73
  problems with degenerate geometry , 40                                     periodicity
  selecting and previewing mesh faces , 97                                      description, 72
  types of controls available for mesh refinement , 68                       picking
meshing                                                                         geometry elements using the Tools menu, 7
  advancing front surface mesher, 87                                         plug-in mode
  an overview of the meshing process, 1                                         See also reader mode, 25
  delaunay surface mesher, 87                                                point
  extruded 2D, 90                                                               selecting, 13
  extruded 2D meshing , 94                                                   point control
  generator, 1                                                                  description, 69
  halting the meshing process, 16                                            preview
  list of features, 63                                                          display mode, 98
  mesh generation process for a periodic pair , 74                              face color, 98
  parallel volume meshing, 88                                                   inflated layers, 98
  skipping the geometry creation - using tutorials,119                          shine, 98
  strategy - controlling the global meshing behavior ,                          transparency, 98
  87                                                                         preview group
  toolbar, 16                                                                   default preview group , 97
  tutorials - See also examples , 122                                           mesh statistics, 97


N                                                                            R
Named Selections                                                             reader mode
  description and guidelines, 59                                                See also plug-in mode , 25
                                                                             regions
                                                                                defining the location, 1
O                                                                               description - See also requirements, 57
options                                                                         picking 2D regions and faces - using the selection
  auto backup options, 103                                                      rectangles, 57
  extruded 2D, 91                                                            relative error

                      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                  of ANSYS, Inc. and its subsidiaries and affiliates.                                245
Index

   specifying the curvature for an edge or face in terms                         length scale, 2
   of deviation, 67                                                           shaded display - See also viewing, 8
removing - See also clearing; geometry; virtual topology,                     short edges - See also sliver, 44
44                                                                            sliver
requirements                                                                     description of sliver factor - See also checking, 43
   conditions on geometry for meshing needs, 27                                  edge - checking the short edges, 42
   creating an inflated boundary, 81                                             face - checking the faces with high sliver factor, 43
   creating the geometry for meshing needs, 27                                   removing the short edges - methods, 53
   modeling guidelines to improve poorly-parameter-                           spacing, 63
   ized surfaces, 37                                                             body - specifying the background length scale for
   periodic pair - extruded 2D meshing , 94                                      volume, 63
   specifying the location and topology of faces in the                          edge - specifying the mesh length scale on an edge,
   periodic pair, 74                                                             65
restrictions                                                                     face - specifying the mesh length scale on a face, 64
   creating a new body spacing, 63                                               point - specifying the spacing attribute for volumetric
   meshing a thin surface topology, 35                                           controls, 68
   Named Selections and Composite 2D Regions cre-                                relative error, 67
   ated in DesignModeler, 59                                                     specifying the angular resolution, 67
reverting                                                                     status symbols
   mesh settings to the last saved database - See also                           status of items in the Tree View, 17
   clearing, 6                                                                suppressing
rotation modes, 9                                                                effects - viewing the bodies and parts in the Tree
   free, 11                                                                      View , 45
   pitch, 11                                                                     objects - See also hiding, 19
   roll, 11                                                                   surface mesh - See also meshing, 40
   toolbar, 9
   yaw, 11                                                                    T
ruler - See also toolbars; viewing, 15                                        tolerance
                                                                                 checking the sliver edge, 42
S                                                                                consideration for virtual edges, 51
saving                                                                           short edge limit, 43
   volume mesh, 101                                                              sliver factor limit, 43
selecting                                                                     toolbars, 9
   location, 12                                                                  geometry, 15
   point on a face, 13                                                           interrupt, 16
   using coordinates, 13                                                         mesh edge length, 14
   using graphics window, 12                                                     meshing, 16
   using selection rectangles, 12                                                rotation modes, 9
   using tree view, 12                                                           selection modes, 14
   vertex, 13                                                                    triad and ruler, 14
selection filter                                                                 zoom controls, 9
   edge, 13                                                                   total thickness
   face, 13                                                                      considerations for inflation , 79
   point, 13                                                                  tree view
   region, 13                                                                    hide and show - items in the Tree View , 20
   toolbar, 13                                                                   highlighting the tree view items, 17
selection modes                                                                  status symbols - status of items in the Tree View, 17
   box select, 14                                                                suppressing objects, 19
   flood select, 14                                                           triad - See also toolbars; viewing, 15
   toolbar, 14                                                                triangle control
selection rectangles - See also regions, 12                                      description, 71
setting                                                                       troubleshooting

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
246                                                of ANSYS, Inc. and its subsidiaries and affiliates.
                                                                                                                                     Index

   common queries related to the meshing, 107                                     mouse zoom, 7
   error messages generated by CFX-Mesh, 107                                      zoom to fit, 9
   valid and invalid values, 107
tutorials
   list of features, 122

U
unsuppressing
  See also suppressing, 45
updating
  modifying the geometry, 25

V
verifying - See also checking, 43
vertex
   selecting, 13
viewing
   error messages due to undesirable geometry, 41
   mesh edge length, 14
   pan, 7
   restoring the original window layout, 8
   rotate, 7
   shaded display with 3D edges or wireframe using
   the display toolbar, 8
   status symbols - status of items in the Tree View, 17
   zoom - See also zoom controls, 7
virtual edges
   description, 51
   removing the short edges, 53
virtual faces
   description and example of, 48
virtual topology
   automatically edge merging tolerance, 103
   automatically remove invalidated virtual cells, 103
   creating a virtual faces, 48
   creating the virtual edges, 51
   defined, 47
   guidelines for creating and adding virtual face and
   virtual edge, 47
visibility - See also selecting; viewing, 12
volume mesh
   generating, 3
   problems with degenerate geometry , 40
   saving volume mesh, 101

W
wireframe display - See also viewing, 8

Z
zoom controls
  box zoom, 9

                       Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
                                                   of ANSYS, Inc. and its subsidiaries and affiliates.                                247
      Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
248                               of ANSYS, Inc. and its subsidiaries and affiliates.

				
DOCUMENT INFO
Categories:
Tags:
Stats:
views:8
posted:8/22/2012
language:English
pages:256
Subrahmanian KR Subrahmanian KR
About Civil Engineer