Chapter 1 Introduction to Autodesk Inventor - Goodheart-Willcox

This sample chapter is for review purposes only. Copyright © The Goodheart-Willcox Co., Inc. All rights reserved.
Learning Objectives
CHAPTER
Introduction
to Autodesk
Inventor
After completing this chapter, you will be able to do the following:
✓ Describe the primary Autodesk Inventor file types.
✓ Explain the concept of parametric modeling.
✓ Define the elements of a part model.
✓ Perform basic file activities, such as creating, opening, saving, and
closing files.
✓ Describe the Autodesk Inventor user interface.
✓ Control the multiple document interface.
✓ Access application options.
✓ Locate and use help resources.
Autodesk Inventor, referred to as Inventor throughout this textbook, combines
three-dimensional (3D) solid modeling with two-dimensional (2D) drawing capabilities.
See Figure 1-1. Inventor is a powerful computer-aided design and drafting
(CADD) system that allows you to start with very basic product design ideas and end
with a virtual prototype and a complete set of working drawings.
Inventor can be adapted to use and conform to a variety of mechanical drafting
standards. This textbook focuses on using Inventor according to the American National
Standards Institute (ANSI) and the American Society of Mechanical Engineers (ASME)
design and drafting standards. Other common standards, such as the American
Welding Society (AWS) standards, are also presented when appropriate.
Inventor Files
Inventor uses different files to prepare 3D part, assembly, and presentation models,
as well as 2D drawings. Each file serves a specific design and documentation purpose.
A basic design may require only a single part file or a part file and drawing file.
Complex projects that include multiple items may require hundreds of part, assembly,
presentation, and drawing files.
1
part: An item
or product or an
element of an
assembly.
Figure 1-1.
Inventor provides tools to create three-dimensional solid models and two-dimensional
drawings.
B
.394
.886 4X .541(=2.165)
(.541)
.886 .394
1.772 .394
2.657 .394
3.543
3.937
NOTES:
1. INTERPRET DIMENSIONS AND TOLERANCES PER ASME Y14.5M-1994.
2. REMOVE ALL BURRS AND SHARP EDGES.
.492
5X Ø5.000
THRU
Ø 10.000 5.000
Ø.005
M A B C M
.984
Part Files
Part files are used to create single parts and sheet metal parts. Figure 1-2 shows
an example of a part. You can create a part in a part file or build it in place while
you are working in an assembly file. When created in place, each part is saved as a
unique part file. Part files are referenced into assembly files as parts for assemblies
and weldments, and into drawing files to create 2D part drawings. Part files have the
file extension .ipt.
2 Inventor and Its Applications 2009
.984
C
2X R.394
8X R.394
.394
A
8X R.197
1.969
8X Ø.394
Ø.005
M A B
Ø.005
M
UNLESS OTHERWISE SPECIFIED
APPROVALS
DATE
DIMENSIONS ARE IN INCHES (IN.)
TOLERANCES:
.X
± .1
DRAWN DPM 6/20/2008 MADSEN DESIGNS INC.
.XX
± .01
CHECKED
.XXX DPM
± .005
TITLE
ANGULAR: ± 10'
APPROVED
FINISH: 62μIN.
SLIDE BAR HINGE
THIRD ANGLE PROJECTION
MATERIAL
SAE 51410
FINISH
SIZE DWG NO.
CAGE CODE
ALL OVER B
09-00125
REV
0
DO NOT SCALE DRAWING
SCALE
SHEET
1:1
1 OF 1

Figure 1-2.
An example of a
C-clamp body
created in a part file.
Assembly Files
Assembly files are used to create assemblies, subassemblies, and weldments.
Parts and subassemblies used to build an assembly are known as components. An
example of an assembly is shown in Figure 1-3. You can develop an assembly in a
separate assembly file or create it in place as a subassembly while you are working in
an assembly file. When created in place, each assembly is saved as a unique assembly
file. Assembly files are referenced into other assembly files as subassemblies, into
presentation files for creation of exploded and animated assemblies, and into drawing
files to create assembly drawings. Assembly files have the extension .iam.
Presentation Files
Presentation files are used to create exploded, animated, and stylized assembly
models that show how separate parts and subassemblies interact within the full
assembly. See Figure 1-4. Presentation files have an .ipn extension and reference
existing assembly files. They are also referenced into drawing files to create exploded
assembly drawings.
Figure 1-3.
An example of a
C-clamp developed
in an assembly file.
weldment: An
assembly in which
parts are fixed
together with welds.
components: The
individual parts
and subassemblies
used to create an
assembly.
Chapter 1 Introduction to Autodesk Inventor 3
drawings: 2D
representations of
models containing
views, dimensions,
and annotations.
Figure 1-4.
This presentation of
a C-clamp contains
trails, or connection
graphics between
components that
show their relative
positions in the
assembly.
Drawing Files
Drawing files are used to create 2D drawings. See Figure 1-5. Drawings reference
existing part, assembly, and presentation files. Drawing files can have the extension
.idw or .dwg.
Figure 1-5.
A drawing file should contain enough information to describe the part or assembly
completely. This drawing is used to document the design of a C-clamp body.
14
9.5
9.5
25.45
20.65
14
2X R6.35
50.8
M10x1.5 - 6H
NOTES:
1. INTERPRET DIMENSIONS AND TOLERANCES PER ASME Y14.5M-1994.
2. REMOVE ALL BURRS AND SHARP EDGES.
19
14
14
19
14
101.6
14
4 Inventor and Its Applications 2009
Trail
Trail
UNLESS OTHERWISE SPECIFIED
APPROVALS
DATE
DIMENSIONS ARE IN MILLIMETERS (mm)
TOLERANCES:
.X
± 0.5
DRAWN
DPM 6/20/2008 GOODHEART-WILLCOX
.XX
± 0.05
.XXX
±0.005
CHECKED
TITLE
ANGULAR: ± 10'
APPROVED
FINISH:
3.2μm
C-CLAMP BODY
THIRD ANGLE PROJECTION MATERIAL
SAE 4140
FINISH
SIZE
CAGE CODE DWG NO.
ALL OVER A3
09-98089
REV
0
DO NOT SCALE DRAWING
SCALE 1:1
SHEET 1 OF 1

Web site
Exercise 1-1
Access the Student Web site (www.g-wlearning.com/CAD/InventorApps2009),
select Chapter 1 from the Chapter Materials drop-down list, and select
and complete Exercise 1-1.
Parametric Solid Modeling
Inventor works on the concept of parametric solid modeling. Parameters can be
adjusted to make changes to the model, but if the modifications conflict with other
geometry, the model cannot be built without errors. The parametric concept is also
referred to as intelligence because of the way model information is stored and managed
in a database.
Parametric Association
The easiest way to understand the basic principle of parametric association is
to study the size of a parametrically created geometric shape. For example, the first
circle shown in Figure 1-6 was drawn with a 1″ diameter. Adding a dimension to the
circle that defines the circle diameter as 2″ changes the size of the circle according
to the 2″ diameter dimension. When a new diameter of 3″ is applied to the circle, the
size of the circle changes from two to three inches in diameter. This example shows
how the size of the circle is associated with the circle dimension. The size of the
circle changes only when the parametric value of the dimension is edited.
Parametric modeling allows you to control every aspect of a model and drawing
during and after the design and documentation process. In the parametric modeling
world of Inventor, you begin a design with a basic 2D shape and develop it into a
complex 3D model. As you learn to use Inventor, you will recognize and work with the
parametric relationships between model and drawing elements throughout the entire
design process. Planning how to build a model and thinking about how it relates to
future parts, assemblies, and drawings is an important step in beginning a design.
Throughout this book, you will explore many examples of parametric relationships
and learn how to work within the parametric Inventor environment.
Figure 1-6.
After creating the circle, you can control its size by assigning a dimension.
Drawn at
1″ diameter
Added a 2″ diameter
dimension
Changed the dimension to 3″
parametric solid
modeling: A form
of modeling in which
parameters and
constraints drive
the model form and
function to produce
models that contain
object volume and
mass data that
can be used to
analyze internal
and external object
characteristics.
parameters:
Characteristics that
control the size,
shape, and position
of model geometry.
Chapter 1 Introduction to Autodesk Inventor 5
constraints:
Parameters that
control the size,
location, and
position of model
elements, including
sketches and
features.
fully constrained
model: A model that
has no freedom of
movement.
Understanding Constraints
Constraints are added in the form of dimensions and geometric associations. The use
of well-defined constraints preserves specific design intentions, even as revisions are made.
For example, if the center of a ∅10 mm hole in a square plate must be 12 mm away from
a specific edge, a constraint in the form of a dimension identifying the 12 mm distance is
added. If the edge is moved, the hole moves also, maintaining the 12 mm distance.
Constraints define model elements and protect your model and design ideas. An
under-constrained model is shown in Figure 1-7. As you progress through the design
process, you will often fully constrain the model to ensure that your design is accurate.
However, an over-constrained model—one that contains too many constraints—
generates a modeling failure and a warning. See Figure 1-8. Over-constrained and
modeling failure situations must be resolved before you can create a model.
Part Model Elements
Part models are the primary solid models. They are used to form subassemblies,
assemblies, and 2D part drawings. A part model begins as a sketch or group of sketches
that are then used to construct a feature. Additional features are added to the initial
feature to create a part model.
Sketches and Sketched Features
A sketch is typically the first item you create when developing a model. See
Figure 1-9. Sketches are used to create sketched features. Typically, every part model
contains at least one sketch and at least one sketched feature. Most of the time, the
sketch: A 2D
drawing that
provides the
profile or guide
for developing a
sketched feature.
sketched features:
Features such Figure 1-7.
as extrusions, The hole can be moved horizontally because it is not fully constrained.
revolutions, sweeps,
lofts, and coils that This hole is not fixed in
are built from a the horizontal direction
sketch.
6 Inventor and Its Applications 2009

Figure 1-8.
This warning appears when you try to add a dimension that causes an over-constrained situation.
Figure 1-9.
This simple sketch
has two dimensions
that control the
object’s size.
This dimension
is not needed
base feature is produced as a sketched feature. Ribs, embossments, and some holes
are also sketched features. See Figure 1-10.
Placed Features
Placed features include shells, fillets, chamfers, threads, and face drafts. See
Figure 1-11. Generating placed features requires adding size dimensions and selecting
a location, such as a point or edge.
base feature: The
initial model feature,
on which all others
are based.
placed features:
Features added to
an existing feature
without using a
sketch.
Chapter 1 Introduction to Autodesk Inventor 7
work features:
Reference or
construction
features that direct
the location and
arrangement of
other features.
Figure 1-10.
These sketched features are added to the base feature.
Extruded sketched
features
Figure 1-11.
Threads, fillets,
and chamfers are
a few of the placed
features available in
Inventor.
Work Features
Embossment created from
text on a sketch
Fillet
Work features are used for construction and reference purposes. They serve as a
basis for creating part geometry and features in areas where no other geometry is available.
Work features include work planes, work axes, and work points. See Figure 1-12.
Work features may be placed anywhere on a feature or in 3D space. Like other features,
work features are parametrically associated with a model.
8 Inventor and Its Applications 2009
Rib
Threads
Base feature
Chamfer

Figure 1-12.
Work features
are used to build
and control other
features.
Figure 1-13.
An example of a
catalog feature. This
feature contains
three holes and a
round.
Work
plane
Catalog feature
Work
point
Chapter 1 Introduction to Autodesk Inventor 9
Work
axis
Catalog Features
Catalog features are similar to placed features, because you can place a catalog
feature onto an existing feature. However, catalog features are often far more complex
than a standard shell, fillet, chamfer, or face draft. See Figure 1-13. Catalog features
include design elements such as iFeatures and derived components.
Feature Patterns
Once you create a feature, such as a hole, you may copy it into an arrangement
called a feature pattern. Inventor feature patterns include rectangular patterns, circular
patterns, and mirrored features. Examples of feature patterns are shown in Figure 1-14.
iFeature: An
existing feature or
set of features you
create and then
save and store in a
catalog to be used
in other models.
derived
components:
Features that can
contain a complete
model consisting of
several features, or
even multiple parts;
often used as a
base feature.
feature pattern:
An arrangement
of copied existing
features, generating
occurrences of the
features.
Exercise 1-2
Access the Student Web site (www.g-wlearning.com/CAD/InventorApps2009),
select Chapter 1 from the Chapter Materials drop-down list, and select
and complete Exercise 1-2.
Getting Started
icon: A small When Inventor is first installed, Windows creates an Inventor icon, which is
graphic representing
an application, file, displayed on the Windows desktop and in the list of programs available from the
or tool.
Start menu. One of the quickest methods to start Inventor is to double-click on the
Inventor desktop icon. Another option is to pick the Start button in the lower-left
corner of the Windows desktop, move the cursor to Programs and hold it there or
pick, and then select Autodesk, Autodesk Inventor 2009, and finally Autodesk Inventor
Professional 2009.
The Open dialog box appears by default when you start Inventor. See Figure 1-15.
The Open dialog box is used to locate and open existing files. Options are also available
for accessing the New File dialog box and for activating and managing projects.
templates: Files
with predefined
settings that are
used to begin new
documents.
Figure 1-14.
Use patterns to create multiple copies of a feature or group of features.
Rectangular Pattern Circular Pattern Mirrored Feature
Web site
Beginning a New File
Pick the New File button in the Quick Start area of the Open dialog box to begin a
new file using the New File dialog box. See Figure 1-16. This dialog box is the primary
tool used to access templates for creating new Inventor parts, assemblies, presentations,
and drawings. The New File dialog box can also be accessed by selecting the
New… option on the File pull-down menu, typing [Ctrl]+[N], or picking the New button
on the Inventor Standard toolbar.
10 Inventor and Its Applications 2009

Figure 1-15.
The default display shown when you first launch Inventor includes the Open dialog box.
Pick to access
the New File
dialog box
Pick to access
the Open
dialog box
Figure 1-16.
Templates for
creating new files
are located in tabs
along the top of the
New File dialog box.
New and Open options are available
from the File pull-down menu
Pick to begin
a new file
Sheet metal
part
This button becomes
available after certain
files are selected
Contains templates based on choosing English
or metric during program installation
Contains templates based on U.S. Customary units
Contains templates based on metric units
Standard
drawing
Standard
assembly
Standard
drawing
Standard
presentation
Standard part
Weldment
(welded
assembly)
Chapter 1 Introduction to Autodesk Inventor 11
When AutoCAD is
configured to display
a screen menu, the
commands appear in
a separate screen.
NOTE
The New button on the Inventor Standard toolbar, shown in
Figure 1-15, is a fl yout that contains Assembly, Drawing, Part, and
Presentation options. These selections are used to quickly access
a new standard part, assembly, drawing, or presentation template
fi le. The templates located in the New fl yout button are those found
in the Templates folder and listed in the Default tab of the New File
dialog box.
By default, the New File dialog box contains Default, English, and Metric tabs. On
each tabbed page are Inventor template files, represented by unique icons. You can
specify the Default tab as English or Metric when you install the program, based on the
units you typically use. The English and Metric tabs hold templates with specific units
for each Inventor file type, including ANSI in the English tab, and ANSI, BSI, DIN, GB,
ISO, and JIS in the Metric tab.
Sheet metal and weldment templates are also available in the New File dialog box.
These templates are not actually separate file types, as indicated by the .ipt and .iam file
extensions. They are template files that are preset for specific model applications. A
sheet metal template automatically provides the tools used to create a sheet metal part.
A weldment template offers the welding tools necessary to create a weldment.
To begin a new file, double-click on the template icon. You can also pick the icon
and then pick the OK button in the lower-right portion of the New File dialog box to
start a new file.
When AutoCAD is
configured to display
a screen menu, the
commands appear in
a separate screen.
Web site
NOTE
The tabs and template fi les displayed in the New File dialog box are
fully customizable. To specify the tabs and templates shown in the
New File dialog box, use projects or create new tabs in the default
template folder. Projects and templates are introduced in Chapter 2.
Exercise 1-3
Access the Student Web site (www.g-wlearning.com/CAD/InventorApps2009),
select Chapter 1 from the Chapter Materials drop-down list, and select
and complete Exercise 1-3.
Opening an Existing File
Use the Open dialog box, shown in Figure 1-15, to access existing Inventor files
and to import non-native CADD files into Inventor. Access the Open dialog box from
the New File dialog box by picking the Open button in the Quick Start area. The Open
dialog box can also be accessed by selecting the Open… option from the File pull-down
menu, typing [Ctrl]+[O]; or picking the Open button on the Inventor Standard toolbar.
12 Inventor and Its Applications 2009

When AutoCAD is
configured to display
a screen menu, the
commands appear in
a separate screen.
NOTE
You can open existing fi les directly from Microsoft Windows
Explorer, or you may be able to fi nd fi les using the quick document
access area located near the bottom of the File pull-down menu. This
area lists the path and fi le name of several previously used documents.
The fi les are listed in the order they were opened, and each
path is associated with a number. Number 1 is the most recently
opened fi le.
When you access the Open dialog box, the folder assigned to the active project
is displayed, allowing you to quickly access files associated with the active project.
However, you can navigate to any file on your computer or the network. Files do not
have to be in the active project to be opened. The Open dialog box functions much like
similar dialog boxes found in other Windows applications.
Use the Files of type drop-down list to specify the type of files to display in the
Open dialog box. Then use the Look in drop-down list, the Go To Last Folder Visited,
Up One Level, Create New Folder, and View Menu buttons along the top of the dialog
box, and the Preview area as needed to locate the desired file. Once you select a file,
the Options... button may become available. Picking this button opens the File Open
Options dialog box. The choices available in this dialog box vary depending on the
selected file type. To open a file, double-click on the file icon, or pick the icon and then
pick the Open button in the lower-right portion of the New File dialog box.
When AutoCAD is
configured to display
a screen menu, the
commands appear in
a separate screen.
Web site
PROFESSIONAL TIP
If you forget where an Inventor fi le has been placed, you can use the
Windows search tool to fi nd it, but Inventor also has a method of
fi nding fi les that may be quicker. The Inventor search tool is conveniently
located in the Open dialog box. Pick the Find... button to open
the Find: Inventor Files dialog box.
NOTE
Double-clicking on an Inventor fi le in Microsoft Windows Explorer
causes Inventor to start, if it is not already running, and opens the
selected fi le.
Exercise 1-4
Access the Student Web site (www.g-wlearning.com/CAD/InventorApps2009),
select Chapter 1 from the Chapter Materials drop-down list, and select
and complete Exercise 1-4.
Saving Your Work
A model or drawing you want to keep must be saved. Typically, the first step
in creating a model or drawing is to save the file in an appropriate location using a
descriptive name or code. Then, as you work, save the file frequently; at least every five
to ten minutes, in case of a sudden loss of power or a computer problem that may cause
the loss of your file.
Chapter 1 Introduction to Autodesk Inventor 13
Using the Save Tool
A quick way to save your work is to pick the Save button on the Inventor Standard
toolbar. You can also select the Save option from the File pull-down menu or type
[Ctrl]+[S]. The Save tool resaves the file if it has already been saved, or opens the Save As
dialog box if the file has not previously been saved. See Figure 1-17. The Save As dialog
box functions much like similar dialog boxes found in other Windows applications.
The file type listed in the Files of type drop-down list should be set to the current
file type. Use the Look in drop-down list or the buttons along the top of the dialog box
as needed to locate the file. Pick the Options... button to open the File Save Options
dialog box, which controls the method of generating a preview image for the file. This
image is displayed in the Preview area of the File Open dialog box. Pick the Save button
to complete the save.
Using the Save As Tool
The Save As tool, which displays the Save As dialog box, is available by picking
the Save As… option from the File pull-down menu. When you use the Save As tool,
the original file closes, and the newly saved file with the specified name appears. For
example, if you are working on a part named LARGE PLATE and want to use the file
as a basis for a small plate design, use the Save As tool to save a copy of the part titled
SMALL PLATE. The LARGE PLATE file closes and the SMALL PLATE file appears, ready
for modification. You will use the Save As tool throughout the exercises and problems
in this textbook to save an existing file using a different name.
Using the Save Copy As Tool
The Save Copy As tool is available by picking the Save Copy As… option from
the File pull-down menu. Selecting this tool displays the Save Copy As dialog box,
which is similar to the Save As... dialog box. When you use the Save Copy As tool, the
original file does not close. The copy is saved to the specified location and does not
open. Use the Save Copy As tool when you want to continue working on the original
file, but make a copy as a design state backup or for use at a later time.
The Save Copy As tool is also used to save an Inventor file as a non-native or alternative
format, such as IGES, JPEG, or STEP. These file formats may be necessary when
Figure 1-17.
The Save As dialog box appears if the current file has not been saved.
The list of file types is restricted
to match the current type
Type the new file name in this box
14 Inventor and Its Applications 2009

you are collaborating with others or when you need to create an image from what is
shown on-screen. Savable file formats are available from the Save as type drop-down
list in the Save Copy As dialog box.
Closing a File
One of the quickest methods of closing a file, without ending the Inventor session,
is to pick the Close button on the right side of the file window title bar. Other options
include double-clicking on the file icon on the file window title bar, and selecting the
Close option from the File pull-down menu.
When AutoCAD is
configured to display
a screen menu, the
commands appear in
a separate screen.
NOTE
Many design projects require that multiple fi les be open. To save
changes to all open fi les, use the Save All tool. To close all open
fi les, use the Close All tool. Both tools are available from the File
pull-down menu.
Exiting Inventor
To exit Inventor, pick the Close button located in the upper-right corner of the
Inventor window, double-click the Inventor window title bar, select Exit from the File
pull-down menu, or pick the Inventor icon located in the upper-left corner of the Inventor
window and select Close. When you close a file or exit Inventor, several alert boxes may
appear, depending on the situation. For example, if you have not saved your work, you
are asked if you want to save the file before closing.
Web site
Exercise 1-5
Access the Student Web site (www.g-wlearning.com/CAD/InventorApps2009),
select Chapter 1 from the Chapter Materials drop-down list, and select
and complete Exercise 1-5.
The Inventor Interface
Interface, or user interface, items include devices such as the keyboard and mouse
to input data, and the monitor to receive information. The Inventor graphical user
interface (GUI), shown in Figure 1-18, includes both standard Microsoft Windows
functions and specialized Inventor items. The specialized interface tools and options
are used for preparing models and drawings and are described when appropriate
throughout this textbook.
The Inventor interface constantly changes as you develop a part, assembly, presentation,
or drawing. Only the tools and options that apply to the current work environment
and design or drafting task are available. For example, the part file interface is
displayed in Part mode and contains the tools and options required to create parts.
Interface items such as the panel bar and pull-down menu options automatically change
as you progress through each design phase and work with different file types.
interface (user
interface): The
tools and techniques
used to provide
information to and
receive information
from a computer
application.
graphical user
interface (GUI):
On-screen
interface items.
Chapter 1 Introduction to Autodesk Inventor 15
floating: Describes
interface items,
displayed within a
border, that can
be freely resized
or moved.
docked: Describes
interface items
that are locked
into position on
an edge of the
Inventor window
(top, bottom, left,
or right).
Figure 1-18.
Elements of the Inventor interface.
Panel bar Shortcut and hot keys Toolbar buttons Dialog box
Browser bar Shortcut menu Communication center button
When AutoCAD is
configured to display
a screen menu, the
commands appear in
a separate screen.
Interface Terminology
NOTE
This textbook focuses on the default Inventor interface. Only
default interface items are shown throughout this textbook, except
in specifi c situations that require additional information.
Figure 1-19 provides a list and description of interface terms used throughout
this textbook. Become familiar with these terms and reference Figure 1-19 as you
learn Inventor.
Controlling Windows and Interface Items
The Inventor program and graphics windows are similar to other windows within
the Windows operating system. To minimize, maximize, or close the Inventor window or
individual graphics windows, pick the small control icon in the upper-left corner, which
displays a standard window control menu, or pick the appropriate icon in the upperright
corner. Window sizing operations are the same as those for any other window.
Several Inventor interface items, including the Inventor and graphics windows,
can float or be docked. Different options and functions are available, depending on
the particular interface item and whether the item is floating or docked. Some items,
16 Inventor and Its Applications 2009

Figure 1-19.
Common interface terms and descriptions.
Term Description
Alias A keyboard key or key combination used to define and access a
command or tool.
Button A button on the screen or mouse.
Command An instruction issued to the computer.
Cursor The primary means of pointing to and selecting objects within the
Inventor window.
Default A value maintained by the computer until you change it.
[Enter] (↵) The [Enter] key on the keyboard.
Function key One of the keys labeled [F1]–[F12] along the top of the keyboard.
Glyph A graphic representation, typically initiating an action, symbol, or
function. For example, a perpendicular glyph represents a
perpendicular geometric situation.
Graphics window The largest area in the Inventor window, where modeling and
drawing occur.
Hover Use the mouse to move the cursor over an item and hold the cursor
at the location to display additional information or options.
Icon An image identifying or depicting the function of an interface item.
Key A key on the keyboard.
Option An aspect of a command or tool that can be selected.
Pick or click Use the left mouse button to select an item on the screen.
Tool A command used to perform a specific task. For example, the Line
tool is used to draw lines.
such as the graphics window, have a title bar at the top or side. The close and minimize
or maximize options are often available, and most items can be resized. Some floating
items, such as toolbars and panels, include grab bars.
When AutoCAD is
configured to display
a screen menu, the
commands appear in
a separate screen.
NOTE
The graphics windows can be adjusted and positioned only within
the Inventor window.
Using Shortcut Menus
Shortcut menus, also known as pop-up, cursor, and right-click menus, are used extensively
in Inventor. See Figure 1-20. The option at the top of a shortcut menu allows you
to quickly access the previously selected tool or option. Some menu options have a
small arrow to the right of the option name. When you pick one of these options, a
cascading menu appears. See Figure 1-21.
grab bars: Two thin
bars at the top or left
edge of a docked or
floating item; used
to move the item.
shortcut menus:
Menus that allow
access to tools and
options by rightclicking
anywhere in
the graphics window
or on an object or
selection.
cascading menu:
A secondary menu
that contains options
related to the chosen
menu item.
Chapter 1 Introduction to Autodesk Inventor 17
context-sensitive
shortcut menu:
Menu in which only
items associated
with the current
work environment
and application are
displayed.
pull-down menus:
A text-based menu
input system in
which options
appear when you
pick the menu name.
Figure 1-20.
The shortcut menu that appears depends on the item under the cursor when you right-click.
Cursor is on the Cursor is on a sketch
graphics window
in the browser
Figure 1-21.
Cascading menus
are available from
shortcut menus and
from pull-down
menu options that
have a flyout arrow.
You can access the tools and options available from shortcut menus using many of
the other interface techniques. However, because shortcut menus are context sensitive
and positioned near the cursor, you can improve the speed with which you perform
tasks and access options that may otherwise be difficult to find. A shortcut menu often
provides the quickest method for accessing a tool or option. Therefore, shortcut menu
access is presented first in this textbook for tools and options that are best accessed
from a shortcut menu.
Using Pull-Down Menus
Cursor is on a feature
in the browser
Arrow indicates
that cascading menu
is available
Cascading menu
The pull-down menu bar, shown in Figure 1-22, houses the pull-down menus that
are available for the particular work environment. Pick a pull-down menu to reveal the
options for that menu. Then move the cursor down and up to highlight and select the
desired menu option. Like shortcut menus, some pull-down menu options display an
arrow to the right of the menu selection, indicating that a cascading menu of related
options is available. To close the currently selected menu without opening another
menu, press the [Esc] key, pick outside of the menu list, or pick on the menu bar. If you
18 Inventor and Its Applications 2009

Figure 1-22.
The View pulldown
menu is an
example of the many
pull-down menus
available in Inventor.
want to change to a different menu, move the cursor over the specified menu name or
pick the menu name.
A tool or option accessible from a pull-down menu is presented as a graphic in
the margin of this textbook, like the example shown in the margin. The graphic in this
example represents the process of picking the File pull-down menu, then hovering
over and selecting the Save option to activate the Save tool.
When AutoCAD is
configured to display
a screen menu, the
commands appear in
a separate screen.
Pick the menu name
to display options
NOTE
You can also access menus and menu options using menu accelerator
keys. One method involves holding down the [Alt] key while
pressing the key that corresponds to the underlined character in
the menu. Another option involves the use of control keys, which
are shown to the right of the option name and allow you to access
certain tools by pressing and holding the [Ctrl] key while pressing a
second key. Once a menu appears, you can also use the up, down,
right, and left arrow keys to move to different items in the menus.
Press [Enter] to select a highlighted item. Despite the name, using
accelerator keys is usually a more diffi cult means of selecting tools
from the menu system.
The Inventor Standard Toolbar
Toolbars display tool buttons arranged into groups of similar tools that are separated
by thin lines. Many toolbars are available that apply to specific tasks, but by
default, only the Inventor Standard toolbar is shown. See Figure 1-23. Toolbars have
features similar to pull-down menus.
Some toolbar buttons have an arrow to the right of the button, known as a flyout.
See Figure 1-24. These buttons work the same as other toolbar buttons. To use the
flyout, select the arrow next to the button. This opens the other options associated with
the button. In most cases, when you pick a flyout option, the selected button becomes
active and is displayed on the toolbar on the top level of the flyout, hiding the rest of
the buttons.
Menu Browser
File
> Save
tool buttons:
Buttons in a toolbar,
each with a specific
icon, that activate a
tool or option.
flyout: A button
that presents
additional, related
tool buttons,
much like a
cascading menu.
Chapter 1 Introduction to Autodesk Inventor 19
Toolbar
Inventor
Standard
> Save
Figure 1-23.
These detail images of the Inventor Standard toolbar show the types of features that may be
found on all toolbars.
Figure 1-24.
Pick the flyout arrow
next to some buttons
to see additional tool
buttons.
This textbook focuses on the default interface display, which includes only the
Inventor Standard toolbar. A tool or option accessible from the Inventor Standard toolbar
is presented as a graphic in the margin of this textbook, like the example shown in the
margin. The graphic in this example represents the process of picking the Save button
to activate the Save tool.
Web site
Material color list box
Supplemental Material
Pick to close the toolbar
New File button Separator bar
Flyout for the
New button
Additional Toolbars
Additional Inventor toolbars are available and can be displayed in the
Inventor window. These toolbars are usually application- or task-specific. For
more information on displaying and using toolbars, go to the Student Web
site (www.g-wlearning.com/CAD/InventorApps2009) and select Chapter 1 in the
Chapter Materials drop-down list. In the Supplemental Material section, select
Additional Toolbars.
20 Inventor and Its Applications 2009

Using the Panel Bar
The panel bar, shown in Figure 1-25, provides a list of design tools available for
creating sketches, models, and drawings, depending on the specific work environment.
Only the tools and options used for creating parts are available in the panel bar
while you are working on a part. The specific tools displayed in the panel bar change
as you move from one design stage to another. For example, only sketch tools are available
while you are working on a part in sketch mode. When you finish the sketch, the
Part Features panel bar appears. In addition, only tools that can be used in the current
design stage are available for selection; all others are shaded.
Click on the current panel bar title, such as 2D Sketch Panel, or right-click on
or beside any of the panel bar tools to display a shortcut menu of options. Select a
panel bar mode from the shortcut menu to change manually from one list of options
to another. By default, the panel bar displays each tool with both an icon and the name
of the tool, as shown in Figure 1-25A. This helps you to recognize tools when you
first begin to work with Inventor. Deselect the Display Text with Icons option from the
shortcut menu to display only tool buttons. This is helpful if you want a smaller panel
bar display, allowing for a larger graphics window. See Figure 1-25B.
When AutoCAD is
configured to display
a screen menu, the
commands appear in
a separate screen.
NOTE
The panel bar can be moved and resized, and it can be docked or
fl oat in the graphics window.
A tool or option accessible from the panel bar is presented as a graphic in the
margin of this textbook, like the example shown in the margin. The graphic in this
example represents the process of picking the Extrude button from the Part Features
panel bar to activate the Extrude tool.
Keyboard Shortcuts
An alternative method to access some Inventor tools and options is to type a
keyboard character or combination of characters. For example, press the [Ctrl] and
[S] keys, a combination identified in this textbook as [Ctrl]+[S], to activate the Save tool.
Figure 1-25.
A—The panel bar
displayed with
names to aid in
identifying tools.
B—The panel bar
with the Display
Text with Icons
option deselected
to conserve screen
space.
A B
panel bar: A
panel-like window
that appears by
default on the left
side of the Inventor
graphics window.
Panel bars are the
primary location
for accessing
design tools.
Panel
Part Features
Chapter 1 Introduction to Autodesk Inventor 21
Extrude
Type
E
browser bar
(browser): A panel
that displays all the
items in the current
model or drawing.
However, accessing tools from a shortcut or pull-down menu, toolbar, or the panel bar
can offer advantages over typing at the keyboard. One benefit is that you do not need
to memorize tool aliases and combinations. As an Inventor user, you decide which tool
selection technique works best for you. A combination of tool selection methods often
proves most effective.
When AutoCAD is
configured to display
a screen menu, the
commands appear in
a separate screen.
NOTE
Even though you may choose not to access tools by typing keyboard
shortcuts, you must still enter certain values at the keyboard. For
example, you may have to enter the diameter of a circle using
the keyboard.
A tool or option that is accessible by typing is presented as a graphic in the
margin of this textbook, like the example shown in the margin. The graphic in this
example represents the process of pressing the E key on the keyboard to activate the
Extrude tool.
Web site
Pressing the [Esc] key is a fast and easy way to exit a tool. The [Delete]
key is a quick way to remove an item, and may be the only way to
delete certain selections or settings from a dialog box. Press the [Enter]
key or space bar to access the previously selected tool.
Supplemental Material
Character Keys and Key Combinations
Many individual character key and key combination shortcuts are available
for accessing Inventor tools and options. For a list of keyboard shortcuts,
go to the Student Web site (www.g-wlearning.com/CAD/InventorApps2009) and
select Chapter 1 in the Chapter Materials drop-down list. In the Supplemental
Material section, select Character Keys and Key Combinations.
Using the Browser Bar
PROFESSIONAL TIP
The browser bar, or browser, provides a historical reference of model design and
drafting. See Figure 1-26. The number and type of items available in the browser
varies depending on the current model type, work environment, and design stage.
For example, a browser shown when a part file is open typically displays the name of
the file and an icon on top, followed by the Origin folder and all of the origin options,
followed by individual sketches and features. End of Part displays last, unless it has
been moved. An item in the browser is active when all other items are shown with a
gray background.
When AutoCAD is
configured to display
a screen menu, the
commands appear in
a separate screen.
NOTE
Items in the browser are listed in the order they were created or
inserted, although it is possible in some cases to drag and drop
browser items up or down in the list.
22 Inventor and Its Applications 2009

Figure 1-26.
The browser bar
contains information
regarding the
objects in a model
or drawing. The
browser in this
figure is associated
with a part file
that contains two
sketched features
and a placed feature.
Many of the items displayed in the browser are arranged in a tree structure, which
contains parent nodes and child nodes. A sketched feature is an example of a parent
node. The sketch from which the feature was created is the associated child node.
The Origin folder is another example of a parent node. To display child nodes, pick
the Expand button (+ symbol) to the left of the object name or right-click on the object
name and select Expand All Children. To hide child nodes, pick the Collapse button
(– symbol) to the left of the object name or right-click on the object name and select
Collapse All Children.
When AutoCAD is
configured to display
a screen menu, the
commands appear in
a separate screen.
Using the Status Bar
Pick to collapse
the branch
Pick to expand
the branch
The Origin folder contains
planes, axes, and a center
point to position and
orient geometry
Parent node
Child node
NOTE
The browser can be moved and resized, and it can be docked or
fl oat in the graphics window.
The status bar is located along the bottom of the Inventor window. See Figure 1-27.
The status bar is divided into panes that display and control a variety of drawing aids
and tools. The left side of the status bar provides information about a tool option by
displaying a help string. For example, if you highlight New... in the File pull-down menu,
the help string in the status bar is Create a new document. When you access the Line tool
to sketch a line, the help string is Select start of line, drag off endpoint for tangent arc.
Figure 1-27.
The status bar displayed when a part file is open.
Help string
Sketch resources
Number of
occurrences
Number of
open documents
Displays
memory
usage
Pick to access the
Communication
Center
parent node: An
item in the tree
structure, similar
to a folder, that is
associated with
subordinate
child nodes.
child node:
Subordinate nodes
that create, are
associated with, or
are consumed by a
parent node item.
help string: A short
text description of
what happens if
you select a tool
or option over
which the cursor
is hovering; or, if a
tool is selected, a
prompt indicating the
appropriate action.
Chapter 1 Introduction to Autodesk Inventor 23
dialog box: A
window-like part of
the user interface
that contains various
kinds of information
and settings.
The items on the right side of the status bar include a coordinate display field
or sketch constraint information, number of occurrences in the document, number
of open documents, memory usage, and a link to the Communication Center. Status
bar items appropriate to basic Inventor functions are described when applicable
throughout this textbook.
Using Dialog Boxes
Pick any menu selection or button displaying an ellipsis (…) to activate a dialog
box. See Figure 1-28. The cursor is used to set variables and select items in a dialog
box. In addition, many dialog boxes include images, previews, or other methods to
help you select appropriate options. When you pick a button in a dialog box that is
followed by an ellipsis, another dialog box appears. You must make a selection from
the second dialog box before you can return to the original dialog box. A button with
an arrow icon requires you to make a selection in the drawing area.
Figure 1-28.
Pick a menu option or tool button that includes an ellipsis (…) to display a dialog box.
Tabs
Preview box
Check box
Radio button
Edit box
Command button
Ellipsis indicates a dialog
box is available
Drop-down list
This dialog box
appears when
Print... is picked
24 Inventor and Its Applications 2009

Web site
Supplemental Material
Features of Dialog Boxes
Dialog boxes contain many of the same features found in other interface
items, including icons, text, buttons, and flyouts. For more information
about these features, go to the Student Web site (www.g-wlearning.
com/CAD/InventorApps2009) and select Chapter 1 in the Chapter Materials
drop-down list. In the Supplemental Material section, select Features of
Dialog Boxes.
Identifying Tooltips
Many buttons found in toolbars, the panel bar, and dialog boxes provide tooltips
to help you understand and recognize the button. Figure 1-29 shows the tooltip for the
Open button on the Inventor Standard toolbar. The tooltip tells you that the button you
see activates the Open tool.
Web site
Web site
Figure 1-29.
Place the cursor over
a button to reveal
the button name as a
tooltip.
Exercise 1-6
Access the Student Web site (www.g-wlearning.com/CAD/InventorApps2009),
select Chapter 1 from the Chapter Materials drop-down list, and select
and complete Exercise 1-6.
Supplemental Material
Using the Customize Dialog Box
The Customize dialog box is a basic tool for customizing the Inventor
interface. It can be used to define settings for the work environment, toolbars,
and tools. For more information on using the Customize dialog box,
go to the Student Web site (www.g-wlearning.com/CAD/InventorApps2009)
and select Chapter 1 in the Chapter Materials drop-down list. In the
Supplemental Material section, select Using the Customize Dialog Box.
Tooltip for the
Open button
tooltip: A small text
box that displays
when you hover
over a button,
giving information
about the function
of the button.
Chapter 1 Introduction to Autodesk Inventor 25
multiple document
interface: An
interface that
allows you to have
several documents
or document views
open at the same
time. Also called
multiple design
interface.
Managing Multiple Documents
You can use individual file Window Control pull-down menus and the Windows
pull-down menu to manage the multiple document interface. The Window Control
pull-down menu for an Inventor file is accessed by picking the Inventor file icon.
If the file window is maximized, the Window Control pull-down menu is located
to the left of the pull-down menu bar. If the file window is restored or minimized,
the Window Control pull-down menu is located in the graphics window to the left
of the file menu bar. The menu options available when you select a file icon function
much like program window control menu options. However, when you restore,
move, size, minimize, maximize, or close a file window, the operation affects only
the file window, not the entire program. The Next option allows you to toggle among
multiple open files.
The Window pull-down menu, shown in Figure 1-30, contains options for controlling
the multiple document interface. Pick the New Window option to create a new
window for the active file. Additional windows enable you to have several design
views open and accessible at once. The Cascade option arranges all windows in a
cascading fashion. See Figure 1-31A. The Arrange All option arranges all windows in
a way that shows each window in its entirety. See Figure 1-31B.
The names of all currently open documents are displayed at the bottom of the
Window pull-down menu. Refer again to Figure 1-30. The file name with a check mark
next to it is currently the active window. To make a different window active, pick its
file name.
Web site
Figure 1-30.
Use the Window
pull-down menu
to create a new
window, position the
current windows,
and view the list of
open files. A check
appears next to the
active file.
Exercise 1-7
Access the Student Web site (www.g-wlearning.com/CAD/InventorApps2009),
select Chapter 1 from the Chapter Materials drop-down list, and select
and complete Exercise 1-7.
Currently
active
document
This window was created when
the New Window option was selected
while Frame.ipt was active
Currently open
documents
26 Inventor and Its Applications 2009

Figure 1-31.
Positioning windows in Inventor using the Cascade option (A), and the Arrange All option (B).
A
B
Controlling Application Options
Application options are located in the Application Options dialog box. See
Figure 1-32. To display this dialog box, select Application Options… from the Tools
pull-down menu. Application options are general program settings and preferences
and are not specific to any particular file. However, many application options do
help configure specific work environments, as well as design and drafting tasks.
For example, options in the Sketch tab of the Application Options dialog box control
functions specific to preparing sketches.
Menu Browser
Tools
> Application
Options…
Chapter 1 Introduction to Autodesk Inventor 27
Figure 1-32.
The General tab of the Application Options dialog box. This dialog box controls many general,
file, and environment-specific program settings.
Application options control an extensive number of Inventor functions. For
example, the User name text box on the General tab, shown in Figure 1-32, is used
to redefine your username, which is used in multiple applications to indicate who
has worked on a file. Another example in the General tab is the Start-up action check
box. When selected, this check box allows you to choose to display the Open dialog
box, display the New File dialog box, or immediately begin a new file using a selected
template when you launch Inventor.
As you learn Inventor, you will become familiar with many application options,
and you may need to adjust the settings to fit your needs. You should explore the
Application Options dialog box and learn to recognize the purpose and usefulness of
each option. This textbook focuses on the default application options. Specific options
are covered only if they require adjustment in order to improve productivity, accomplish
certain tasks, accommodate design and drafting standards, or require explanation
for basic Inventor applications. These options are described when applicable
throughout this textbook.
Web site
Exercise 1-8
Pick a tab to
access specific
application
options
Pick to apply
options before
closing
Access the Student Web site (www.g-wlearning.com/CAD/InventorApps2009),
select Chapter 1 from the Chapter Materials drop-down list, and select
and complete Exercise 1-8.
28 Inventor and Its Applications 2009

Figure 1-33.
The Autodesk Inventor Help dialog box contains several tools to help you understand various
areas of Inventor.
Type keywords to
display matching
help topics
Access help
information
organized in
a book-like
format with
expandable
“chapters”
Search for
specific
words
and phrases
Getting Help
Inventor includes an extensive help file system that provides learning resources
and can be used to receive answers to questions. You can select from a variety of help
tools in the Help pull-down menu, including links that open the Autodesk Inventor
Help dialog box, Inventor and Vault tutorials, the New Features Workshop, and other
learning tools.
The Help button, next to the Help pull-down menu, opens the Autodesk Inventor
Help dialog box. See Figure 1-33. The help file system is similar to other Windowsbased
help files. It allows you to further explore areas of Inventor and receive answers
to any questions you may encounter. You can also access the Autodesk Inventor Help
dialog box by selecting Help Topics from the Help pull-down menu, pressing the [F1]
key; or picking the Help button on numerous dialog boxes, the panel bar, or the browser.
Picking a Help button in a dialog box opens the Autodesk Inventor Help dialog box
with information specific to the content of the dialog box.
Define and
display help
topics as
favorites
Chapter 1 Introduction to Autodesk Inventor 29
Web site
Chapter Test
Answer the following questions. Write your answers on a separate sheet of paper or go to the
Student Web site (www.g-wlearning.com/CAD/InventorApps2009), select the correct chapter
from the Chapter Materials drop-down list, and complete the electronic chapter test.
1. Define parts in the context of the Inventor software.
2. Describe the basic use of part files and specify the part file extension.
3. What is an assembly?
4. What name is given to an assembly in which parts are fixed together with welds?
5. What are components?
6. Identify the basic use of assembly files and specify the assembly file extension.
7. Explain the relationship between assemblies and subassemblies.
8. What name is given to the connection graphics between components that show
how each component fits into an assembly?
9. What are tweaks?
10. Describe the basic use of presentation files and specify the presentation file
extension.
11. What is the purpose of a drawing in Inventor?
12. Describe the basic use of drawing files and provide two possible file extensions
for these files.
13. What is parametric solid modeling?
14. In the context of solid modeling, what is a parameter?
15. Why is the parametric concept referred to as intelligence?
16. What is the purpose of a database in Inventor?
17. What are constraints?
18. Describe the basic function of a sketch.
19. Define the term placed feature and identify at least three examples of objects that
can be placed features.
20. Describe the basic function of work features.
21. What is a feature pattern?
22. What dialog box appears by default when you start Inventor?
23. What are templates, and what are they used to create?
24. Define interface and identify at least two items that are included in a typical
computer interface.
25. What is the Inventor graphical user interface (GUI), and what does it include?
26. What does it mean when an interface item is floating?
27. Describe the appearance of a docked interface item.
28. What is the purpose of a multiple document interface?
29. Which dialog box in Inventor allows you to control general program settings and
preferences that are not specific to a particular model or file, and how can you
access this dialog box?
30. How can you access the extensive Inventor help file system and learning resources?
30 Inventor and Its Applications 2009

Problems
Launch Inventor and complete the activities described in each problem. When you are finished,
continue working with Inventor or exit if necessary.
1. Perform the following tasks:
A. Begin a new Inventor file of your choice.
B. Explore the Inventor pull-down menu system by picking any of the menu
titles and moving the cursor down and up through the menu options.
C. Pick the File pull-down menu and highlight the New... option. Notice the help
string displayed in the status bar.
D. Pick the Open... option on the File pull-down menu to display the Open
dialog box.
E. Pick the Cancel button to close the Open dialog box.
F. Explore cascading submenus by highlighting the Toolbar option on the View
pull-down menu.
G. Press the [Esc] key or pick outside of the menu to close the View pulldown
menu.
2. Perform the following tasks:
A. Begin a new Inventor part file and explore the default part interface.
B. Close the part file without saving.
C. Begin a new Inventor assembly file and explore the default assembly interface.
D. Close the assembly file without saving.
E. Begin a new Inventor drawing file and explore the default drawing interface.
F. Close the drawing file without saving.
G. Begin a new Inventor presentation file and explore the default presentation
interface.
H. Close the presentation file without saving.
3. Perform the following tasks:
A. Open blade_main.ipt from the following folder: Autodesk/Inventor 2009/Samples/
Models/Assemblies/Scissors/ Components
Locate and explore the panel bar.
B. Pick the panel bar title, Part Features, and deselect the Display Text with Icons
option. Observe the changes in the panel bar. Pick the panel bar title again
and select Display Text with Icons to show the text once again.
C. Locate and explore the default browser.
D. Drag the End of Part indicator up and above Sketch4 and notice the changes.
E. Pick the Expand [+] button to the left of the Origin folder to expand all children.
F. Right-click on the Origin folder and select Collapse All Children.
G. Close blade_main.ipt without saving.
4. Perform the following tasks:
A. Begin a new Inventor part file.
B. Locate and explore the Inventor Standard toolbar.
C. Select Toolbars > Inventor Precise Input to open the Inventor Precise Input
toolbar, and dock the toolbar by double-clicking its name.
D. Place the cursor over several toolbar buttons and observe the tooltip and help
strings provided.
E. Pick one of the flyout buttons located in the Inventor Standard toolbar, select one
of the flyout options to initiate a tool, and modify the flyout button displayed.
Chapter 1 Introduction to Autodesk Inventor 31
Basic
Basic
Medium
Medium
Drawing Problems - Chapter 1
Drawing Problems - Chapter 1
Medium
Advanced
Advanced
Advanced
5. Write a brief description of the Inventor interface. Include answers to the following
questions: What is an interface? What are the primary Inventor interface items,
and how do they function? Reflect on the concept of a computer software interface.
Are some of the Inventor interface items similar to those in other programs
you have used? Submit a hard copy of your description to your drafting instructor
or supervisor.
6. Write a short description of each of the four Inventor file types. Include information
about file extensions and the circumstances in which each file type should
be used. Reflect on the capabilities of Inventor. How is Inventor similar and
different from other CADD programs you may have used? Submit a hard copy
of your description to your drafting instructor or supervisor.
7. Write a brief report on each part model element and the importance of constraints
and parametric associations in parametric solid modeling. Reflect on your understanding
of parametric modeling, and describe your experience with working
in parametric situations. Submit a hard copy of your report to your drafting
instructor or supervisor.
8. Create a new part file and draw a freehand sketch of the standard Inventor
screen display. Label each of the screen areas and the interface items described
in this chapter.
32 Inventor and Its Applications 2009