Autodesk Inventor 2010
Getting Started
January 2009Part No. 527B1-050000-PM01A
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Contents
Chapter 1 Digital Prototypes in Autodesk Inventor . . . . . . . . . . . . . . 1
Digital Prototype Workflow . . . . . . . . . . . . . . . . . . . . . . . . 1
Components of Digital Prototypes (file types) . . . . . . . . . . . . . . . 3
Associative Behavior of Parts . . . . . . . . . . . . . . . . . . . . . 7
Associative Behavior of Assemblies . . . . . . . . . . . . . . . . . . 7
Associative Behavior of Drawings . . . . . . . . . . . . . . . . . . 8
Chapter 2 Create Digital Prototypes . . . . . . . . . . . . . . . . . . . . . 9
Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9
Single Body Parts . . . . . . . . . . . . . . . . . . . . . . . . . . 10
iParts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10
Sheet Metal Parts . . . . . . . . . . . . . . . . . . . . . . . . . . 11
Derived Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13
Multi-body Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . 14
Shrinkwrap Parts . . . . . . . . . . . . . . . . . . . . . . . . . . 14
Assembly Substitute Parts . . . . . . . . . . . . . . . . . . . . . . 15
Content Center Parts . . . . . . . . . . . . . . . . . . . . . . . . 16
Content Center Libraries . . . . . . . . . . . . . . . . . . . 18
Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18
Sketched Features . . . . . . . . . . . . . . . . . . . . . . . . . . 19
Sketch Environment . . . . . . . . . . . . . . . . . . . . . 23
Sketch Blocks . . . . . . . . . . . . . . . . . . . . . . . . . 24
Sketch Constraints . . . . . . . . . . . . . . . . . . . . . . 25
iii
2D AutoCAD Data in Sketches . . . . . . . . . . . . . . . . 25
Placed Features . . . . . . . . . . . . . . . . . . . . . . . . . . . 26
iFeatures . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 27
Assembly Features . . . . . . . . . . . . . . . . . . . . . . . . . . 27
Work Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28
Edit Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 29
Assemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 29
Place Components . . . . . . . . . . . . . . . . . . . . . . . . . 30
Drag Components into Assemblies . . . . . . . . . . . . . . 31
Assembly Constraints . . . . . . . . . . . . . . . . . . . . . . . . 31
Degrees of Freedom . . . . . . . . . . . . . . . . . . . . . . 32
Top-down Design . . . . . . . . . . . . . . . . . . . . . . . . . . 33
Create Subassemblies In-place . . . . . . . . . . . . . . . . . . . 33
Design Accelerator Components . . . . . . . . . . . . . . . . . . 34
Design Mechanisms . . . . . . . . . . . . . . . . . . . . . . . . . 35
Check for Interference . . . . . . . . . . . . . . . . . . . . . . . 37
iAssemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 38
Chapter 3 Document and Publish Designs . . . . . . . . . . . . . . . . . . 39
Drawings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39
Start Drawings . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39
Types of Drawing Files . . . . . . . . . . . . . . . . . . . . . . . 40
Create Views of Models . . . . . . . . . . . . . . . . . . . . . . . 41
Types of Drawing Views . . . . . . . . . . . . . . . . . . . . 41
Drawing View Operations . . . . . . . . . . . . . . . . . . . 43
Drawing View Tips . . . . . . . . . . . . . . . . . . . . . . 44
Exploded Views . . . . . . . . . . . . . . . . . . . . . . . . . . . 45
Annotate Drawing Views . . . . . . . . . . . . . . . . . . . . . . 45
Types of Drawing Annotations . . . . . . . . . . . . . . . . 46
Styles and Standards . . . . . . . . . . . . . . . . . . . . . . . . 50
Studio in Autodesk Inventor . . . . . . . . . . . . . . . . . . . . . . . 51
Publish Designs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 53
Chapter 4 Manage Data . . . . . . . . . . . . . . . . . . . . . . . . . . . 55
Share Files in Work Groups Using Vault . . . . . . . . . . . . . . . . . 55
Autodesk Vault Add-ins for Design Applications . . . . . . . . . . 56
Microsoft Office Add-ins . . . . . . . . . . . . . . . . . . . . . . 57
Copy Designs Using Vault . . . . . . . . . . . . . . . . . . . . . 57
Share Files Externally . . . . . . . . . . . . . . . . . . . . . . . . . . . 57
Autodesk Vault Manufacturing . . . . . . . . . . . . . . . . . . . 58
Autodesk Design Review . . . . . . . . . . . . . . . . . . . . . . 58
Import and Export Data . . . . . . . . . . . . . . . . . . . . . . . . . . 59
AutoCAD Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . 59
Import Files from Other CAD Systems . . . . . . . . . . . . . . . 61
Export Files to Other CAD System Formats . . . . . . . . . . . . . 62
iv | Contents
Chapter 5 Set Your Environment . . . . . . . . . . . . . . . . . . . . . . . 63
Commands and Tools . . . . . . . . . . . . . . . . . . . . . . . . . . . 63
Environment Preferences . . . . . . . . . . . . . . . . . . . . . . . . . 65
Application Options . . . . . . . . . . . . . . . . . . . . . . . . . 65
Document Settings . . . . . . . . . . . . . . . . . . . . . . . . . 65
Styles and Standards . . . . . . . . . . . . . . . . . . . . . . . . . . . . 65
Style Libraries . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66
Views of Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66
Templates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 67
Projects . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 68
Vault Projects . . . . . . . . . . . . . . . . . . . . . . . . . . . . 69
Default Projects . . . . . . . . . . . . . . . . . . . . . . . . . . . 70
New Projects . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 70
Learning Resources . . . . . . . . . . . . . . . . . . . . . . . . . . . . 71
New Features Workshop . . . . . . . . . . . . . . . . . . . . . . . 71
Integrated Help . . . . . . . . . . . . . . . . . . . . . . . . . . . 71
Tutorials . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 72
Skill Builders . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 73
Index . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 75
Contents | v
vi
Digital Prototypes in Autodesk Inventor
Autodesk Inventor® provides a comprehensive set of 3D mechanical CAD tools for producing,
validating, and documenting complete digital prototypes. The Inventor model is a 3D digital
prototype. The prototype helps you visualize, simulate, and analyze how a product or part
works under real-world conditions before it is built. Manufacturers get to market faster with
fewer physical prototypes and more innovative products.
Inventor provides an intuitive 3D design environment for creating parts and assemblies.
Engineers can focus on the function of a design to drive the automatic creation of intelligent
components, such as steel frames, rotating machinery, tube and pipe runs, electrical cables,
and wire harnesses.
Tightly integrated motion simulation and stress analysis in Inventor are easy to use. They
make it possible for engineers to optimize and validate the digital prototype.
Generating manufacturing documentation from a validated 3D digital prototype reduces
errors and associated engineering change orders (ECOs) before manufacturing. Inventor offers
rapid and accurate output of production-ready drawings directly from the 3D model.
Inventor is tightly integrated with Autodesk® data management applications. This integration
enables the efficient and secure exchange of digital design data and promotes earlier
collaboration between design and manufacturing workgroups. Different workgroups can
manage and track all components of a digital prototype with Autodesk® Design Review
software. This software is the all-digital way to review, measure, mark up, and track changes
to designs. You can better reuse crucial design data, manage bills of materials (BOMs), and
collaborate with other teams and partners.
1
Digital Prototype Workflow
Before you start a design, determine the most efficient workflow. A top down
workflow is often the most efficient way to create a design. In a top down
1
workflow, you design your components in the context of other components.
This method can greatly reduce errors in form, fit, and function.
Some examples of a top-down workflow are:
■ Create new parts or sub-assemblies in the destination assembly.
■ Create multiple solid bodies in a part file and then save the individual
bodies as unique parts.
■ Create 2D sketch blocks in a part file to simulate a mechanism. You can
use the sketch blocks to create 3D components in an assembly that is
controlled by the layout.
Following are questions to consider before you start:
■ Which view of the part best describes the basic shape?
■ Is the part a sheet metal part?
■ Can this part be used as a part factory (iPart) to generate multiple parts?
■ Can a spreadsheet control one or more parts?
■ Can I create the part automatically by using a Design Accelerator?
■ If the part is a component in a structural steel frame, can I use Frame
Generator to create the entire frame?
■ If the part is a common library part, does it exist in the Content Center or
other library?
The following image shows a multi-body part file saved as individual parts in
an assembly. Individual bodies in a multi-body part file can share features
with other bodies such as fillets and holes.
2 | Chapter 1 Digital Prototypes in Autodesk Inventor
LocationFor more information
Search: “Multi-body parts”Help topic
Parts 1 - Create PartsTutorial
PartsSkill Builders
Components of Digital Prototypes (file types)
Create or activate a project file before you open an existing file or start a new
file to set the file location. Click New to see the New File dialog box with
templates for a new part, assembly, presentation file, sheet metal part,
weldment, or drawing. You can choose from several templates with predefined
units.
A template can contain property information, such as part and project data,
and drawing views. You can see information stored in a file by viewing its
properties.
For more information about templates, see Templates on page 67. For more
information about projects, see Projects on page 68.
For more information about projects, see Projects on page 68.
Components of Digital Prototypes (file types) | 3
Part (.ipt) Files
When you open a part file, you are in the part environment. Part tools
manipulate sketches, features, and bodies which combine to make parts. You
can insert a single body part into assemblies and constrain them in positions
they occupy when the assembly is manufactured. You can extract multiple
part files from a multi-body part.
Most parts start with a sketch. A sketch is the profile of a feature and any
geometry (such as a sweep path or axis of rotation) required to create the
feature.
A part model is a collection of features. If necessary, solid bodies in a
multi-body part file can share features. Sketch constraints control geometric
relationships such as parallel and perpendicular. Dimensions control the size.
Collectively this method is called Parametric modeling. You can adjust the
constraints or dimensional parameters that control the size and shape of a
model, and automatically see the effect of your modifications.
The following image shows a single body part in the upper half of the image,
and a multi-body part in the lower half of the image. Notice the different part
icons in each image.
Assembly (.iam) Files
In Autodesk Inventor, you place components that act as a single functional
unit into an assembly document. Assembly constraints define the relative
position these components occupy with respect to each other. An example is
the axis of a shaft aligning with a hole in a different component.
4 | Chapter 1 Digital Prototypes in Autodesk Inventor
When you create or open an assembly file, you are in the assembly
environment. Assembly tools manipulate whole subassemblies and assemblies.
You can group parts that function together as a single unit and then insert
the subassembly into another assembly.
You can insert parts into an assembly or use sketch and part tools to create
parts in the context of an assembly. During these operations, all other
components in the assembly are visible.
To complete a model, you can create assembly features that affect multiple
components, such as holes that pass through multiple parts. Assembly features
often describe specific manufacturing processes such as post-machining.
The assembly browser is a convenient way to activate components you want
to edit. Use the browser to edit sketches, features, and constraints, turn
component visibility on and off, and do other tasks. In the following image
of an assembly, two of the components display an icon indicating they are
part of a contact set. Components that belong to a contact set behave as they
would in the physical world.
Presentation (.ipn) Files
Presentation files are a multi-purpose file type. Use a presentation file to:
■ Create an exploded view of an assembly to use in a drawing file.
■ Create an animation which shows the step by step assembly order. The
animation can contain view changes and the visibility state of components
at each step in the assembly process. You can save the animation to a .wmv
or .avi file format.
Components of Digital Prototypes (file types) | 5
Drawing (.idw, .dwg) Files
After you create a model, you can create a drawing to document your design.
In a drawing, you place views of a model on one or more drawing sheets. Then
you add dimensions and other drawing annotations to document the model.
A drawing that documents an assembly can contain an automated parts list
and item balloons in addition to the required views.
The templates to use as the starting point for your drawings have the standard
drawing file extension (.idw, .dwg).
6 | Chapter 1 Digital Prototypes in Autodesk Inventor
Autodesk Inventor maintains links between components and drawings, so
you can create a drawing at any time during the creation of a component. By
default, the drawing updates automatically when you edit the component.
However, it is a good idea to wait until a component design is nearly complete
before you create a drawing. Edit the drawing details (to add or delete
dimensions or views, or to change the locations of notes and balloons) to
reflect the revisions.
LocationFor more information
Help topic
Guide
Search:
“Autodesk Inventor file types”
“Set file names”
Manual in PDF format.Autodesk Vault Implementation
Associative Behavior of Parts
Other than the origin work planes, work axes, the center point, and grounded
work points, all work features are associated to the features or geometry used
to create them. If you modify or delete the locating geometry, the work feature
changes accordingly. Conversely, changes to the work feature affect any feature
or geometry that is dependent on a work feature for its definition.
A parent-child relationship is a term frequently used to describe the
relationship between features. A child feature cannot exist without the parent
feature. If you delete a parent feature, you can choose to retain the originating
sketch of a child feature. If you create geometry on an origin plane or a work
plane created from an origin plane you can often avoid creating parent-child
relationships.
A derived part can maintain associative links to the source component so it
can be updated. You can also choose to break the link between the derived
part and the source part or assembly to disable updates.
For more information about derived parts and work features, see Parts on page
9 and Features on page 18.
Associative Behavior of Assemblies
An assembly maintains active links to the source components. Each time you
open an assembly, Inventor detects the latest version of the components
Associative Behavior of Parts | 7
contained in the assembly. When you open an assembly file in which one or
more components are modified, a message displays asking if you want to
update the assembly. Answer yes to update the assembly to the last saved state
of the components. Answer no to disregard any modifications to the referenced
components.
Associative Behavior of Drawings
Drawings maintain associativity to the components contained in the file views.
If you change a component, the component view automatically updates the
next time the drawing file is opened. You can choose to disable automatic
updates by enabling Defer Updates in the Drawing tab of Document Settings.
If the drawing contains a parts list and item balloons, the balloon numbers
are associative to the item numbers in the parts list. The parts list is also
associative to the Bill of Materials in the source assembly. If items are deleted
from the assembly, they are no longer contained in the drawing parts list. The
parts list is associative to the iProperties of the components being detailed for
entries such as part number and description.
LocationFor more information
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Search:
“3D modeling concepts”
“2D to 3D bidirectional associativity”
“Assembly components in patterns”
“Design view representations in drawings”
8 | Chapter 1 Digital Prototypes in Autodesk Inventor
Create Digital Prototypes
2
Traditionally, designers and engineers create a layout, design the parts, and then bring
everything together in an assembly. Once the design is created, the next step in the traditional
process is to build and test a physical prototype.
NOTE This chapter describes how to create digital prototypes in Inventor LT
With Autodesk Inventor®, you can create an assembly at any point in the design process. You
can virtually explore, test, and validate a digital prototype as the design evolves. You can
visualize and simulate real-world performance of the design, so there is less reliance on costly
physical prototypes.
The basic component of a digital prototype is the part file. A part model is a collection of
features or solid bodies that define your digital prototype. Parametric modeling provides the
ability to apply driving dimensions and geometric relationships to the model. These dimensions
and relationships are called parameters. Parameters control the size and shape of a model.
When you change a parameter, the model updates to reflect the changes. Using parameters,
you can control multiple parts in an assembly.
Parts
A file with an .ipt extension represents a part file. A part is represented on disk
with only one file type. However, there are many different types of part files.
They can be simple to complex. Some of the common types of parts are
explained in the following section. The workflow you use to create the part is
what determines the part type.
9
Single Body Parts
The most basic part type can vary greatly in complexity from just a few features
to a complex design. The distinguishing features are that it is composed of
one material and one solid body, of which the thickness can vary.
A single body part contains one solid body that shares
a collection of one or more features. A single body part
defines a single item in a parts list.
LocationFor more information
iParts
Help topics
Search:
“Create parts in assemblies”
“Work with parts”
Parts 1 - Create PartsTutorial
Most designers have parts that differ by size, material, or other variables, but
the same basic design works in many models.
An iPart is a table driven master part that
configures standard parts to different sizes
and states. The table can be edited within
Inventor or externally in a spreadsheet.
Each row can control feature state (enabled or suppressed), and many other
variables such as feature size, color, material, and part number. Table driven iFeatures can also be included in an iPart
table.
10 | Chapter 2 Create Digital Prototypes
An iPart typically generates multiple
unique parts that belong to the same
family.
NOTE You can create an iPart and save
it as a table-driven iFeature.
Use the iPart Author to create the part family members in each table row.
When placing the part in an assembly, select a row (member) to generate a
unique part.
LocationFor more information
Search: “iPart Fundamentals”Help topic
Skill Builder
Sheet Metal Parts
Within the Autodesk Inventor design environment, a sheet metal part can be
displayed as a folded model or a flat pattern. With sheet metal commands,
you can unfold features and work on a model in a flattened state, and then
refold the features.
You create sheet metal parts from a template file. The sheet metal template
file incorporates a set of rules. The rules determine some common attributes
such as material type and thickness, unfolding rules, gap sizes, and so on. By
changing a single rule, you can change the material of a sheet metal part from
Parts:
iParts - The Basics
iParts - Beyond the Basics
Chances are that a design you have been asked to create
contains components that lend themselves to fabrication
from sheet metal.
Autodesk Inventor provides functionality that simplifies the
creation, editing, and documentation of digital prototypes
of sheet metal components.
A sheet metal part is often thought of as a part fabricated
from a sheet of uniformly thick material. If you design small
objects, this material is often thin. However, in Autodesk
Inventor you can utilize the sheet metal commands on any
design where the material is of uniform thickness.
Sheet Metal Parts | 11
aluminum to stainless steel. A change of material often requires changes to
the attributes that define bends and corners. Such changes often require
changes to shop floor machinery and set-ups used to fabricate the parts.
Like other parts created within Autodesk Inventor, sheet metal parts begin
with a base feature. The base feature of a sheet metal part is often a single face
of some shape to which other features (often flanges) are added. A complex
design could use a contour flange or contour roll as the initial base feature.
Some parts could utilize a lofted flange as the initial feature.
Unlike regular parts, sheet metal parts are always created from a uniformly
thick sheet that is flat. This sheet is formed into the final part using various
fabrication techniques. In the sheet metal environment, you can create a
folded model and unfold it into a flat pattern. The flat pattern is typically
used to detail the fabrication. The sheet metal commands you use to work
with flat patterns can provide critical fabrication information.
If a regular part created in Autodesk Inventor is of a consistent thickness, you
can convert it to a sheet metal part. The same is true for parts imported from
other systems.
LocationFor more information
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Skill Builders
Search:
“Sheet Metal Defaults”
“Templates for sheet metal parts”
Build sheet metal partsTutorial
Parts:
Sheet Metal Punch iFeatures - part 1
Sheet Metal Punch iFeatures - part 2
12 | Chapter 2 Create Digital Prototypes
Derived Parts
A derived part can contain features independent of the parent component,
and can be:
■ Driven by the original component or the link can be disabled.
■ Used for scaling and mirror operations.
■ Derived from a specific assembly Level of Detail.
■ Used to perform add and subtract operations on assembly components.
A derived part is a new part or body created from an
existing part or assembly.
Use Derived Component to:
■ Create modified or simplified versions of other
components.
■ In an empty part file, create a derived part from
another part or assembly.
■ In a multi-body part, insert components as toolbodies.
■ Mirror or scale a part or assembly
■ Perform Boolean operations.
■ An existing component inserted as a new toolbody in a multi-body part
file.
LocationFor more information
Help topics
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“Derived parts and assemblies”
“Derived parts”
Create Parts from Derived GeometryTutorial
Parts - Derived PartsSkill Builder
Derived Parts | 13
Multi-body Parts
Shrinkwrap Parts
A shrinkwrap part uses the derived component mechanism to create a
simplified part file from an assembly. The Shrinkwrap command uses rule
based face and component removal and hole patching to simplify an assembly.
A shrinkwrap surface composite (the default setting) uses less memory and
Multi-body parts are used to control complex curves across
multiple parts in plastic part design or organic models.
A multi-body part is a central design composed of features
contained in bodies that can be exported as individual part
files.
You can insert components into a multi-body part file with
the Derived Component command. Use the Combine
command to perform Boolean operations.
LocationFor more information
Search: “Combine solid bodies”Help topic
Explore Multi-Bodies and Plastic FeaturesTutorial
14 | Chapter 2 Create Digital Prototypes
provides the best performance when used as a substitute LOD in consuming
assemblies.
Use Shrinkwrap to:
■ Create an envelope of an assembly to provide
information to an outside group such as AEC.
■ Create a part that uses less memory and provides
better performance in consuming assemblies.
■ Create a part that protects intellectual property
by concealing holes and components.
■ Create a simplified part to use as a substitute LOD
in the owning assembly.
NOTE A shrinkwrap part is created from an assembly
to remove parts and small features from the assembly.
Use a shrinkwrap part to simplify a design or protect
intellectual property.
LocationFor more information
Search: “Shrinkwrap assemblies”Help topic
Assembly Substitute Parts
An assembly substitute part is a simplified representation of an assembly. It
can be created from any part file on disk, or derived in place in the owning
assembly. You can create a shrinkwrap substitute part in an assembly to reduce
file size and complexity.
Assembly Substitute Parts | 15
Content Center Parts
Autodesk Inventor Content Center libraries provide standard parts (fasteners,
steel shapes, shaft parts) and features to insert in assemblies.
Two types of parts are included in the Content Center library: standard parts
and custom parts. Standard parts (fasteners, shaft parts) have all part parameters
defined as exact values in the table of parameters. Custom parts (steel shapes,
rivets) have a parameter set arbitrarily within the defined range of values.
LocationFor more information
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The basic component in a Content Center library is a family (part
family or feature family). A family contains family members that
16 | Chapter 2 Create Digital Prototypes
have the same template and family properties, and represent
size variations of a part or feature.
Families are arranged in categories and subcategories. A
category is a logical grouping of part types. For example, studs and hex head
bolts are functionally related
and are nested under the
Bolts category. A category
can contain subcategories
and families.
Use the Content Center environment to work with Content Center library
parts in the design process.
■ Open and view a part family, and choose the family member.
■ Insert a part from Content Center library into an assembly file.
■ Insert a feature from Content Center library in a part.
■ Use AutoDrop to place a part interactively from a Content Center library
into an assembly file.
■ Change the size of a placed Content Center library part.
■ Replace an existing (also non-Content Center) part with a part from the
Content Center library.
LocationFor more information
Search: “Content Center Environment”Help topic
Use Content CenterTutorial
Content CenterSkill Builders
Content Center Parts | 17
Content Center Libraries
Content Center libraries contain data required to create part files for Content
Center library parts. The data are:
■ Parametric .ipt files which provide models for Content Center library parts.
■ Family tables which include values of part parameters.
■ Descriptions for parts including family properties such as family name,
description, standard, and standard organization.
■ Preview pictures displayed in the Content Center.
Parametric .ipt files, description texts, and preview pictures are common for
all members of one family. Sets of parameter values specify particular family
members.
A set of standard Content Center libraries can be installed with Autodesk
Inventor. Standard libraries are read-only and cannot be edited directly. You
must copy parts to the read/write library first.
Use the Content Center Editor to build user libraries and to modify or expand
standard content delivered with the Autodesk Inventor installation.
LocationFor more information
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Features
The building blocks of a part model are called features. There are four basic
types of Features:
■ Sketched Features that require a sketch.
■ Placed Features that modify existing geometry. For example, a hole is a
placed feature.
■ Work Features used for construction purposes.
■ iFeatures that represent common shapes and are saved in a reusable library.
An iFeature driven by a table can represent different shape configurations.
18 | Chapter 2 Create Digital Prototypes
Content Center User LibrariesTutorial
You can create surfaces with many of these operations to define shapes or
aspects of the part body. For example, you can use a curved surface as a
termination plane for cuts in a housing.
You can edit the characteristics of a feature by returning to its underlying
sketch or changing the values used in feature creation. For example, you can
change the length of an extruded feature by entering a new value for the
extent of the extrusion. You can also use equations to derive one dimension
from another.
Sketched Features
Most parts start with a sketch. A sketch is the profile of a feature and any
geometry (such as a sweep path or axis of rotation) required to create the
feature. Your first sketch for a part can be a simple shape.
Sketched part features depend on sketch geometry. The first feature of a part,
the base feature, is typically a sketched feature. All sketch geometry is created
and edited in the sketch environment, using Sketch commands on the ribbon.
You can control the sketch grid, and use sketch commands to draw lines,
splines, circles, ellipses, arcs, rectangles, polygons, or points.
LocationFor more information
Search: “Adaptive features, parts, and subassemblies”Help topics
Create and Reuse iFeaturesTutorial
You can select a face on an existing part, and sketch on it. The sketch displays
with the Cartesian grid defined. If you want to construct a feature on a curved
surface, or at an angle to a surface, first construct a work plane. Then sketch
on the work plane.
The browser displays the part icon, with its features nested under it. Surface
features and work features are nested or consumed by default. To control
nesting, or consumption of surface and work features for all features, set the
option on the Part tab of the Applications Options dialog box. To override
consumption on a per-feature basis, right-click the feature in the browser, and
then select Consume Inputs.
Sketched Features | 19
The following features are dependent on a sketch you create:
Extrude
Adds depth to a sketch profile along
a straight path.
Can create a body.
Revolve
Projects a sketch profile around an axis.
The axis and the profile must be coplanar.
Can create a body.
Loft
Constructs features with two or more
profiles.
.
Transitions the model from one shape
to the next.
Aligns the profiles to one or more
paths.
Can create a body.
20 | Chapter 2 Create Digital Prototypes
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