Autodesk Inventor 2010 Getting Started Part No.
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Contents Chapter 1 Digital Prototypes in Autodesk Inventor . . . . . . . . . . . . . . 1 Digital Prototype Workflow . . . . . . . . . . Components of Digital Prototypes (file types) . Associative Behavior of Parts . . . . . . . Associative Behavior of Assemblies . . . . Associative Behavior of Drawings . . . . Chapter 2 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .1 .3 .7 .7 .8 Create Digital Prototypes .
2D AutoCAD Data in Sketches . . . Placed Features . . . . . . . . . . . . . . iFeatures . . . . . . . . . . . . . . . . . . Assembly Features . . . . . . . . . . . . . Work Features . . . . . . . . . . . . . . . Edit Features . . . . . . . . . . . . . . . . Assemblies . . . . . . . . . . . . . . . . . . . . Place Components . . . . . . . . . . . . Drag Components into Assemblies . Assembly Constraints . . . . . . . . . . . Degrees of Freedom . . . . . . . . . Top-down Design . . . . . . . . . . . . .
Chapter 5 Set Your Environment . . . . . . . . . . . . . . . . . . . . . . . 63 Commands and Tools . . . . . Environment Preferences . . . Application Options . . . Document Settings . . . Styles and Standards . . . . . . Style Libraries . . . . . . Views of Models . . . . . . . . Templates . . . . . . . . . . . Projects . . . . . . . . . . . . Vault Projects . . . . . . Default Projects . . . . . New Projects . . . . . . . Learning Resources . . . . . . New Features Workshop . Integrated Help . . . . .
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Digital Prototypes in Autodesk Inventor 1 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.
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.
For more information Location Help topic Search: “Multi-body parts” Tutorial Parts 1 - Create Parts Skill Builders Parts 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.
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.
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.
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).
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.
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.
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.
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.
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.
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.
Derived Parts 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.
Multi-body Parts 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.
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.
For more information Location Help topic Search: “Create Substitutes” 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.
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.
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 .
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.
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.
Sweep Projects a single sketch profile along a single sketched path. The path can be open or closed. A sketch profile can contain multiple loops that reside in the same sketch. Can create a body. Coil Projects a sketch profile along a helical path. Use Coil to create springs or to model physical threads on a part. Can create a body. The models created by these operations are typically solid features or new bodies that form a closed volume. Surfaces You can create surfaces with many of these operations.
The following features require sketches, but do not create a base feature because they are dependent on existing geometry. Rib Creates a rib or web extrusion from a 2D sketch. Use Rib to create thin-walled closed support shapes (ribs) and thin-walled open support shapes webs. Emboss Creates a raised (emboss) or recessed (engrave) feature from a sketch profile.
Decal Applies an image file to a part face. Use decal to add realism or to apply a label. For more information Location Help topic Search: “Plan and create sketches” “Sketch properties” Tutorial Parts 1 - Create Parts Sketch Environment When you create or edit a sketch, you work in the sketch environment. The sketch environment consists of a sketch and sketch commands. The commands control the sketch grid and draw lines, splines, circles, ellipses, arcs, rectangles, polygons, or points.
sketch environment. You can create geometry for part features. The changes you make to a sketch are reflected in the model. For more information Location Help topic Search: “Sketch Environment” “Application Options settings > Part tab” “Application Options settings > Sketch tab” Tutorial Work with Sketch Blocks Sketch Blocks In many assembly designs, rigid shapes are repeated. You can use sketch blocks to capture such shapes as a fixed set, and place instances of the set where needed.
Sketch Constraints Constraints limit changes and define the shape of a sketch. For example, if a line is horizontally constrained, dragging an endpoint changes the length of the line or moves it vertically. However, the drag does not affect its slope. You can place geometric constraints between: ■ Two objects in the same sketch. ■ A sketch and geometry projected from an existing feature or a different sketch. As you sketch, constraints are automatically applied to the various sketch elements.
be converted. You can choose to import AutoCAD blocks as Autodesk Inventor sketch blocks. When you export Autodesk Inventor drawings to AutoCAD, the converter creates an editable AutoCAD drawing. All data is placed in paper space or model space in the DWG file. If the Autodesk Inventor drawing has multiple sheets, each is saved as a separate DWG file. The exported entities become AutoCAD entities, including dimensions. You can open a .
Dialog boxes define values for placed features, such as the Hole dialog box. iFeatures An iFeature is one or more features that you can save and reuse in other designs. You can create an iFeature from any sketched feature. Features dependent on the sketched feature are included in the iFeature. After you create an iFeature and store it in a catalog, you can drag it from Windows Explorer and drop it in the part file. You can also use the Insert iFeature command.
For more information Location Showme Show me how to create an assembly feature Work Features Work features are abstract construction geometry that you can use to create and position new features when other geometry is insufficient. To fix position and shape, constrain features to work features. Work features include work planes, work axes, and work points. The proper orientation and constraint conditions are inferred from the geometry you select and the order in which you select it.
Edit Features In the browser, right-click a feature, and then use one of several options on the menu to modify the feature: Show Dimensions Edit Sketch Displays the sketch dimensions so you can edit them. ■ Change the dimensions of a feature sketch. ■ Change, add, or delete constraints. Activates the sketch so it is available for edit. ■ Modify or create a new profile for the feature. After you modify a part sketch, exit the sketch and the part updates automatically.
of the assembly. In a typical modeling process, some component designs are known and some standard components are used. Create the designs to meet specific objectives. Place Components In the assembly environment, you can add existing parts and subassemblies to create assemblies, or you can create parts and subassemblies in-place. A component (a part or subassembly) can be an unconsumed sketch, a part, a surface, or any mixture of both.
When you create a component in the assembly context, the created component is nested under the active main assembly or subassembly in the browser. A sketch profile for the in-place component that uses projected loops from other components within the assembly, is associatively tied to the projecting components. Drag Components into Assemblies You can place multiple components in an assembly file in a single operation by dragging them into an open assembly window.
Degrees of Freedom Each unconstrained component in an assembly has six degrees of freedom (DOF). It can move along or rotate about each of the X, Y, and Z axes. The ability to move along X, Y, and Z axes is called translational freedom. The ability to rotate around the axes is called rotational freedom. Whenever you apply a constraint to a component in an assembly, you remove one or more degrees of freedom. A component is fully constrained when all degrees of freedom (DOF) are removed.
Top-down Design The top-down design technique (also known as skeletal modeling) centralizes control of your design. The technique enables you to update your design efficiently and with minimal disruption to your design documents. Top-down design begins with the layout. The layout is a 2D part sketch that is the root document of your design. You create a layout that represents your assembly, subassembly, floor plan, or equivalent.
When you create a component in-place, you can do one of the following: ■ Sketch on one of the assembly origin planes. ■ Click in empty space to set the sketch plane to the current camera plane. ■ Constrain a sketch to the face of an existing component. When you create a subassembly in place, you define an empty group of components. The new subassembly automatically becomes the active assembly, and you can start to populate it with placed and in-place components.
You insert components using Design Accelerator generators and calculators in the assembly environment. The generators and calculators are grouped according to functional areas. For example, all welds are together.
■ Create a Contact Set and add members as required to simulate physical contact between components and to determine the range of motion. ■ Use Positional representations to save a mechanism in various states such as maximum and minimum extension. ■ Use Inventor Studio to animate simultaneous or sequential movement.
■ Use the Dynamic Simulation Environment to calculate displacements, velocities, accelerations, and reaction forces without the cost of a physical prototype. ■ Use the Stress Analysis Environment to conduct structural static and modal stress analysis studies on the digital prototype.
iAssemblies An iAssembly is a configuration of a model with a few or many variations called members. Each member has a set of unique identifiers, such as diameter or length. A member could have different components, such as a power train for a vehicle with several different engine sizes. Create an iAssembly if you want to show different quantities for assembly components in a parts list. You can define the required parts list quantity for each iAssembly member. You can manage iAssemblies from a table.
Document and Publish Designs 3 During the process of creating digital prototypes in Inventor, there is often a need to communicate the design to individuals outside the design team. In Autodesk Inventor®, you can create the appropriate type of documentation for any consumer, such as customers or manufacturers.
number)\Templates folder. The available templates are presented in the tabs of the New File dialog box. Drawing templates can contain sheet formats, borders, title blocks, and sketched symbols. Templates also control the default styles and standards used for the appearance of views and annotations. When you start a drawing, the title block, border, sheet size, and other elements come from the template.
You can open them only in Inventor or Inventor View. This file type results in smaller file sizes. The DWG file type is native to AutoCAD®. You can open DWG files in AutoCAD, Inventor, or DWG TrueView. If you create data using Inventor in a DWG file, you can modify the data only with Inventor. If you create data using AutoCAD in a DWG file, you can modify the data only with AutoCAD. If a downstream consumer of your Inventor data needs a DWG file, consider using DWG files as the default in Inventor.
Projected View An orthographic or isometric view that is generated from a base view or other existing view. You can create multiple projected views in a single operation. The position of the cursor relative to the parent view determines the orientation of the projected view. Projected views inherit the scale and display settings from the parent view. Orthographic projected views keep alignment with the parent view. The active drafting standard defines the first-angle or third-angle projection.
Overlay View A single view that shows an assembly in multiple positions. Overlays are available for base, projected, and auxiliary views. The overlay view is created on top of the parent view. Draft View A view created from a 2D sketch in the drawing file. You can place a draft view and construct a drawing without an associated model. A draft view can provide detail that is missing in a model.
Crop An operation that provides control over the view boundary in an existing drawing view. The clipping boundary can be a rectangle or circle you create during the command, or a closed profile you select from a sketch. Slice An operation that produces a zero-depth section from an existing drawing view. You perform the Slice operation in a selected target view. The slice lines are defined in a sketch associated to a different view.
■ You can suppress views so that they do not display on the drawing sheet. Suppressed views are useful when one view is created only for creating a child view. The suppressed view can still be accessed in the browser. For more information Location Help topic Search: “Drawing views” Tutorial Prepare Final Drawings Skill Builders Drawings Exploded Views Exploded views are commonly used to describe assemblies by moving components out from their assembled position.
Types of Drawing Annotations General Dimensions You can create general dimensions in orthographic or isometric views. The geometry you select determines the dimension type and the options available in the right-click menu. You can override the dimension text, which does not affect the model geometry. You can change the dimension precision and tolerance, edit the leader and arrowheads, or modify the content of dimension text.
Center Marks Center marks are added to the selected arc or circle. Center mark extension lines are automatically sized to fit the geometry. Center marks can be added individually or using the automated centerlines command. Centerlines Creates centerlines for selected edges, at the midpoint for lines, or at the center point of arcs or circles. Creates a circular centerline when features form a circular pattern. Autodesk Inventor supports three types of centerlines: bisector, centered pattern, and axial.
User-defined or sketched symbols are defined in the Drawing Resources and are placed like standard symbols. They are used to define custom symbols that are not available in Autodesk Inventor. Bend Notes A bend not adds fabricating information to sheet metal bend, contour roll, and cosmetic centerlines. Bend notes can be added to flat pattern views of sheet metal parts. A bend note is associated with the selected bend centerline. The default placement of the bend note is above the selected bend centerline.
Balloons Balloons are annotation tags that identify items listed in a parts list. Balloons can be placed individually or automatically for all components in a drawing view. You can add balloons to a custom part after it is added to the parts list. The balloon shape and value can be overridden using Edit Balloon on the right-click menu. You can combine balloons to use a single leader using the attach balloon options on the right-click menu.
Revision Tables and Tags Revision tables include information about design changes. Revision tables can be created for the entire drawing file or a single sheet. A revision tag marks an object changed by design revisions. The default revision level for the tag is the latest revision in the table. The revision level of the tag can be changed using the right-click menu. Text or Leader Text Use the Text command to add general notes to a drawing.
■ You can store all or some of the style information in a drawing file or template instead of using the styles library. This method is useful when you make one-time overrides that you do not want to affect all drawings. ■ If a style is stored in a template, it is available only to future documents created with the template. Update manually the documents you created previously. With style libraries, a style definition is available in any document simply by refreshing the library.
Inventor Studio is a rendering and animation environment within Part and Assembly documents. You can produce both illustrative and realistic imagery of your part or assembly. Inventor Studio images can be used to document products, present concepts to investors, clients, or your management team. The images you create can be used in a wide variety of places within the corporate environment. In addition, you can provide animations of how your design works.
Publish Designs Digital prototype data can be published to various formats in Inventor. This data can include parts, assemblies, drawings, or a combination of these depending on the file type selected. To publish, use the Save Copy As command and select a file type, or use the various Export commands.
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Manage Data 4 Autodesk Inventor® provides various means to share files within your internal workgroups, and with team members outside your organization. You can import and export files from and into other CAD software, and you can share Inventor files with team members who do not use CAD software. Share Files in Work Groups Using Vault Autodesk® Vault is a work group data management system for sharing design data across a project team.
Design teams use Autodesk Vault for version control and to store and share all types of engineering files and related data. Files can be Autodesk Inventor, AutoCAD®, Autodesk® DWF™ (Design Web Format), FEA, CAM, or Microsoft® Office. They can be any other file used in the design process. All versions of files that are checked into the vault are retained, along with any file dependencies, providing a living history of the project.
Microsoft Office Add-ins The Microsoft Office Add-in performs basic vault functions on documents, spreadsheets, and other non-CAD data within any of these Microsoft Office applications: Word, Excel®, and PowerPoint®. Copy Designs Using Vault The Copy Design function in Autodesk Vault copies an Inventor design with all related files to create another design. Use Copy Design to copy an entire assembly structure, including all related 2D drawings and 3D models, to derive a new design.
Autodesk Vault Manufacturing Vault Manufacturing is a product data management (PDM) application that provides a modular and practical approach to controlling your design data. It bridges the gap between CAD data and the manufacturing process. You can: ■ Track the life cycle of designs and materials used to manufacture a product. ■ Manage what you make, buy, assemble, and deliver to customers. Vault Manufacturing automates the process of tracking and managing the engineering release process.
For more information Location Web links autodesk.com/designreview dwfcommunity.autodesk.com Import and Export Data To translate files, you open or import the files in Autodesk Inventor. You can also place part and assembly files as components in Autodesk Inventor assemblies and drag and drop part and assembly files into Autodesk Inventor. In the open, import, and place components workflows, you can choose from specific import options to achieve the intended results.
You can export Autodesk Inventor drawings to AutoCAD. The converter creates an editable AutoCAD drawing and places all data in paper space or model space in the DWG file. If the Autodesk Inventor drawing has multiple sheets, each is saved as a separate DWG file. The exported entities become AutoCAD entities, including dimensions. You can open a DWG file and then copy selected AutoCAD data to the clipboard and paste into a part, assembly, or drawing sketch. The data is imported at the cursor position.
Import Files from Other CAD Systems You can import part and assembly files from other CAD systems. The import operation does not maintain associativity with the original file, except when you associatively import Alias files. After you import the files, you can treat them as if they were originally created in Autodesk Inventor.
Export Files to Other CAD System Formats You can export Autodesk Inventor parts, assemblies, and more to other CAD system formats. The export operation does not maintain associativity with the original Autodesk Inventor file. You can export these files: ■ CATIA V5 ■ JT ■ Pro/ENGINEER® ■ Parasolid® You can also export to SAT, STEP, IGES, DWF, and various graphic files formats.
Set Your Environment 5 The basics in this manual get you started using the Autodesk Inventor® software. References in For More Information tables throughout the manual guide you to Help topics, tutorials, and other resources that contain detailed information and specific instructions. Find out more within books about Autodesk Inventor, online resources of other Autodesk Inventor users, and the Autodesk® Newsgroup at http://discussion.autodesk.com.
The arrows on some of the commands and panel name bars reveal more options. The display of commands on the ribbon changes as you open and work in different types of files. Commands that are not accessible are shown as shaded, and you cannot select them. Purpose or task drives the environments within Autodesk Inventor. The components of each environment are consistent in their placement and organization, including points of access for entry and exit.
Environment Preferences The options you select on the Application Options and Document Settings dialog boxes control the display of the environment. Access to the dialog boxes is on the Tools tab, Options panel. Application Options The settings in the Application Options dialog box control the look and feel of Autodesk Inventor. Various tabs control the color of your display, the behavior and settings of files, the default file locations, and various multiple-user functions.
enough to get you started. Use the Style and Standard Editor to customize styles. By default, actions such as creating or modifying styles affect only the current document. You can choose to save the style to the style library, a master library that contains definitions for all available styles associated with a drafting standard. Usually, a CAD administrator manages the style library.
When ViewCube and NavBar are selected, they display in the upper right corner of the graphics window. The NavBar contains the basic view commands. For more information Location Help topics Search: “Overview of the ViewCube” “Navigation Tools” “Views of models” Templates Once you activate Autodesk Inventor, you can open an existing file or start a new file. Templates are available on the Application menu under New. You can choose from several templates with predefined units.
Templates are stored in the following directories in the English or Metric subdirectories. ■ Windows® XP: Autodesk\Inventor(version number)\Templates ■ Windows Vista®: C:\Users\Public\Documents\Autodesk\Inventor(version number)\Templates Subdirectories in the Templates directory are displayed as tabs in the Open New File dialog box. You can create and save custom templates in the Templates directory..
Vault Projects We recommend that you use Vault projects to collaborate on projects with multiple designers. Common files are stored in a vault and are never accessed directly. Each designer has a personal project that defines where the files are copied for viewing and editing. The vault also maintains version history of files as well as additional attributes. To use the vault project, Autodesk Vault software must be installed. A different dialog box opens so that you can create a Vault project.
■ Autodesk Vault maintains copies of all of the previous checked-in versions of data files. It stores additions about edit history, file properties, and file dependencies in its database. ■ You can set up queries on file properties, track file references, and retrieve past configurations. For a vault project, create a workspace at a path relative to the project file folder (such as .\ or .\workspace), and no other editable locations.
Workspace locations One defined at .\ One defined at .\ Workgroup locations None None Libraries One or more One or more not nested under workspace The default projects folder location is My Documents/Inventor, but you can change it to a different location.
Tutorials The tutorials you link to from the Help home page and the Get Started tab are a comprehensive set of hands-on lessons. The tutorial set is organized into three categories: fundamental, general interest, and specific interest. You can learn to be productive quickly, whether you are new to Autodesk Inventor or transitioning from AutoCAD.
Skill Builders Skill Builders help you sharpen your skills in various specific areas of functionality. Use the link on the Help home page to navigate to the Skill Builders Web page.
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Index A add-ins for design applications 56 for Microsoft Office 57 Analyze Interference tool 37 analyzing interference 37 animations 52 annotations in drawing views 45 assemblies 30 associative behavior 7 components 34 features 27 files 4 interference, checking 37 rendering and animating 52 subassemblies 34 associative behaviors 7 AutoCAD files 25, 59 Autodesk Design Review 1, 58 auxiliary views 42 D B balloons 6, 49 base views 41 baseline dimensions 46 bend notes 48 bend tables 49 bills of materials (BOM
Interference Detected 37 iPart Author 11 Open New File 68 Project Editor 68 Style and Standard Editor 65 digital prototypes 1, 9 publishing 53 workflow 1 dimensions in drawings 46 documenting designs 39, 52 DOF (degrees of freedom) 32 draft views 43 drafting standards 50 dragging components 31 drawing files 6 drawing views 41 annotating 45 operations 43 tips 44 types 41 drawings 6–7, 39 associative behavior 8 exporting to AutoCAD 60 file types 40 mark up 58 tables 49 templates 40 views 41 DWG files 40 F E
L leader text in drawings libraries of parts 18 lofted features 20 50 M mark up designs and drawings mirror features 26 model dimensions in drawings multi-body parts 14 58 46 N New Features Workshop notes in drawings 50 71 O Open New File dialog box options in projects 68 ordinate dimensions 46 overlay views 43 68 P part models 4 creating 3 modifying 29 templates 68 parts 9 assembly substitute 15 derived 13 envelope 15 features 18 multi-body 14 rendering 52 sheet metal 11 shrinkwrap 14 single body 1
table driven parts 10 templates 67 drawing files 40 new files 3 thread features 26 thread notes 47 top-down design 33 translating data 59 copying designs 57 Vault Manufacturing 58 Vault Manufacturing Web Client Vault mode in projects 69 Video Producer 52 views annotating 45 exploding 45 in drawings 41 modeling 66 V W T vault 55 add-ins for design applications 78 | Index 56 work features 7, 18, 28 work groups 55 58
