Autodesk Inventor 2009 Getting Started Part No.
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Contents Chapter 1 Introducing Autodesk Inventor . . . . . . . . . . . . . . . . . . 1 Getting Started . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1 Projects . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1 Data Files for Exercises . . . . . . . . . . . . . . . . . . . . . . . . 2 File Types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2 Application Options . . . . . . . . . . . . . . . . . . . . . . . . . 3 Document Settings . . . . . . . . . . . . . .
Files from Other Applications . . . . SAT Files . . . . . . . . . . . . . . . STEP Files . . . . . . . . . . . . . . IGES Files . . . . . . . . . . . . . . DWF Files . . . . . . . . . . . . . . . . . Learning Autodesk Inventor . . . . . . . Using Technical Publications . . . . Help . . . . . . . . . . . . . . . . . Help for AutoCAD Users . . . . . . Tutorials and Show Me Animations . Feedback Links . . . . . . . . . . . Skill Builders . . . . . . . . . . . . . Chapter 2 . . . . . . . . . . . . . . . . .
Chapter 3 Working with Sketched Features . . . . . . . . . . . . . . . . . 53 Parametric Part Modeling . . . . . . Part Modeling Environment . Workflows . . . . . . . . . . . Base Features . . . . . . . . . Adding Sketched Features . . . . . . Extrude Features . . . . . . . . Revolve Features . . . . . . . . Sweep Features . . . . . . . . Loft Features . . . . . . . . . . Coil Features . . . . . . . . . . Rib and Web Features . . . . . Modifying Features . . . . . . . . . Chapter 4 . . . . . . . . . . .
Learn About Projects . . . . . . . . . . . . . . . . . . . . . . Default Project . . . . . . . . . . . . . . . . . . . . . . Set an Active Project . . . . . . . . . . . . . . . . . . . How Referenced Files are Found . . . . . . . . . . . . . Setting Up Projects . . . . . . . . . . . . . . . . . . . . . . . Project Types . . . . . . . . . . . . . . . . . . . . . . . Single-user Projects . . . . . . . . . . . . . . . . Vault Projects . . . . . . . . . . . . . . . . . . . Set Up Folder Structures . . . . . . .
Other Sources of Components . . . . . . . Moving and Rotating Components . . . . Constraining Components . . . . . . . . Place Constraints . . . . . . . . . . . Mate Constraint . . . . . . . . Angle Constraint . . . . . . . . Tangent Constraint . . . . . . Insert Constraint . . . . . . . . Motion Constraints . . . . . . iMates . . . . . . . . . . . . . Viewing Constraints . . . . . . . . . . . . Editing Constraints . . . . . . . . . . . . Tips for Managing Assembly Constraints . Chapter 9 . . . . . . . .
Insert All Components At Work with Calculators . . . . . . . . Author User Parts . . . . . . . . . . Set File Names . . . . . . . . . Chapter 12 Once . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 194 . 197 . 198 . 201 Setting Up Drawings . . . . . . . . . . . . . . . . . . . . . . . 203 Creating Drawings . . . . . . . . . . . . . . . . . Edit Model Dimensions in Drawings . . . . Formatting Drawings with Styles . .
Viewing Multiple Positions of Assemblies . . . . . . . . . . . . . . . . 236 Tips for Creating Drawing Views . . . . . . . . . . . . . . . . . . . . 237 Chapter 14 Annotating Drawings . . . . . . . . . . . . . . . . . . . . . . 239 Annotation Tools . . . . . . . . . . . . . . . . . Using Styles to Format Annotations . . . . . . . Working with Tables . . . . . . . . . . . . . . . Hole Tables . . . . . . . . . . . . . . . . . General and Configuration Tables . . . . . Parts Lists . . . . . . . . . . . . . .
Tips for Using Content Center . . . . . . . . . . . . . . . . . . . . . . 270 Using the Publish Tool . . . . . . . . . . . . . . . . . . . . . . . . . . 270 Managing Administrative Tasks . . . . . . . . . . . . . . . . . . . . . 271 Chapter 16 Autodesk Inventor Utilities . . . . . . . . . . . . . . . . . . . 273 Editing Projects . . . . . . . . . . . . . . . . . . . . Legacy Project Types . . . . . . . . . . . . . . . . . Resolving File Links . . . . . . . . . . . . . . . . .
Introducing Autodesk Inventor 1 Welcome to Autodesk® Inventor™. This book explains the fundamental skills to start using Autodesk Inventor. In these chapters, the basic features are presented through examples and step-by-step procedures. The data files used in the procedures are installed with the Autodesk Inventor software. Getting Started Autodesk Inventor provides options during installation. The options selected determine what you see the first time you start Autodesk Inventor.
where design data is stored, where you can edit files, and maintains valid links between them. You use projects when you work in a team, work on multiple design projects, and share libraries among several design projects. See ProductName Utilities on page 273, for detailed information about setting up and using projects. Data Files for Exercises When you install Autodesk Inventor, a project called tutorial_files is created.
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. TRY IT: View the Properties dialog box ■ With a file open, right-click a component in the browser or in the graphics window, and then choose Properties from the menu. ■ Click the tabs to see properties. Application Options You can change the look and feel of Autodesk Inventor using settings on the Application Options dialog box.
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, the style library is managed by a CAD administrator. This practice ensures that the style definitions, used by all documents that use the drafting standard, are not accidentally replaced by a custom style.
Using Shortcut Keys and Command Aliases Autodesk Inventor provides shortcut keys and command aliases to help you perform certain tasks more quickly. A command alias is an alphanumeric character or character sequence used to start a command. Define a shortcut by using any of the following keys or key combinations: ■ A punctuation key (including ` - = [ ] \ ; ' , . /), or one of the following virtual keys: Home, End, Page Up, Page Down, Up Arrow, Down Arrow.
Key Result F5 Returns to the previous view. F6 Returns to isometric view. B Adds a balloon to a drawing. C Adds an assembly constraint. D Adds a dimension to a sketch or drawing. DO Adds an ordinate dimension to a drawing. E Extrudes a profile. FC Adds a feature control frame to a drawing. H Adds a hole feature. L Creates a line or arc. P Places a component in the current assembly. R Creates a revolved feature. S Creates a 2D sketch on a face or plane.
Key Result In a sketch, moves spline shape points. SHIFT + right-click Activates the Select tool menu. SHIFT + Rotate tool Automatically rotates model in graphics window. Click to quit. CTRL + ENTER Return to previous editing state. CTRL + Y Activates Redo (revokes the last Undo). CTRL + Z Activates Undo (revokes the last action). Spacebar When the 3D Rotate tool is active, switches between dynamic rotation and standard isometric and single plane views.
To rotate a view in 3D, use the Free Orbit or Constrained Orbit tool in the Standard toolbar to rotate a view around one of the coordinate axes. Zoom Tools The zoom tools are located in the Standard toolbar and are also available from the SteeringWheels. Zoom Use the Zoom tool on the Standard toolbar to enlarge or reduce the image in the graphics window. Click the tool. In the graphics window, press the cursor as you move it up or down to zoom the view dynamically in or out.
Zoom Window Use the Zoom Window tool on the Standard toolbar to define an area of a part, assembly, or drawing to fill the graphics window. Zoom Selected Use the Zoom Selected tool on the Standard toolbar to zoom a selected edge, feature, or other element to the size of the graphics window. Pan Use the Pan tool on the Standard toolbar to move the view in the graphics window in any direction planar to the screen. You can pan the view while other tools are active.
Look At Use the Look At tool on the Standard toolbar to zoom and rotate the display in the graphics window. You can position a selected planar element parallel to the screen or position a selected edge or line horizontal to the screen. Rotate Use the Orbit tools on the Standard toolbar to: ■ Rotate a part or assembly in the graphics window. ■ Display standard, isometric, and single plane projections of a part or assembly. ■ Redefine the isometric view.
Shaded, Hidden Edge, and Wireframe Display Use one of the Change Display tools to switch among the three display modes: Shaded, Hidden Edge, and Wireframe. You can apply display modes to part and assembly models, and to views in the Engineer's Notebook. Ground Shadow Display Use the Ground Shadow tool to cast a shadow on the plane beneath the model. Orthographic and Perspective Camera Views The Camera View tool has two settings: Orthographic Camera mode and Perspective Camera mode.
vanishing point. It is the way real objects are perceived by the human eye or by a camera. The following chart shows how the other viewing tools behave and how they can be modified in each camera mode.
you can export Autodesk Inventor drawings as DXF™ or AutoCAD drawing (DWG) files. The options for importing and saving AutoCAD files in Autodesk Inventor are: ■ Selection of layers. ■ Window selection of entities. ■ Saving files in DWG format. ■ Support for DXF files back to version 12. ■ Creation of AutoCAD® Mechanical files, if AutoCAD Mechanical is installed. NOTE Mechanical Desktop files can be linked to Autodesk Inventor assemblies without importing.
When you 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.
SAT Files SAT (*.sat) files contain nonparametric solids that can be Boolean solids or parametric solids with the relationships removed. You can use a SAT file in an assembly and add parametric features to the base solid. When you import a SAT file that contains a single body, it produces an Autodesk Inventor part file with a single part. If it contains multiple bodies, it produces an assembly with multiple parts. Surface data in a SAT file is also supported.
visual representation of 2D and 3D data in one file. Download and install the free Autodesk Design Review viewer to view a DWF file. Learning Autodesk Inventor You can select a learning tool that suits your preferred learning style. You can get help for the current task, follow a workflow in a tutorial or Show Me animation, learn a new skill using a Skill Builder, or click through Help topics. You can gain 3D knowledge as you transition from 2D and watch animations of operations.
Help Click Help ➤ Help topics for easy access to the Help topics, Skill Builders, and Tutorials. You can also navigate through the Table of Contents or use the Index and Search functions. When using Autodesk Inventor, click Help buttons on dialog boxes to retrieve a reference topic automatically that describes options for the dialog box.
Help for AutoCAD Users In Autodesk Inventor, click Help. If you selected “Users transitioning from AutoCAD” as your preference during the installation, your Help home page opens with topics and tutorials that ease the transition from 2D to 3D. You can also navigate to them through the AutoCAD Topics section in the Table of Contents.
Tutorials and Show Me Animations Online tutorials are step-by-step illustrated lessons that show you how to create and document your designs. You can access them from the Help home page or click Help ➤ Tutorials. Show Me animations are videos that show step-by-step instructions how to complete an operation. You can access Show Me animations from the Standard toolbar, the Help home page, and in individual help topics.
Skill Builders Autodesk Inventor provides extended learning through its Skill Builders learning modules. Skill Builders are posted throughout a release cycle on the Web to address customer needs and requests. You can access them (if you have Internet access) by clicking the link on the Help home page.
Creating Sketches 2 In Autodesk® Inventor™, sketching is the first step in creating a part. This chapter gives you an overview of the sketch environment and the workflow for creating sketches. Understanding Sketches 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. All sketch geometry is created and edited in the sketch environment, using Sketch tools on the panel bar.
The model you create in Autodesk Inventor is linked to its underlying sketches and sketch information. If you change a sketch, the model is automatically updated. Sketch Environment When you create or edit a sketch, you work in the sketch environment. The sketch environment consists of a sketch and sketch tools to control the sketch grid, and to draw lines, splines, circles, ellipses, arcs, rectangles, polygons, or points. When you open a new part file, the sketch environment is active.
Sketch Coordinate System When you start a new sketch, the sketch coordinate system is displayed as X and Y axes of the sketch grid. You can turn on the 3D indicator to display it at the sketch origin. (Click Tools ➤ Application Options ➤ Sketch tab. In the Display box, select the Coordinate System Indicator check box.) The default grid lies on the sketch plane. You can reposition and change orientation of the sketch coordinate system to: ■ Change the orientation of dimensions you create.
Using Model Edges as References for Sketches While you sketch, you can: ■ Automatically project edges of the part to the sketch plane as you sketch a curve. ■ Create dimensions and constraints to edges of the part that do not lie on the sketch plane. ■ Control the automatic projection of part edges to the sketch plane. Workflow overview: Project part edges to a sketch plane ■ Click the Project Geometry tool, and then select any part edge.
4 Press TAB to activate the Y field, and then enter a value. 5 Press ENTER to accept your input. The sketch is drawn according to the input. 6 Right-click and select Done to end the sketch tool. Creating Sketches In this exercise, you create a part file, and then create sketch geometry using basic sketching techniques. The following illustrates a completed sketch and sketched feature. Create Sketches When you open a new part file, the Sketch environment is active.
TRY IT: Start a sketch 1 On the standard toolbar, click File ➤ New. On the Metric tab, double-click Standard(mm).ipt. The new part is listed in the browser, and the sketch environment is active. 2 On the 2D Sketch panel bar, click the Line tool. Click the left side of the graphics window to specify a first point, move the cursor to the right approximately 100 units, and then click to specify a second point.
3 Move the cursor down and create a vertical line of approximately 10 units. 4 Move the cursor to the left to create a horizontal line of approximately 40 units. 5 Move the cursor up until the parallel constraint symbol is displayed and a dotted line appears. Click to specify a point. 6 Move the cursor left until the parallel constraint symbol is displayed and a dotted line appears, and then click to specify a point.
7 Move the cursor down until it touches the first point you specified at the beginning of the exercise. When the coincident constraint symbol is displayed, click to close the sketch. 8 In the graphics background, right-click and select Done. 9 Right-click again and select Finish Sketch. The sketch is completed. Do not save the file. Create Profiles with Tangencies In this exercise, you create a part file, and then use basic sketching techniques to create a simple profile.
2 On the standard toolbar, click View ➤ Toolbar ➤ Autodesk Inventor Precise Input to display the Precise Input toolbar. 3 Click the Line tool on the panel bar or on the 2D Sketch panel toolbar. Click the center of the graphics window, and then enter 65 in the X field of the Precise Input toolbar. Move the cursor to the right to display the horizontal constraint symbol, and then click to create a 65-mm horizontal line. 4 On the Precise Input dialog box, click the Y field, and then enter 15.
2 Move the cursor to the start point of the profile and click when the coincident constraint symbol is displayed. 3 In the graphics background, right-click, and select Done, and then right-click and select Finish Sketch. The sketch is completed. Do not save the file. Drag Sketch Geometry After you create sketch geometry, and while it is unconstrained or underconstrained, you can drag it to resize it. Tips for Sketching ■ Start a line by dragging off a circle or an arc.
When you start a new line, arc, or circle from an existing line, Autodesk Inventor can infer a coincident constraint to the midpoint, endpoint, or interior of the line. ■ Use SHIFT to drag. All drag features, except for a tangent spline, are also available by pressing and holding SHIFT while moving the cursor. ■ Drag multiple lines, curves, or points at the same time. Select the geometry, and then drag the last item you selected. ■ Switch between the Trim and Extend tools.
by dragging geometry until the cursor brushes the geometry you want to constrain. To view or remove constraints, use the Show Constraints tool on the 2D Sketch panel toolbar. Alternatively, right-click in the graphics window, and then use options on the menu to show or hide all constraints at once. To delete a constraint, select a constraint symbol, right-click, and then select Delete. Some geometric constraints work only with lines, while others work only with arcs, circles, or radial features.
Add Constraints to the First Sketch In this exercise, you practice adding geometric constraints to an existing sketch containing three closed loops. In some cases, you can greatly reduce the number of dimensional constraints required on a sketch. This exercise contains geometry that does not meet design criteria and requires additional geometric constraints to comply with the design intent.
Click the three sloping lines (be sure that you do not select the midpoint of the lines). Your sketch should look like the one in the following figure. 9 Right-click the graphics window, and select Done. 10 Right-click the graphics window, and select Show All Constraints. 11 All constraints display as shown in the following figure. 12 Right-click the graphics window, and select Hide All Constraints. 13 Click Return on the standard toolbar to exit the sketch.
3 Click the arrow beside the Constraint tool on the panel bar or on the 2D Sketch panel toolbar to open the pop-up menu. Click the Collinear constraint tool. Click the horizontal lines at the top of the sketch. Your sketch should look like the following figure. Note the collinear lines identified by the red arrows. 4 Press ESC to cancel the Collinear constraint tool. Drag the top-right horizontal line down and note how the sketch changes. This technique is known as constrained drag.
7 In the graphics background, right-click and select Done, and then right-click Finish Sketch to exit the sketch. Delete and Add Constraints Constraints can be removed from sketches. Show constraints, and then use the Delete option on the context menu. TRY IT: Delete a constraint and add a constraints 1 Activate Sketch3. 2 On the standard toolbar, click the Zoom Window tool, and then drag a window around the third sketch loop. The third sketch loop is centered on your screen.
6 Apply a tangent constraint to the arc and line at the left side of the sketch. 7 Apply equal constraints to the radii of the three arcs. Your sketch should look like the following figure. 8 In the graphics background, right-click and click Finish Sketch to exit the sketch. Do not save the file. Tips for Constraining Sketches ■ Turn off automatic constraints. Press and hold CTRL while sketching. ■ Infer a constraint. Move the cursor over other geometry while sketching to infer a constraint.
Dimensioning Sketches To retain design intent, sketch geometry generally requires dimensions in addition to geometric constraints to maintain size and position. Geometric constraints, such as horizontal, vertical, or parallel can be applied while you sketch. Dimensions are typically added after your sketch geometry is in place. In general, all dimensions within Autodesk Inventor are parametric. You can modify the dimension to change the size of the item dimensioned.
TRY IT: Create a parametric dimension 1 Create a sketch, or open an existing sketch. 2 In the Sketch environment, on the panel bar or on the 2D Sketch panel toolbar, click the General Dimension tool. 3 Select the sketch geometry you want to dimension, and then drag to a point to display the dimension. 4 Double-click the dimension to open the Edit Dimension box. 5 Enter a dimension value. You can enter numeric values or the parameter names associated with other dimensions or equations.
■ Use the Dimension tools to provide critical dimensions, and then use Auto Dimension to finish constraining the sketch. ■ Use AutoDimension in complicated sketches when you are unsure which dimensions are missing to constrain the sketch fully. ■ Remove automatic dimensions and constraints. NOTE To ensure that your sketch is fully dimensioned, use the Project Geometry tool to project all reference geometry to the sketch before using the Auto Dimension tool.
For example, when you dimension an edge to a vertex, the dimension automatically aligns itself with the edge. Diametric Dimensions In the design process of creating a revolved part, you can add a centerline as the axis of rotation. If this centerline is used in a sketch dimension, it is placed as a diametric dimension by default. Driven Dimensions You can place driven dimensions with Autodesk Inventor, and you can change the dimension type of an existing dimension to driven.
TRY IT: Apply dimensions to linear objects 1 With the project tutorial_files active, open the file dimsketch.ipt. The sketch geometry requires dimensional constraints to maintain its overall size. Geometric constraints were already applied to maintain the shape of the sketch. 2 In the browser, double-click Sketch1 to make the sketch active. 3 Click the Look At tool on the standard toolbar, and then select any line to obtain a plan view of the sketch. Click the Zoom All tool to view the entire sketch.
6 Click the dimension to display the Edit Dimension box. Enter 135 and press ENTER. In this example, you clicked the dimension to display the dialog box. If you are placing many dimensions, you can display the Edit Dimension box automatically. 7 With the General Dimension tool active, right-click the graphics window background, and select Edit Dimension from the context menu. 8 Complete the dimensional constraints as follows: Add a dimension of 10. Add a dimension of 60.
Add a dimension of 35. Add a dimension of 10.
Add dimensions of 25 and 30. 9 Right-click the graphics window and select Done from the context menu to exit the General Dimension tool. Delete and Add Dimensions Next, you remove the existing dimensions and use the Auto Dimension tool to quickly dimension the sketch. TRY IT: Remove dimensions and add dimensions to the sketch 1 Hold down the SHIFT key while you select each of the dimensions on your sketch. 2 When all the dimensions are selected, press DELETE to remove them.
Notice that the Auto Dimension dialog box now indicates that two dimensions are required. This is due to two missing Fix constraints. 5 Click Done on the Auto Dimension dialog box. 6 In the sketch, select and reposition dimensions so they are easier to read. Your dimensions should look like the following figure. Close the file without saving changes. Tips for Creating Dimensions ■ Place critical dimensions using the General Dimension tool, and then use Auto Dimension to speed up the dimensioning process.
all sketch geometry. You can then delete unwanted dimensions instead of selecting sketch geometry individually for automatic dimensioning. ■ If Auto Dimension does not dimension your sketch appropriately, you can experiment with selecting some of the sketch geometry to control how automatic dimensions are applied.
4 In the Count box, specify the number of elements in the pattern. 5 In the Angle box, specify the angle to use for the circular pattern. 6 Optionally, click More, and then choose one or more options: ■ Click Suppress to select individual pattern elements to remove from the pattern. The geometry is suppressed. ■ Click Associative to specify that the pattern updates when changes are made to the part. ■ Click Fitted to specify that pattern elements are equally fitted within the specified angle.
Tips for editing sketch patterns ■ You can modify the spacing between pattern elements, change the pattern count and direction, change the pattern calculation method, and suppress geometry in the sketch pattern. Right-click the sketch in the browser and select Edit Sketch. Then right-click a pattern member in the graphics window, and select Edit Pattern. On the pattern dialog box, revise values as needed. ■ You can edit pattern dimensions.
NOTE To delete individual sketch curves, edit the sketch, select the curve, and then press Delete. You can remove dimensional constraints from a sketch, and allow the sketch to resize as needed. Parts with adaptive features resize in when they are constrained to fixed geometry. Workflow overview: Delete sketch dimensions 1 Right-click the sketch in the browser and choose Edit Sketch. 2 Click the Select tool. 3 Right-click the dimension in the graphics window and select Delete.
When working in a 3D sketch, points can lie on any plane. Like 2D sketches, you can constrain sketch geometry to control its shape, add dimensions, and precisely position points relative to the last placed point. One way to learn about sketching in 3D is to create a box. TRY IT: Create a box and sketch 3D lines on X, Y, and Z planes 1 On the 2D Sketch panel bar, click the rectangle tool and create a rectangle and then enter E on your keyboard to use the shortcut to start the Extrude command.
Sketch some 3D lines and then use some of the other tools on the 3D Sketch panel bar: ■ Use the General Dimension tool to dimension the lines. ■ Use constraint tools to constrain 3D lines to other lines or points. ■ Optionally, change the setting on the Sketch tab of the Application Options dialog box to add or remove automatic bends in 3D lines.
Working with Sketched Features 3 In this chapter, you learn about parametric part modeling and the process for creating sketched features on parts. Parametric Part Modeling A part model is a collection of features. Parametric modeling gives you the flexibility to adjust the parameters that control the size and shape of a model, and automatically see the effect of your modifications.
Parent/child relationships exist between features, which means that one feature controls another. There can be multiple levels of parent/child relationships. A child feature is created after the parent feature, and cannot exist without a parent feature. For example, you can create a boss on a casting, and it may or may not have a hole drilled in it, depending on the application. The boss (the parent) can exist without the hole (the child), but the hole cannot exist without the boss.
Workflows Before you begin, analyze the part to determine which features to create, and the most efficient order in which to create them. Answer these questions before you start to model your design: ■ Are you creating a stand-alone part, a component in an assembly, or the first of a family of parts? Determine whether to create the part in a part file or within an assembly file, and whether you create constraints using fixed values or equations.
Workflow overview: Create a parametric solid model and associated drawings 1 Create a part in a part file (.ipt) or assembly (.iam) file. If you are working on a small assembly or it is early in the design process, consider creating your part in a part file. 2 Use tools on the Sketch toolbar or panel bar to sketch the basic shape of the base feature. Geometric constraints define the shape of objects in your sketch.
You can change the lengths of lines and the radii of arcs within the sketch at a later time. 5 Extrude, revolve, sweep, loft, or coil the parametric sketch to create the first, or base feature of the part. 6 Repeat the process to create additional features, selecting join, cut, or intersect to complete the part. 7 Document the part in an Autodesk Inventor drawing file to create the desired annotated 2D drawing views. Any time during the part modeling process, you can create a drawing file (.
You can select a face on an existing part, and sketch on it. The sketch is displayed 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. Each of the following operations creates a solid extrusion from a sketch profile. Extrude, Revolve, Sweep, and Loft can also create surface extrusions: Extrude Projects a sketch profile along a straight path. Use to create surfaces as well as solids.
2 Click the Extrude tool to display the Extrude dialog box. If there is only one profile in the sketch, it is automatically selected. If there are multiple profiles, on the Shape tab, click Profile, and then select the profile to extrude. Use Select Other to cycle through selectable geometry, and then click to select. 3 In Output, click either the Solid or Surface button. For base features, only Surface is available for open profiles. For assembly extrusions, only Solid is available.
Close the file without saving. Revolve Features Use the Revolve tool on the Part Feature panel bar to create a feature by rotating one or more sketched profiles around an axis. The axis and the profile must be coplanar. If this is the first feature, it is the base feature. Workflow overview: Create a revolved feature 1 To begin, sketch a profile that represents the cross section of the revolved feature you want to create. Except for surfaces, profiles must be closed loops.
Sweep Features Use the Sweep tool on the Part Features panel bar to create a feature by moving or sweeping one or more sketched profiles along a selected path. The path may be an open or closed loop, but must pierce the profile plane. Except for surfaces, profiles must be closed loops. There are three ways to create sweeps. You can create a sweep surface by: ■ Sweeping a profile along a path. ■ Sweeping a profile along a path and guide rail. The guide rail controls scale and twist of the swept profile.
9 Click OK. The sweep feature is created. Loft Features Use the Loft tool on the Part Features panel bar to blend or transition between the shapes of two or more profiles (called sections) on work planes or part faces. You can create a simple loft, a loft with rails (path), or a centerline loft. You can also select a point for one or both end sections of an open loft. To use an existing face as the beginning or end of a loft, create a sketch on the face so the edges of the face are selectable for the loft.
6 If appropriate, click the Closed Loop check box to join the beginning and ending profiles of the loft. 7 If appropriate, click the Merge Tangent Faces check box so that an edge is not created between tangent faces. 8 In Operation, click Join, Cut, or Intersect. 9 On the Conditions tab, the start and end profiles are listed. Click each, and specify a boundary condition: Free Condition Apply no boundary conditions. It is the default.
Workflow overview: Create a coil spring 1 To begin, sketch a profile that represents the cross section of the coil feature, and then use the Line tool or the Work Axis tool to create an axis of revolution for the coil. 2 Click the Coil tool. The Coil dialog box is displayed. If there is only one profile in the sketch, it is automatically highlighted. 3 If there are multiple profiles, click Profile, and then select the profile. 4 Click Axis. It can be at any orientation but cannot intersect the profile.
Use the Zoom and Rotate tools to position the part so the face where the rib is located is visible. Workflow overview: Set the sketch plane and create profile geometry for a rib 1 Create a work plane to use as the sketch plane. 2 On the Standard toolbar, click the 2D Sketch tool, and then click the work plane or a planar face to set the sketch plane. 3 Use the Look At tool to reorient the sketch. 4 Use tools on the 2D Sketch panel to create an open profile to represent the rib shape.
6 Optionally, in the Taper box, enter a taper or draft value. The direction must be perpendicular to the sketch plane to apply a taper value. 7 Click OK to create the rib. NOTE To create a rib or web network, sketch multiple intersecting or nonintersecting profiles on the sketch plane, and then follow the previous steps. Modifying Features There are several methods available to modify an existing feature.
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Creating and Editing Placed Features 4 In this chapter, you learn about placing and editing part features. Exercises step you through creation of holes, fillets, chamfers, threads, shells, circular and rectangular patterns, mirror features and analyzing faces. Adding Placed Features Placed features are common engineering features that do not require a sketch when you create them with Autodesk® Inventor™. When you create these features, you usually provide only the location and a few dimensions.
Dialog boxes define values for placed features, such as the Hole dialog box in the following illustration. Hole Features With Autodesk Inventor, you can create different types of holes: ■ Drill ■ Counterbore ■ Countersink ■ Spotface You can specify hole depth using one of three termination options: Distance, Through All, and To. Use the Drill Point option to set flat or angle drill points. Holes also can be classified as simple hole, clearance hold, tapped hole, or taper tapped hole.
7 In Termination, select Through All. 8 Click OK. The hole you defined is placed on the face. Close the file without saving or save the file under a different name to preserve the original data file. You can specify hole depth using one of three termination options: Distance, Through All, and To. TRY IT: Place a hole feature using arc centers 1 With the project tutorial_files active, open file hole.ipt. The part looks like the following figure.
The edges of the face and arc centers are projected onto the new sketch, allowing you to position the hole features. 3 In the graphics background, right-click, and then click Finish Sketch to close the sketch. 4 Click the Hole tool in the Part Features panel bar to display the Holes dialog box. In the preview window, edit the value of the hole diameter to read 6 mm. 5 Click the four arc centers. 6 In Termination, select Distance. 7 In the preview window, edit the value of the hole diameter to read 6 mm.
Close the file without saving or save the file with a new name to preserve the original data file. Fillet Features Fillet features add fillets or rounds to one or more part edges, between two faces or face sets, or between three adjacent faces or face sets. Fillets add material to interior edges to create a smooth transition from one face to another. Rounds remove material from exterior edges.
When you create variable radius edge fillets and rounds, you choose between a smooth blend from one radius to another and a straight blend between radii. The method you choose depends on your part design and the way adjacent part features blend into the edge. You can also specify points between the start and endpoints of a selected edge, and then define their relative distances from the start point and their radii. This technique provides flexibility when creating variable radius edge fillets and rounds.
Chamfer Features Chamfers are like fillets, except that the edge is beveled rather than rounded. When you create a chamfer on an interior edge, material is added to your model. When you create a chamfer on an exterior edge, material is cut away from your model. When you create a chamfer, you can specify one of three operations: ■ Distance ■ Distance and Angle ■ Two Distances A distance chamfer creates a face at an equal distance along the two faces that meet at the selected edge.
TRY IT: Add a chamfer 1 With the project tutorial_files active, open the file chamfillet.ipt. The file contains a model of a shaft socket bracket. 2 Click Chamfer from the Part Features panel bar. 3 On the Chamfer dialog box, click the Edges button, and then select the four vertical edges of the base. NOTE You may need to rotate the model to select the appropriate edges. Press F6 to return to the default isometric view. 4 In Distance, enter 10 mm, and then click OK.
Next, you add equal distance chamfers to top-hole edges. 5 Click Chamfer, and then select the top edge of each of the three holes in the part. 6 On the Chamfer dialog box, change the distance to 1 mm, and then click OK. Next, you add different distance chamfers to complete the basic shape of the socket support. 7 Click Chamfer, and then click the Two Distances button. Select the edge shown in the following figure.
8 Enter the following values: Distance 1: 14 mm Distance 2: 18 mm Click the Direction button to see how the preview changes when the distances are switched. 9 Click the Direction button again to return to the original settings, and then click OK to create the chamfer feature. 10 Repeat this process to add the same size chamfer to the other side of the part. Your part should now look like the following figure. Next, you add fillets to complete the final shape of the part.
TRY IT: Add fillets to a part 1 Click Fillet from the Part Features panel bar and ensure that the Edge Fillet button is selected. Select the two edges shown in the following figure. 2 Rotate the part, and then select the same two edges on the other side. In the Fillet dialog box, on the Constant tab, change the radius to 16 mm. 3 Under the edges and radius text, click the line that reads Click to Add. For the next set of edges, select the two vertical edges at the corners at the top of the part.
The fillet feature is added to the part and to the browser. 5 Click Fillet, and then select the two horizontal edges on the front of the rib, as shown in the following figure. 6 On the Fillet dialog box, enter 30 mm for the radius. 7 To add another set of edges, click the Click to Add text, and then select the two horizontal edges shown in the following figure.
8 On the Fillet dialog box, change the radius for the second selection set to 22 mm. Click the Click to Add text to create a third set of edges. 9 Rotate the model and select the horizontal edge on the back face directly opposite the second selection set. Enter 10 mm for the radius. When your dialog box and preview look like the following figures, click OK.
Fillet feature added to part 10 Click Fillet, and then select the three edges where the rib meets the cylinder at the top of the part. Change the radius to 2 mm, and then click OK. 11 Click Fillet. Select the two front edges of the rib, and then select the back edge of the rib (A). These edges are added to the selection set. 12 Select the three edges on each side where the base meets the other features (B). 13 On the Fillet dialog box, select the Loop option in the Select Mode section.
15 In the Error box, click Edit. 16 On the Fillet dialog box, select the Edge selection mode. Press SHIFT while you select the six edges where the base meets the other features of the part. When these edges are removed from the selection set, click OK. 17 Add a 2 mm fillet to the edges where the base meets the other features of the part. Notice how the fillets from Fillet 4 connect all the edges so only one selection point is required on each side. The completed part looks like the following figure.
Close the file without saving or save the file with a new name to preserve the original data file. Tips for Working with Fillets ■ To edit a fillet, right-click the fillet name in the browser and select Edit Feature. ■ To edit only the dimensional value of a fillet, double-click the fillet name in the browser. In the Edit Dimension box, change the value of the fillet.
2 Use Zoom Window to zoom in on the bottle top and cap. 3 Use Zoom Window to zoom in on the bottle top and cap.
4 In the graphics window or browser, select the cap, and then right-click and clear the check mark on Visibility in the context menu. 5 In the graphics window or browser, double-click the bottle to activate editing mode. 6 Click the Thread tool on the Part Features panel bar. 7 On the Location tab, enter settings to match the following figure. 8 Select the split surface as shown in the following figure. Notice how the thread is previewed on the model.
The Thread feature is created, as shown in the following figure, and is added to the browser. NOTE You can temporarily change the part color to see the threads more easily. On the Standard toolbar, click the arrow on the Styles box and choose a different color. 10 Click the Return button to exit edit mode for the bottle, and then turn off visibility for the bottle. 11 In the browser, double-click cap:1 to activate editing mode.
13 Double-click the assembly in the browser, turn on visibility of the bottle, and then restore the Isometric view. Your completed model should look like the following figure. Close the file without saving or save the file with a new name to preserve the original data file. Shell Features The Shell tool creates a hollow cavity in a part with walls of a specific thickness. It removes material from a part by offsetting existing faces to create new ones on the inside, outside, or both sides of the part.
Autodesk Inventor provides a precise shell feature. If a precise solution does not exist and approximation is enabled, an approximation is attempted. Start with a single feature, a part, or a part in an assembly. Workflow overview: Create a shell feature 1 For this exercise, create a simple block or cube. 2 After you extrude the sketch profile, click the Shell tool. 3 In the graphics window, select the face or faces to remove.
Creating Pattern Features Many designs call for the repetitive use of one or more features on a single part. Single features or groups of features can be duplicated and arranged in patterns. A pattern feature is a rectangular, circular, or mirrored duplication of features or groups of features. Individual occurrences in a pattern can be suppressed, as necessary. An example of a pattern feature is a rectangular pattern of identical holes cut from a calculator case.
TRY IT: Create a hole feature 1 With the project tutorial_files active, open the file recpattern.ipt. 2 On the Part Features panel bar, click the Hole tool. 3 On the Hole dialog box, in the Placement box, select Linear. Click the Face button, and then select the top face of the part. 4 In the Hole dialog box, click the Reference1 button. 5 In the graphics window, click the leftmost edge of the part for Reference 1, and then the bottom edge for Reference 2.
7 On the Holes dialog box, Termination, select Through All, and verify that the hole diameter is 3 mm. 8 Click OK to create the hole in the part according to the specifications you entered. Add Hole Patterns Use the hole feature you just created to create a hole pattern. TRY IT: Create a hole pattern from a hole feature 1 On the Part Features panel bar, click Rectangular Pattern. 2 In the graphics window, click the hole feature.
3 On the Rectangular Pattern dialog box, click the Direction 1 button, and then click the bottom horizontal edge of the part. Click the Flip button to change the direction, if needed. 4 Verify that Spacing is selected in the drop-down list, and then in the Column Count field enter 5, and in Column Spacing enter 17.5 mm. A preview of the pattern is displayed in the graphics window for Direction 1. 5 Click the Direction 2 Select button, and then click the leftmost vertical edge of the part.
Suppress Pattern Occurrences A review of the design intent for the part shows that two unneeded occurrences were added. You can suppress all or individual occurrences in a pattern. TRY IT: Suppress pattern occurrences 1 In the browser, Expand Rectangular Pattern1 to display the occurrences. Point to the occurrences. As the cursor points to each occurrence, it is highlighted in the graphics window. 2 Highlight the occurrence that did not execute.
TRY IT: Create a circular pattern 1 With the project tutorial_files active, open file circpattern.ipt. 2 On the Part Features panel bar, click the Circular Pattern tool. 3 On the lower flange of the part, click the counterbored hole feature. 4 On the Circular Pattern dialog box, click the Rotation Axis button, and then in the browser, click Work Axis1. A preview of the pattern is displayed. 5 In Placement ➤ Count, verify that the value is 6.
7 Click OK to create a circular pattern. Close the file without saving or save the file with a new name to preserve the original data file. Mirror Features You can mirror part, surface, and assembly features to create and maintain symmetry. By using a mirror feature, you can also reduce the amount of time required to create a model. You can mirror individual solid features, work features, surface features, or the entire solid.
Workflow overview: Mirror a part 1 Create a part body to mirror. Create a work plane to serve as a mirror plane or, if you prefer, use a planar face as the mirror plane. 2 On the Part Features panel bar, click the Mirror Feature tool. 3 On the Mirror Pattern dialog box, click the Mirror Entire Solid button. 4 Click the Mirror Plane button, and then select a work plane or planar face. 5 Click OK.
2 Click the Rectangular Pattern tool. 3 In the Rectangular Pattern dialog box, select the Pattern Individual Features option. 4 Click the Features button and in the graphics window or in the model browser, select features to arrange in a pattern. 5 Click the Path selection button, and then select the path. Click Flip to change the column direction, if appropriate. 6 Enter the count (number of features) for the column, and then click the drop-down arrow to specify pattern length.
■ Under Compute, select Optimized to create optimized pattern, Identical to create identical features, or Adjust to Model to terminate features when encounter a face. ■ Under Orientation, select Identical to orient all features the same as the first selected, or Direction 1 or Direction 2 to specify which path controls the rotation of pattern features. 9 Click OK. Suppress Pattern Occurrences You can temporarily suppress the display of one or more solid or surface features in a pattern.
Analyzing Parts Analyzing solids and surfaces provides information for validating the geometric quality before manufacturing. You can save several different analyses of the same or different types for a specific model. For example, you can define several ways to analyze a particular set of surfaces on the same model. Once an analysis is applied, an Analysis folder is created in the browser and the analysis is placed in the folder. Each saved analysis is added to the browser in the order it is created.
Workflow overview: Create and use analyses 1 Open a part file or double-click a part in an assembly. 2 Click Tools ➤ Analysis or click the arrow on the Analysis Visibility tool, and then select the type of analysis to create. 3 On the setup dialog box for the analysis, adjust the analysis settings as needed. 4 Apply the analysis. 5 Change visibility on the active analysis as needed. 6 Use the Model browser to edit, copy, delete, and rename saved analyses.
Workflow overview: Create a Zebra Analysis 1 Open a part file or double-click a part in an assembly to in-place edit the part. 2 Click the arrow by the Analysis Visibility tool, and then select New Zebra Analysis from the list. NOTE After the initial analysis is saved, you can right-click the Analysis folder in the Model browser, and then select New Zebra Analysis from the context menu. 3 If appropriate, double-click the name to enter a custom name. 4 Specify horizontal, vertical, or radial direction.
4 Click New. If appropriate, double-click the name to enter a custom name. 5 Specify the degree range (relative to the pull direction) to analyze for draft angle. 6 Select Gradient to display results in a gradient rather than stripes. 7 Select All, Faces, Quilts, and then select the appropriate geometry. 8 Click an edge, axis, or planar face to specify pull direction or click Flip to reverse the direction. 9 Click OK.
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Creating and Editing Work Features 5 In this chapter, you learn about creating and editing work features. Defining Work Features Work features are abstract construction geometry that you can use when other geometry is insufficient for creating and positioning new features. To fix position and shape, constrain features to work features. Work features include work planes, work axes, and work points.
Work Planes A work plane is a flat plane extending infinitely in all directions along one plane. A work plane is similar to the default origin YZ, XZ, and XY planes. However, you create the work plane as needed, using existing features, planes, axes, or points to locate the work plane. Use a work plane to: ■ Create a sketch plane when no part face is available to create 2D sketched features. ■ Create work axes and work points. ■ Provide a termination reference for an extrusion.
■ Provide a reference for assembly constraints. ■ Provide a reference for drawing dimensions. ■ Provide reference for a 3D sketch. ■ Provide reference for a circular pattern. ■ Create lines of symmetry. The following illustrations show some of the methods you can use to define a work axis. Work Points A work point is a point that exists relative to, and is dependent on, features or work features.
Grounded Work Points A grounded work point, like all work points, depends on an associated feature to determine its location. A grounded work point uses features or work features to initiate the grounded work point tool, but its position is then fixed in space and not dependent on, or associated to, those or other features. You can use a grounded work point in the same ways that you would a work point. However, the grounded work point remains fixed in space regardless of changes to model geometry.
4 Continue to revise the position of the work point. When finished, click OK. Modifying Work Features Other than the grounded work point, 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, any feature or geometry that is dependent on a work feature for its definition is also affected by changes to the work feature. Both scenarios are shown in the following illustrations.
A work axis was added to the hole, making the work axis dependent on the hole. If the angle of the plane is modified to 15 degrees, the hole and work axis adjust accordingly.
6 Using Projects to Organize Data In this chapter, you learn how projects help you organize and manage your data. You learn to plan and set up your projects based on your design needs. Key Terms Term Description active project The project that Autodesk® Inventor™ automatically defaults to when opening, saving, or editing components. There can be only one active project in an Autodesk Inventor session. Can be a project you have specified or the default installed project.
Term Description frequently used subfolders Named subfolders of project folders (including libraries) that are frequently accessed. Folders are not used to resolve references or store references. They are listed on file access dialogs so that you can easily locate the folders. The path to frequently used subfolders always begins with the name of the project location. libraries Libraries are project locations containing read-only files that are referenced, but not edited.
Term Description referenced file A file used in the current design. A referenced file may be editable or it may be read-only, as in the case of library parts. relative path In projects, paths are relative to the location of the projects file (.ipj). Autodesk Inventor uses relative paths to locate referenced files. root folder A top-level folder defined as a library, workspace, or workgroup in a project.
Term Description should be the only defined editable location. Learn About Projects A project represents a logical grouping of a complete design or product, including its model files, drawings, presentations, and design notes. Project information is stored in XML files with the .ipj extension that specify where you edit files, how many versions are retained when you save a file, where referenced data is stored, and other settings.
and libraries for the session. When you work on a different design project, you must make its project active before you can create or edit data files. TRY IT: Make a project active 1 Verify that all Inventor files are closed. 2 Click File ➤ Projects, or on the Microsoft® Windows® Start menu, click Programs ➤ Inventor (release number) ➤ Tools ➤ Project Editor. 3 On the Projects dialog box, top pane, the existing projects are listed. Double-click a project to make it the active project.
A project searches for nonliterary files in the editable locations. For best results, specify only one editable location in each project. Because other design groups may also use the same library parts, library locations may be specified in multiple projects. It is a good practice to make library locations and the files in them read-only. Setting Up Projects Set the project type when you create or edit a project.
Single-user Projects Use single-user projects for individual designers: ■ All design files are in one folder (the workspace) and its subdirectories, except for files referenced from libraries. ■ Store the project file (.ipj) in the workspace (root) folder and specify .\ as the workspace. ■ The file check-out status is not available in the browser. Typical Single User project setup Type Single User Workgroup Location None Location One workspace defined at .\.
Vault Projects To use the vault project, Autodesk Vault software must be installed. A different dialog box opens so that you can create a Vault project. Characteristics of a vault project include: ■ Designers never view or work directly on the vaulted version of a file. ■ Each designer uses a project file that defines a personal workspace where Autodesk Vault copies the vaulted files for viewing and editing.
Folder Options Defines the folders containing project-specific Styles, Templates, and Content Center files. Vault Options Values are typically set in Autodesk Vault. Virtual folder = virtual folder within the vault database that maps to the root folder for the project. Publish folder = specifies where Streamline data is published.
■ If you intend to reference released design files, copy them to a library folder, or define a library in your project that locates the root folder of the released project. If the released project also references libraries, include them in the project or use Pack and Go to flatten the file structure into a single folder. ■ Keep the subfolder structure relatively flat and do not store files that are unrelated to the project under the root folder.
Workspace locations One defined at .\ One defined at .\ Workgroup locations None None Libraries One or more One or more not nested under workspace TRY IT: Create a project with the Project Editor 1 Close all documents in Autodesk Inventor. When files are open, the active project is read-only. The only exception is that you can add libraries without closing all files.
5 Click Next to specify libraries. New projects often use the same libraries as existing projects. In the left pane, libraries are collected from all project files in the projects list. ■ In the right pane, click the right arrow to add a library location to the New Project. ■ Click the left arrow to remove a library location from the New Project.
The Library location box shows the location of a library selected in the left or right panes. 6 Click Finish. Once the project is created, double-click it in the Project Editor, and then customize it by setting options. In the next sections, customize the project you just made by following the procedures. Set Project Options The project type, the default workspace, and library names and locations are set in the project wizard.
When setting the workspace path: ■ Specify only one location in a workspace, preferably at the root location containing the project file or in a subfolder of the project file. The recommended location is .\. In a single user project, the workspace should be the only location in your project, except for library locations. ■ For best results, use Autodesk Vault to check out rather than manually copy files.
■ A library creates an association between a library name and the folder for the current project. ■ The relative path stored in the referencing file is relative only to the library folder, not to any other project locations. Only the named library is searched when resolving a library reference.
■ You cannot open or edit a proxy file. ■ Proxy files are updated only when you open or save the assembly that uses the corresponding Mechanical Desktop file. ■ Proxy files contain the Mechanical Desktop design data for a single part, translated to the Inventor data format. ■ Design properties (iProperties) are stored in proxy files, and are lost if you lose the proxy file.
■ You cannot open or edit a proxy file. ■ iPart and iAssembly Factory proxy files are catalog elements from the factory, published with a specified set of parameters. ■ Update proxy files by opening or saving the assembly that uses the corresponding factory member file. ■ Do not make an iPart or iAssembly proxy library folder read-only, because the factory has to create new members there.
Other Types of Libraries In Projects Most projects use libraries such as third party components, company collections of commonly used parts, Mechanical Desktop parts, iAssemblies and iParts. However, you may find that your organization has other component files that you would like to reference but do not intend to edit. Because library references include the library name, and only that library location is searched to resolve a library reference, library file names need only be unique within that library.
Avoid Duplicate File Names In general, it is not a good idea for different files to have the same file name, even if they reside in different folders. Inventor uses search rules to resolve references and duplicate names can lead to difficulty in locating a file. Avoid using duplicate file names and set the project option Using Unique File Names to Yes. Libraries are an exception to this rule. Often the files come from third-party vendors that have their own file naming schemes.
NOTE If you specified Frequently Used Subfolders in the project options, they are also listed in the Locations pane. 5 Double-click a file to open it.
Managing Assemblies 7 This chapter introduces assembly modeling. You will learn about the assembly environment, assembly browser and working in the assembly environment. Assembly Environment In Autodesk® Inventor™, you place components that act as a single functional unit into an assembly document. Constraints define the relative position these components occupy with respect to each other. When you create or open an assembly file (.iam), you are in the assembly environment.
Assembly Design Strategies Traditionally, designers and engineers create a layout, design the parts, and then bring everything together in an assembly. With Autodesk Inventor, you can create an assembly at any point in the design process instead of at the end. For a clean sheet design, you start with an empty assembly and create the parts as you develop the design. To revise an assembly, you create the new parts in-place so they mate with existing parts.
Top-Down Assembly Design When you design from the top down, you begin with design criteria and create components that meet those criteria. Designers list known parameters and may create an engineering layout (a 2D design that evolves throughout the design process). A layout can include contextual items such as the walls and floor where an assembly will stand, machinery that feeds into or receives output from the assembly design, and other fixed data.
Each default workplane is coplanar with its respective axes. For example, the YZ plane is coplanar with the Y axis and the Z axis. Assembly Constraints Assembly constraints are applied to components to define positional relationships in the assembly. For example, you can force two planes on separate parts to mate, or specify that a hole and a bolt always remain concentric.
Projects manage component locations by specifying such things as: ■ The master location of files (the workgroup), when you work in a design team. ■ A private workspace specified by each designer, where files are created and edited. ■ Libraries of standard and custom components. ■ Locations of templates and style libraries. ■ The names of frequently used subfolders, to make file location faster.
■ Designate a component as grounded. ■ Edit or delete the assembly constraints between first-level components. The features of an activated part can be edited in the assembly environment. When you activate a part, you are working in the part environment. Double-click a parent or top-level assembly to reactivate it. Visibility of Components Controlling component visibility is critical to managing large assemblies.
assembly with flat structure assembly after restructure Components restructured as a group maintain constraints between them. Constraints to components outside the group are lost. Restructure Assemblies In the browser, components are initially listed in the order in which they were placed in the assembly. You can rearrange components by dragging them to a new position in the browser or by using the context menu.
Workflow overview: Create a new subassembly containing selected components 1 Start with an open assembly. 2 Select components from the assembly browser or in the graphics window. 3 Right-click, and then select Component ➤ Demote. The Create In-Place Component dialog box displays. 4 Enter a file name for the new assembly, select a new template if necessary, and then click OK. A new subassembly is created and populated with the selected components.
Assembly View Nests assembly constraint symbols below both constrained components. Part features are hidden. Selecting this button disables Modeling View. Modeling View Places assembly constraint symbols in a folder at the top of the browser tree. Part features are nested below parts, just as they are in part files. Selecting this button disables Assembly View.
Producing Bills of Materials You can create a bill of materials (BOM) for an assembly. A bill of materials is a table that contains information about parts in an assembly, such as quantities, names, costs, vendors, and all of the other information someone manufacturing the assembly might need. Bill of materials information is automatically collected from iProperties.
Placing, Moving, and Constraining Components 8 In this chapter, you learn how to place and constrain components, and to edit constraints using the Edit Constraints dialog box. Placing Components In Assemblies In the assembly environment, you can add existing parts and subassemblies to create assemblies or you can create new 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.
The first component placed in an assembly is automatically grounded (all degrees of freedom are removed). Its origin and coordinate axes are aligned with the origin and coordinate axes of the assembly. It is a good practice to place assembly components in the order in which they would be assembled in manufacturing. Click in the graphics window to place additional ungrounded occurrences of the first component in the assembly. To finish placing the first component, right-click, and then select Done.
Drag Components into Assemblies You can place multiple components in an assembly file in a single operation by dragging them into the graphics window. You can drag components to an open assembly window from the following locations: ■ From an open folder in Windows Internet Explorer®. Use this technique to quickly populate a new assembly with components. ■ From an open Inventor part file. Drag the top-level icon from the part browser to the assembly graphics window.
If you are working in shaded mode, components that are not enabled are nearly transparent in the graphics window. In wireframe mode, they are displayed in a distinct color in the graphics window. An icon in the Assembly browser identifies the component as not enabled. Parts and subassemblies that are required only for context, or components that do not require editing, are good candidates to be designated as not enabled.
You can use the DWG/DWF™ File Wizard to import parts and assemblies from the Autodesk® Mechanical Desktop®. You should migrate Mechanical Desktop files to the latest version before you translate to Autodesk Inventor. You have an opportunity to fix any errors before the translation. Autodesk Inventor can also place components created in other CAD systems that have been saved as SAT files (ACIS) or IGES files, or exported through a STEP translation process.
Each time you update the assembly, the assembly constraints are enforced. ■ You can make some parts adaptive. Autodesk Inventor allows adaptive part features to change size, shape, and position based on the applied assembly constraints. ■ Assembly constraints remove degrees of freedom from components, positioning them relative to one another. As you modify component geometry, assembly constraints ensure that the assembly stays together, following the rules you have applied.
■ Use the Predictive Offset and Orientation button with Mate, Flush, and Angle constraints. When turned on, it gives the offset value for the current location for the selections you are constraining. It also changes the orientation to a flush constraint if you have it set to mate, then pick two faces with the vectors pointing in the same direction, and visa versa. The dialog box remains open as you place constraints, so you can place multiple constraints of all types.
■ On the Place Constraint dialog box, select Pick Part First. Click the component you want to constrain. Clear the check box to restore the ability to select all components. Selectable geometry is limited to features on the selected component. ■ Point the cursor to the required geometry. Right-click, and then choose Select Other. Click the arrows in the Select Other box to cycle through the underlying face, curve, and point selections. Click the green center button to accept the highlighted selection.
Mate Type - Mate So- Use the mate constraint with the mate solution to make lution two planes face each other and make them coplanar, make two lines collinear, or place a point on a curve or plane.
in the same direction. Faces are the only geometry that can be selected for this constraint. Angle Constraint The angle constraint specifies an angle between planes or lines on two components. Angle Type Specifies an angle between planes, axes, or lines on two components. The two sets of geometry need not be of the same type. For example, you can define an angle constraint between an axis and a plane. Constraints of this type are often used to drive assembly motion.
Tangent Constraint The tangent constraint causes surfaces of planes, cylinders, spheres, or cones to contact at the point of tangency. Tangent Type At least one surface must be non planar. Surfaces defined by spline curves cannot be used in a tangent constraint. Tangency may be inside or outside a curve, depending on the direction of the selected surface normal. Outside Solution Positions the first selected part outside the second selected part at their tangent point.
Insert Constraint The insert constraint causes a circular edge on one component to be concentric and coplanar with a circular edge on another component. The offset value for an insert constraint is the distance between the two faces containing the circular edges. For example, you can use this constraint to place a pin or a capscrew in a hole. Solutions Specifies the direction of the face normal for the planes containing the circular edges. An arrow indicates the normal direction.
want to animate. To return components to their original positions, unsuppress any suppressed constraints. iMates An iMate is a constraint that is saved with a component to tell it how to connect with other components in an assembly. When you insert a component with an iMate, it snaps into place with another component with a matching iMate. The component can be replaced by another component while preserving these intelligent iMate constraints.
When you hover the cursor over an assembly constraint in the browser, the constrained components are temporarily highlighted in the graphics window. Selecting the constraint in the Assembly browser highlights the geometry in the graphics window until you click again in the graphics window or the browser. Editing Constraints You can edit assembly constraints two ways. Workflow overview: Edit constraint values by selecting in the browser 1 In the assembly browser, select an assembly constraint.
■ Drag components to check translational degrees of freedom. You can see how a component is constrained. ■ Create component iMates for repeated use. Using iMates, you can define placement information on parts and assemblies to use repeatedly.
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Creating Assemblies 9 In this chapter, you learn how to create parts and assemblies in place, about adaptive parts, patterns, assembly features, and other procedures for managing assemblies. Creating Assembly Components Assembly modeling combines the strategies of placing existing components in an assembly, and creating other components in place within the context of the assembly.
view orientation as the XY plane. If the YZ or XZ plane is the default sketch plane, you must reorient the view to see the sketch geometry. After you create the base feature of your new part, define additional sketches based on the active part or other parts in the assembly. When defining a new sketch, click a planar face of the active part or another part to define the sketch plane on that face.
Workflow overview: Set a default sketch plane to create a component in place 1 Click Tools ➤ Application Options ➤ Part tab. 2 In the Sketch on New Part Creation box, select a sketch plane for the default. 3 Click OK. 4 Double-click the assembly name in the browser to return to the assembly. 5 In the browser header, click the arrow and select Assembly View. In the assembly view of the browser, assembly constraints are nested below the component with which they are associated.
Projected geometry remains associated with the part from which it was projected and automatically updates to match changes in the original part's geometry. When you project geometry from an existing component onto a new sketch it becomes reference geometry. You can use reference geometry to create an adaptive matching part that automatically updates to reflect any modifications to the outer boundary of the component from which the geometry was projected.
Subassemblies can be nested many layers deep in a large assembly. By planning and building subassemblies, you can efficiently manage the construction of very large assemblies. Additionally, you can create subassemblies that match the intended manufacturing scheme to facilitate creating your assembly documentation. Guidelines for Selecting Subassembly Components When designing a subassembly for modeling, select: ■ Component groups that repeat in an assembly.
a component pattern of a nut and bolt by selecting an existing bolt hole pattern. Edits to the bolt hole pattern control the location and number of bolts and nuts. Associative component patterns: ■ Include and retain constraints of the original component. If the original component is constrained, then the component pattern is constrained. ■ Are associative to a part feature such as a pattern of bolt holes. ■ Contain individual elements that can be suppressed for display or functional purposes.
5 Enter the number of components to be created in the column and the spacing between each. 6 On the Rectangular tab, click the Row Direction selection arrow, and then select an edge or work axis from the graphics window, enter the number of components in the row, and the distance between the components. Click flip to the row direction, if necessary. 7 Click OK. Workflow overview: Create a circular component pattern 1 Place a component in an assembly file.
Workflow overview: Make a pattern element independent of a pattern 1 Expand the pattern in the browser. 2 Right-click an element other than the source component, and then select Independent. The element is suppressed and a copy of the components it contains is added to the browser. NOTE To create a new component based on another component, save a copy with a different name and place the copy in the assembly.
■ Describe a specific manufacturing process, such as match drilling or post-machining. Components can be constrained to assembly features. You cannot, however, place a constraint between an assembly feature on one part and the same assembly feature on another part. You can roll back the state of assembly features to view the effect of each assembly feature on the model or to place additional assembly features in the desired context.
stage, which is replaced by the actual part or subassembly when detailed design is required. Parts from one vendor may be replaced with similar parts from another supplier. In the following illustration, the Replace Component tool is used to replace a simple sketched representation with the actual part. When you replace a component in an assembly, the new component is positioned with its origin coincident with the origin of the component it replaces.
plane. You create half of the assembly, and then mirror it to create the second half. The mirrored components are exact copies, positioned relative to the mirror plane. You can either save a new assembly file with mirrored components and open it in a new window, or reuse components and add the mirrored components to the existing assembly file. TRY IT: Mirror assembly components 1 Open the assembly you want to mirror. 2 On the Assembly panel bar, click the Mirror Components tool.
7 Click the More button to select preview options and specify handling of content library components: ■ To enable the mirrored state for library components, clear the Reuse Content Library Components check box. By default, only instances of the library parts are created in the current or new assembly file. ■ To display status of mirrored components in the ghost color in the graphics window, In Preview Components, select check boxes. 8 Click OK.
13 If you need to change status or select new components, click Return to Selection. Otherwise, click OK to accept and close the dialog box. Copying Assemblies Use the Copy Component tool to create a copy of a source assembly or its components. You can either create a new assembly file and open it in a new window, or add copied components to an existing assembly file. Each copied component creates a new file. You can reuse components instead of copying them.
Status Description Reused Creates a new instance in the current or new assembly file. Excluded Subassembly or part is not included in the copy operation. Mixed Reused/Excluded Indicates that a subassembly contains components with reused and excluded status, or that a reused subassembly is not complete. 4 To enable copying of library components, click the More button and clear the Reuse Content Library Components check box. 5 Choose OK to open the Copy Components: File Name dialog box.
8 To update the filenames, click Apply. To return to the original values, click Revert. 9 On the Component Destination box, choose one of the following: ■ To place components in the current assembly file, click Insert in Assembly. ■ To open a new assembly file, click Open in New Window. 10 To change status or select new components, click Return to Selection. Otherwise, click OK.
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Analyzing Assemblies 10 In this chapter, you learn to analyze assembly components for interference by simulating the motion of the assembly components. Checking for Interference In the physical assembly built from your design, two or more components cannot occupy the same space at the same time. To check for such errors, Autodesk® Inventor™ can analyze assemblies for interference. The Analyze Interference tool checks for interference between sets of components and among the components in a set.
NOTE Creating components in place, using faces of adjacent components as sketch planes, and projecting geometry from other component faces for use in sketches reduces the chance of interference between parts. Workflow overview: Analyze interference between parts 1 Activate the assembly that you want to analyze. Interference analysis is only available in the assembly environment. 2 Click Tools ➤ Analyze Interference. 3 Select the two sets of components to be analyzed. 4 Click OK.
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) have been removed. Autodesk Inventor does not require you to completely constrain any component in an assembly. You can save time by removing only critical DOF for your model.
Careful planning and placement of assembly constraints is the key to obtaining proper assembly motion. Apply as many assembly constraints as needed to position, or in the case of an adaptive part, size your component. Temporarily suppress assembly constraints that interfere with assembly motion. Constraint Drivers Dragging a small component in a large assembly, or dragging a component about an axis of rotation can be difficult.
Use the Drive Constraint tool on the context menu to simulate mechanical motion by driving a constraint through a sequence of steps. Right-click the constraint in the browser and then enter information in the Drive Constraint dialog box to define the drive constraint and to control motion. Constraints may limit the motion of parts. Depending on the geometry, degrees of freedom are removed or restricted.
Animating Assembly Components Mechanical assemblies are rarely static. By animating the movement of constrained assemblies with Autodesk Inventor, you can examine your model throughout its range of motion. Use Inventor assembly animation to visually check for component interference and examine mechanism movement to improve your designs. In this two-part exercise, you first constrain a component in a lift fixture assembly.
2 Click View ➤ Degrees of Freedom. The NewSleeve.ipt part is unconstrained, so all six degrees of freedom are available. 3 Click the Constraint tool in the panel bar or from the Assembly toolbar. Place a mate constraint between the major axis of NewSleeve.ipt and the axis through the cylinder feature of NewSpyder.ipt. This constraint removes two translational degrees of freedom and two rotational degrees of freedom from the sleeve. 4 Remove the last rotational degree of freedom from the sleeve.
5 The sleeve is now constrained to move only along the axis of the spider. Click View ➤ Degrees of Freedom to hide the DOF symbols. 6 Use the Rotate and Zoom tools to orient your view of the assembly as shown in the following figure. 7 Slowly drag the NewLiftRing.ipt. All components with constraints that are linked to the dragged component move in response, while honoring their own assembly constraints. Close the file without saving or save the file with a new name to preserve the original data file.
selection set. You can isolate the selection set by turning off visibility of all components that are not selected. Before you try the following exercises, open an assembly and click the Select button on the Standard toolbar, and then select the priority mode: Part Priority Selects parts or assemblies instead of features, faces or edges. Component Priority Selects only the first-level components of the edited assembly.
TRY IT: Select by component size 1 On the Assembly Standard toolbar, click Select ➤ Component Size. 2 If not preselected, use the Select tool in the Select by Size box to select a component. Selections are contained in a virtual box called a bounding box. Its size is determined by the outermost extremities of the selected component. 3 The size is shown, determined by the bounding box of the selected component. Click At Most or At Least to specify the relative size to select, and then click the green arrow.
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Using Design Accelerator 11 In this chapter, you learn about Design Accelerator and how to work with generators and calculators. What is Design Accelerator Design Accelerator represents an important component of Functional Design, providing engineering calculation, and decision support to identify standard components or create standards-based geometry.
the Design tab, you specify the placement options and select the type of components you want to insert. In the Calculation tab, you enter the calculation values. For Bolted Connection Generator and for some calculators, the Fatigue Calculation is also available to specify values for fatigue calculation. NOTE Only one generator/calculator can be open at a time - when one generator/calculator is opened and you want to open a new one, the first one is automatically closed.
■ Involute Splines ■ Parallel Splines ■ Key Connection ■ Disc Cam ■ Linear Cam ■ Spur Gears ■ Bevel Gears ■ Worm Gears ■ Bearing ■ V-Belts ■ Synchronous Belts ■ Roller Chains ■ Clevis Pin ■ Joint Pin ■ Radial Pin ■ Secure Pin Workflow overview: Insert components using Design Accelerator generators/calculators 1 On the Assembly panel bar, open the Design Accelerator panel bar, and click the appropriate generator or calculator.
Work with Bolted Connections Use the Bolted Connection generator to design and check pretensed bolted connections loaded with axial or tangential force. The purpose of the design calculation is to select an appropriate bolted connection after specifying the required working load. The strength calculation performs a check of bolted connection (for example, pressure in the thread and bolt stress during joint tightening and operation).
TRY IT: Insert a bolted connection 1 With the tutorial_files project active, open Bolted_connection.iam. The assembly should look like the following figure. 2 On the Assembly panel bar, click the Bolted Connection tool. 3 On the Design tab, Type section, select Through All. 4 In our assembly, we have a hole where we want to insert the bolted connection. In the Placement selection list, select By hole. 5 Click the Start Plane button.
6 Select Existing Hole. In the assembly, select the hole as shown in the following figure. 7 Select Termination. In the assembly, select the termination plane as shown in the following figure.
8 Specify the thread type and dimension as follows: As Thread: ISO Metric profile Insert Diameter: 6mm 9 Begin populating the bolted connection. Select Click to add a fastener. A filtered list of available fastener content (from Content Center) displays. It is based upon previously set Thread settings (Standard and Thread size). You can narrow the displayed list of fasteners by selecting a standard. 10 In the displayed list of bolts, select Slotted Flat Countersunk Hex bolt.
11 Select Click to add a fastener. In the washer selection list, select Plain washer (metric). The selected washer displays in the Design tab of the bolted connection generator. In the Inventor assembly, the washer preview is created. 12 Select Click to add a fastener. In the nut selection list, select Hex jam Nut. The selected nut is displayed in the Design tab of the bolted connection generator. In the Inventor assembly, the nut preview is created.
13 Click OK. Now, when the bolted connection is inserted, it is easy to change any component with the bolted connection. We will change the type of washer. 14 In the file Bolted_connection.iam assembly, select the inserted bolted connection. 15 Right-click and select Edit Using Design Accelerator. The Bolted Connection generator displays. 16 Click the arrow at the end of the Plain washer (Metric) edit field to display the washer selection list.
Insert All Components At Once It is also possible to insert all types of components (component, feature, calculation) at one time. In the following exercise, you insert key and shaft groove using the Key Connection generator. TRY IT: Insert Key connection 1 With the project tutorial_files active, open the file bearing.iam. The assembly should look like the following figure.
2 On the Design Accelerator Assembly panel bar, click the arrow next to Shaft item and select Key Connection. The Key Generator displays. 3 On the Design tab, first specify the placement of the shaft groove. Make sure that Create New is selected in the Shaft Groove selection list. Click the shaft element to select reference for shaft groove insertion as shown in the following figure. 4 Select the second reference as shown in the following figure. In the assembly, the shaft groove preview is presented.
5 According to the selected shaft element, the shaft diameter value was inserted to the Key Generator and edit field became disabled. Edit the Key Length by either selecting the value from the selection list or use the preview grip in the assembly. 6 On the Design tab, Select objects to Generate, click the Hub Groove button to disable hub groove insertion. Only the key and shaft groove icons are enabled to insert key and shaft groove. 7 Click OK.
Work with Calculators Design Accelerator offers a set of tools to perform mechanical calculations of selected components. Engineering calculators use standard mechanical formulas and physical theories in design and validation of mechanical systems. You specify calculation criteria and calculators perform the calculation and displays report about a calculation. If the calculation doesn’t indicate the calculation compliance, error message is displayed advising you what values need to be updated.
■ Step Tube Solder Joint ■ Step Solder Joint ■ Separated Hub Joint ■ Slotted Hub Joint ■ Cone Joint ■ Tolerance ■ Limits and Fits ■ Press Fit ■ Power Screw ■ Beam and Column ■ Plate ■ Shoe Drum Brake ■ Disc Brake ■ Cone Brake ■ Band Drum Brake TRY IT: Calculate separated hub joint 1 On the Design Accelerator panel bar, click Separated Hub Joint. 2 On the Calculation tab, enter calculation parameters. 3 Click Calculate to perform the calculation.
for efficient use of functionally smart content ready for publishing to the Content Center Library.
TRY IT: Author user parts 1 Open a custom iPart in Autodesk Inventor. 2 Click File ➤ Component Authoring. 3 Select the part category. The Category selection list displays the list of available publishing categories. Once you select a Category, the graphics and selection prompts change depending upon the Category of component selected. 4 Create the iMates following the tooltips and graphical guide for the specific component.
NOTE Since you selected a category early on in the process, the Content Center displays this category for publishing. For example, a bolt can now be published directly into the Bolt category, an existing subcategory of Bolt, or you can create a category under Bolt. NOTE You can rename the iMates as needed. These new names populate the iMate list in both the panel browser and the Component Authoring dialog under the iMate list.
NOTE In the File Naming dialog, you can only edit items in white edit fields. TRY IT: Set file names 1 In the Design Accelerator Generators and Calculators, click the file Naming icon. 2 Double-click the Display name to insert the display name. 3 Click the button next to the edit filed to specify the folder where component is stored. 4 Click OK to confirm the settings and close the File Naming dialog box.
Setting Up Drawings 12 In this chapter, you learn about setting up drawings, using drawing styles, and using drawing resources such as sheet layouts, title blocks, and borders. Creating Drawings 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.
Inventor™. Set the option to allow drawing dimensions to resize the model. Similarly, your drawing file automatically updates with any changes saved in the model file. Autodesk Inventor comes with standard templates to use as the starting point for your drawings. Template files have the standard drawing extension (.idw, .dwg). Autodesk Inventor stores template files in the Autodesk\Inventor (version number)\Templates folder.
dimensions or views, or to change the locations of notes and balloons) to reflect the revisions. Sometimes it is more efficient to create a quick 2D drawing using a sheet sketch or draft view than it is to design a solid model. With Autodesk Inventor, you can create 2D parametric drawing views, which you can also use as sketches for 3D modeling. NOTE You can directly open AutoCAD® DWG (.dwg) files in Autodesk Inventor using the open command and then view, plot, and measure the file contents.
All styles associated with a drafting standard are stored in a style library. You can customize the style library and link it to a project file (.ipj). All files included in the project then use the same styles for formatting. If you use style libraries on projects, share styles among designers. Documents are uniformly formatted, and updates are easy. When you update the main style definition in the library, all documents that use the style library can update their formatting.
Share Styles Between Documents You can share styles between documents in two ways: ■ Use Format ➤ Save Styles to Style Library to save a new or edited style to the style library. Then it is available for use in any document. ■ Use the Styles Editor Import/Export tool to select one or more styles and export them at once. The same process is used to import styles. Use Styles Available In Drafting Standards Each drafting standard has a complete set of styles.
NOTE Some styles are used on several tabs. For example, the Dimension Text tab specifies appearance of text used in dimensions. The formatting originates in the Text style, accessed in the browser pane. When a style references another style for some of its formatting, the referenced style is called a substyle. Create Styles You can create a style by modifying an existing style. The changed style is saved in the current document and is not available to other documents until it is saved to the style library.
Select the Add to Standard check box so that the style is listed among available styles for the standard. You can check later by clicking the Standard style and then clicking the Available Styles tab. Your new style is listed and its check box is selected. 3 The new style name is listed in the browser pane under Leader. Select the name and change values as desired. 4 Click Save to save the new style in the current document, and then click Done.
Using Drawing Resources You can modify the drawing border and title block to comply with your company specifications. NOTE Always save customized settings to drawing resources in the template. Otherwise, they are available only in the current document. The first folder at the top of the browser is Drawing Resources. You can expand Drawing Resources to show the sheet formats, borders, title blocks, and sketched symbols that are available to use in the drawing.
Sheet Layouts When a new drawing is created, it automatically has at least one sheet. You can change the default sheet size to a standard or custom sheet size, and specify its orientation. You can insert borders, title blocks, and views onto the sheet. Available borders and title blocks are listed in the Drawing Resources folder in the browser. Icons in the browser represent the sheet and all its component elements. You can add multiple sheets to a drawing. Use the browser to move views between sheets.
Format Sheets You can create a sheet with a predefined layout of border, title block, and views by using a sheet format from Drawing Resources ➤ Sheet Formats. Right-click the sheet resource, and then select New Sheet. The format corresponds to a standard sheet size with an appropriate title block and border. If the format you choose contains one or more views, the Select Component dialog box is displayed when you create a sheet. Use the Browse button to specify the model to document.
You can create and save custom borders in the current drawing. Unlike the Default Border, custom borders are not parametric and do not resize when a sheet is resized. Once a custom zone border is inserted, right-click the border and select Edit Definition or Edit Instance. Make changes and save it according to the option selected (to the instance or the definition). If it exists within the Drawing Resources folder under Borders, you can right-click and select Edit.
Title Blocks The title blocks in an Autodesk Inventor drawing reflect information about the drawing, the sheet, and the design properties. As this information changes, the title block is automatically updated to display the current information.
The standard drawing templates contain title block formats that you can customize and use. You can also create your own title block formats. Workflow overview: Define a new title block 1 With an .idw file open, click Format ➤ Define New Title Block. The current sheet becomes an active sketch plane, and the Drawing Sketch panel bar is activated. 2 Use the tools on the Drawing Sketch panel bar to draw the title block. Define and use a grid to accurately sketch the lines for the title block.
NOTE The new title block is added to the Drawing Resources folder in the drawing browser. Align Title Blocks Position a title block in any of the four corners of your drawing sheet. You can set the default position for title blocks using the Title Block insertion control in the Drawing tab of the Options dialog box. To access the Options dialog box, click Tools ➤ Application Options. Autodesk Inventor uses that point to position the title block in the specified corner of the sheet.
■ Use drawing formats with predefined views. To make sheet formats available to new drawings, create them in a template file that you use to create new drawings. Define a sheet for each sheet type you use. ■ Use the Select filters. In addition to the Edge, Feature, and Part filters, you can specify various drawing elements for the Select filter. ■ Drawing formats override units of measure. If components in an assembly have different units, the drawing format overrides them.
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Creating Drawing Views 13 In this chapter, you learn about the types of drawing views you can create using Autodesk ® Inventor™. Drawing Views Drawing views are referenced from, and associative with, external assembly or part files. You can produce multiview drawings of principal orthographic views and auxiliary, detail, section, and isometric views. You can also create views from assembly representations such as design views, positional, and level of detail, and presentation views.
Drawing View toolbar to create a base view and set the options on the Drawing View dialog box. Use the base view to create a projected, auxiliary, overlay, section, and detail views. You can also create an isometric view using the projected view tool. When placing a projected view, move the preview to change the orientation of the projected view to an isometric view. The following types of drawing views are available: projected view Projects from the base view to a desired location.
crop Provides control over the view boundary in an existing drawing view. Set the type of boundary (rectangular or circular) and specify crop boundaries. slice Produces a zero-depth section from an existing drawing view. The Slice operation is performed in a selected target view. Base Views The first view in a new drawing is a base view. Use the Base View button on the Drawing Views panel bar to create additional base views as needed.
To edit view parameters, select the view, right-click, and then select Edit View to open the Drawing View dialog box. Creating Multiview Drawings A multiview drawing contains a set of single plane orthographic views which are used to display an object through one view plane per projection. For example, a first angle projection is one view in a multiview projection set. Base Views In this exercise, you create a base view, and then project views to create a multiview orthographic drawing.
5 Click the Display Options tab, and then verify that All Model Dimensions is not selected. 6 Position the view preview in the lower left corner of the sheet, in Zone B7. Click the sheet to place the view.
7 Click the Projected Views tool in the Drawing Views Panel. Click the base view and move the cursor vertically to a point above the base view. Click the sheet in Zone E6 to place the top view. 8 Move the cursor to the right of the base view. Click the sheet in Zone C2 to place the right-side view. 9 Right-click, and then select Create from the context menu. Now create an isometric view. 10 Click the Projected View tool in the panel bar or from the Drawing Views panel bar.
Section Views Autodesk Inventor can create a full, half, offset, or removed section view from a base view. The crosshatching, section line, and labels are placed automatically. You can also use the Section Views tool to create a view projection line for an auxiliary or partial view. By default, a section view is aligned to its base view. Press and hold CTRL as you position the section view to place it without alignment.
of the cutting line. The cutting line can consist of a single straight segment or multiple segments. When you have defined the view projection line, the Section View dialog box is displayed. NOTE You can use the CTRL key to prevent constraining the view projection line. In this exercise, you create section, detail, and auxiliary views. TRY IT: Create a section view 1 With the project tutorial_files active, open the file sectionview.idw. The drawing contains orthographic views and an isometric view.
Next, drag horizontally until a perpendicular constraint appears (C), and then click to define the second segment of the section line. 7 Drag horizontally to the right of the part (D), and then click to create the last segment of the section line. Right-click, and then select Continue. The projection line is defined, and the Section View dialog box is displayed. 8 Zoom out. Drag the section preview down to Zone D6, and then click to place the view. 9 The section view is placed in the drawing.
NOTE Press F5 to return to the previous view after zooming in to place the cutting plane. Auxiliary Views With Autodesk Inventor, you can create and place a full auxiliary view of a selected view. The auxiliary view is projected from and aligned with a selected edge or line in the base view. The selected edge or line in the base view defines the projection direction. Auxiliary views are labeled, and display a projection line to the base view.
4 Move the preview down and to the left. Click the sheet in Zone B7 to place the auxiliary view. Detail Views With Autodesk Inventor, you can create and place a detail view of a specified area of a drawing view. A detail view is created without alignment to its parent view. By default, the scale of the detail view is double the scale of the parent view, but you can specify any scale. Autodesk Inventor labels the detail view and the area it is derived from on its parent view.
The center point of the fence positions the detail, and the fence determines the extent of the viewed detail. Right-click to select fence shape, click the center point of the detail, and then click a point to set the fence for the detail. Next, you create a detail view to show a portion of the parent view at an enlarged scale. TRY IT: Create a detail view 1 Zoom in on the top view. 2 Click the Detail View tool in the panel bar or from the Drawing Management toolbar.
The view is placed. If necessary, click the view boundary and adjust its position. Close the file without saving or save the file with a new name to preserve the original data file. Break Views You can create breaks in existing base, projected, section, detail, and auxiliary views. You select the existing view, define the appearance of the break, and then specify the location of the break lines in the view. The broken view retains the scale of the original view.
Select the Rectangular or Structural style to define the general appearance of the break lines in your view. Then use the Orientation controls to specify the direction of the break lines. Use the Gap control to set the distance between the remaining segments of the view after it was broken. Adjust the value in the Symbols field to control the number of break symbols displayed each break line. You can set the symbol size in proportion to the gap size by using the slider control.
Delete Views You can delete views that are no longer necessary. If you delete a base view, dependent projected and auxiliary views can either be deleted or retained. Section and detail views require a base view and cannot be retained. To delete a view, select the view, right-click, and then select Delete. In the Delete View dialog box, click the More button (>>) to select the dependent views to retain. TRY IT: Delete a base view 1 With the project tutorial_files active, open the file delbasev.idw.
Align Views Alignment is the constraint relationship between a dependent view and its parent view. An aligned view can be moved only within its constraints. If the parent view is moved, the aligned view moves to maintain its alignment. Most dependent views are created with an alignment, but you can add, change, or remove alignment relationships. There are four possible alignment relationships between a dependent view and its parent view: Vertical, Horizontal, In Position and Break.
Edit Hatch Patterns You can apply double-hatching, and you can modify the following aspects of a section view hatch pattern: ■ Pattern ■ Angle ■ Line weight ■ Scale ■ Shift In the following steps, you edit the section view hatch pattern to represent the material as bronze using the ANSI 33 hatch pattern. TRY IT: Modify a hatch pattern 1 Right-click the hatch pattern in the section view, and then choose Modify Hatch. The Modify Hatch Pattern dialog box is displayed.
Rotate Views You can rotate views by edge or by angle. Views rotate as rigid bodies, including any sketches. When a view is rotated, annotations maintain their associativity to the view and model geometry. Depending upon the drawing standard used, additional information may be provided in the View label indicating that the view is rotated out of its normal position.
■ In the assembly, create as many positional representations as are needed to show different positions. ■ To change to a different positional representation for an overlay view, delete the overlay and specify a new positional representation when creating an overlay. Tips for Creating Drawing Views ■ Create nonaligned section views. Press and hold CTRL while placing section views to break the alignment. ■ Move views between sheets. Click a view in the browser and drag it to another sheet.
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Annotating Drawings 14 In this chapter, you learn about annotating drawings using dimensions, center marks, centerlines, hole tables and hole notes, parts lists and tables, and leader text. Annotation Tools Drawing annotations provide additional information to drawing views to complete documentation of a component. In Autodesk® Inventor™, styles define annotations, according to the active drawing standard. Each standard has a default set of available styles, which can be customized as needed.
Annotation Tool Description Hole/Thread Notes Adds hole and thread notes to features created using the Hole feature or Thread feature tools in parts. Bend or Punch Notes Adds bend or punch notes to drawing views of sheet metal parts. Chamfer Note Adds a chamfer note to a drawing view. Center Mark Automatically sizes center mark extension lines to fit the geometry. You can copy and paste center marks.
Annotation Tool Description Caterpillar Adds a caterpillar annotation to geometry in a drawing view. The annotation is not associated with weldments in the model. End Fill Adds a 2D end fill annotation to geometry in a drawing view. The weld bead style determines the size and formatting. Revision table Places a revision table on a drawing sheet. User Defined Symbols Adds sketched symbols to a drawing or a template.
Hole Tables Hole tables in drawings show the size and location of some or all of the hole features in a model. Hole tables eliminate the need to add notations for each hole feature in a model. In addition to drilled, counterbored, and countersunk holes, you can add center marks, iFeatures, holes in patterns, and extruded cuts to a hole table. The format for hole tables is set in the hole table style.
You can generate a parametric parts list for an assembly. The properties for each part or subassembly are displayed in the parts list. You can specify the items you want in the list, such as part number, description, and revision level. You can edit a parts list. Creating Dimensions In Drawings The tools you use to create drawing dimensions are different from the tools used for model dimensions.
Dimension from a Drawing, you can edit a model dimension and the source component also updates. Use the Retrieve Dimension tool to display model dimensions. After you select the dimension to retrieve, right-click a dimension to delete or edit. You can drag dimensions to adjust their positions. When you place a view, you can choose to display model dimensions. Usually, model dimensions are in the first, or base view in a drawing.
Change Dimensions Dimensions styles control the appearance of dimensions in drawings. When you apply the style to a dimension, it takes on the characteristics defined in the style. Within the dimension style, the text style is referenced as a substyle to format dimension text. Alternate units, the preferred display style, tolerance, leaders (which reference the leader style) and text are also specified in the dimension style.
Use dimension styles to control dimension text, arrowheads, dimension lines, and extension lines. A dimension style is provided for each drafting standard, but you can create new styles to suit your own annotation requirements. These examples show a dimension that uses the default ISO dimension style, and one with custom style settings applied. TRY IT: View dimension styles in the Styles and Standards Editor dialog box 1 Open an existing drawing or create a drawing.
NOTE If you apply a dimension style to a dimension, overrides on that dimension are lost. Copy Dimension Styles among Drawings The Style Library Manager provides a convenient way to copy dimension styles (and other styles) from one drawing to another. Close Autodesk Inventor before using the Style Library Manager. TRY IT: Access the Style Library Manager 1 On your desktop, click Start ➤ Programs ➤ Autodesk ➤ Autodesk Inventor [version] ➤ Tools ➤ Style Library Manager.
■ Centerline ■ Centerline Bisector ■ Centered Pattern Add center marks and centerlines before adding drawing dimensions. You can dimension to the ends of the center marks and centerlines and maintain correct gaps. You can add center marks to extruded circular cut features and include these cuts in a hole table. Add the center marks to the hole table style so they are recognized in the drawing. TRY IT: Add center marks, circular cuts, and hole features to the hole table style. 1 Open a drawing file.
Use the Leader Text tool to add notes to elements in a drawing. If you attach the leader line to geometry in a view, the note is moved or deleted when the view is moved or deleted. The Format Text dialog box is used to enter text and to set the text parameters. Using Hole and Thread Notes Hole and thread notes document both internal and external hole features or threaded objects.
In section views, the hole must either be displayed in its face normal position or seen as a profile. You can also annotate holes in isometric views. Working with Title Blocks Title block information that you typically enter when you complete a drawing is obtained from the drawing properties. Right-click the drawing name in the drawing browser and select iProperties. You enter information in the Properties dialog box, and the values are displayed in the corresponding locations in the title block.
Both model dimensions and drawing dimensions are used to document feature size. TRY IT: Add views to a drawing 1 With the project tutorial_files active, open the file dimsannot-5.idw. The drawing file contains a single sheet with a border and title block. 2 Click the Base View tool in the panel bar or from the Drawing Views panel bar. The Drawing View dialog box is displayed. 3 Click the Browse button, and then double-click views-5.ipt to use it as the source for the view.
6 Position the view preview in the lower left corner of the sheet (in Zone C6). Click the sheet to place the view. 7 Click the Projected View tool in the panel bar or from the Drawing Views panel bar. Click the base view and move the cursor vertically to a point above the base view. Click the sheet in Zone E6 to place the top view. 8 Move the cursor horizontally to the right of the base view. Click the sheet in Zone C3 to place the right-side view. 9 Move the cursor above the right-side view.
Turn Off Tangent Edge Displays Turn off the display of tangent edges in the isometric view. TRY IT: Modify a drawing view 1 Right-click the isometric view, and then select Edit View. 2 In the Drawing View dialog box, click the Options tab, and then clear the check mark from Tangent Edges. Click OK. The following are orthographic and isometric views of the clamp.
Add Model Dimensions Next, you add model and drawing dimensions to the views using the Retrieve Dimensions command. Some model dimensions are removed, while others are repositioned. TRY IT: Add model dimensions 1 Zoom in on the front view. 2 Right-click the front view, and then choose Retrieve Dimensions. In the Retrieve Dimensions dialog box, click the Select Dimensions tool. The model dimensions that are planar to the view are displayed. 3 Select each of the dimensions except for the 45.
Reposition Model Dimensions To reposition dimension text, click a dimension text object, and then drag it into position. The dimension are highlighted when it is a preset distance from the model. Radial dimensions can be repositioned by selecting the handle at the end of the leader. TRY IT: Reposition radial dimensions 1 Drag the dimensions until they appear as illustrated in the following figure. 2 Pan to display the top view, right-click, and then choose Done.
4 Select each of the dimensions except the 13.0 horizontal dimension, and the R6.0 and R2.0 radial dimensions. 5 Click Apply. Each of the selected dimensions are displayed. The dimensions that were not selected are hidden. Click Cancel to exit dialog box. 6 Drag the remaining dimensions until they appear as shown in the following figure. Add Centerlines and Center Marks Centerlines and center marks are added to aid in the placement of drawing dimensions.
3 Pan to display the front view. 4 Click the arrow beside Center Mark and then click the Centerline Bisector tool. 5 Select the two hidden lines that represent the drilled hole through the boss. The bisecting centerline is added. 6 Pan to display the right-side view. 7 Select the two hidden lines that represent the drilled hole through the boss. The bisecting centerline is added. Add Drawing Dimensions Drawing dimensions are added to complete the documentation of the model.
TRY IT: Add drawing dimensions 1 Pan to display the front view. 2 Click the General Dimension tool on the Drawing Annotation panel bar. 3 Click the right endpoint of the bottom edge, and then click the right endpoint of the top of the boss. 4 Move the cursor to the right and place the 16.0 dimension between the 13.0 and 19.0 vertical dimensions, as shown in the following figure. 5 Pan to display the top view. 6 Use the General Dimension tool to add the 13.0, 45.0, and 40.
The drawing dimensions are added. Format Dimensions The dimensions can be formatted to add additional information, to adjust precision, or to add tolerances. TRY IT: Format dimensions in a drawing 1 Right-click the 15° dimension, and then choose Text. 2 In the Format Text dialog box, enter TYP, and then click OK. 3 Right-click the 16.00 dimension, and then select Text. 4 In the Format Text dialog box at the insertion point, press the space bar, and then enter BOSS. Press ENTER.
Click OK. The formatted dimensions are displayed. Add Notes and Leader Text In the following steps, you add a general note and use leader text to document the round. TRY IT: Add a note and leader text to a drawing 1 Click the Text tool in the panel bar or from the Drawing Annotation toolbar. 2 Click a point below and to the right of the top view. 3 Enter TOLERANCE FOR, and then press ENTER. 4 On the next line, enter ALL DIMENSIONS (space). 5 Select the tolerance icon from the symbol list. Enter 0.5.
Edit Model Dimensions If, when you installed Autodesk Inventor, you set the option to allow drawing dimensions to resize the model, when a model dimension is edited, the part model is updated along with the drawing views. TRY IT: Edit a model dimension in a drawing 1 Right-click the 15° dimension, and then choose Edit Model Dimension. 2 In the Edit Dimension dialog box, enter 10-deg for the new dimension, and then press ENTER. The model and drawing are updated.
Notice how the position of the boss was affected by the change to the model dimension. WARNING Modifying a model dimension directly affects your model. Autodesk Inventor automatically updates the part file with the changes you make. Complete Title Blocks The drawing properties are used to complete the title block information. TRY IT: Complete a title block 1 From the File menu, select iProperties. The Properties dialog box is displayed. 2 On the Summary tab, in Author, enter your name.
The drawing is complete. Save the file. Printing Drawing Sheets Autodesk Inventor uses any Microsoft® Windows® configured printer to print a copy of your design documentation. Most large-format plotters can be configured as Windows system printers.
If the drawing is too big to print on one sheet, select the Tiling Enabled check box. This option is only available when the scale is set to Model 1:1. Registration marks are printed on page corners to allow alignment of printed pages. Page identifiers contain the drawing and sheet name and a table cell number to help keep pages in order. Plotting Multiple Sheets Use the Multi-Sheet Plot wizard to plot multiple drawing sheets that include drawings of various sizes.
Using Content Center 15 This chapter provides basic information and concepts about Content Center and Content Center libraries. For more detailed information, see Help in Autodesk® Inventor™ and Autodesk® data management server. About Content Center Content Center is a tool used for accessing and maintaining the Content Center library. You use Content Center to: ■ Find a part in a Content Center library. ■ Insert a Content Center library part in an assembly.
Content Center Library The Autodesk Inventor Content Center library provides Inventor parts (fasteners, steel shapes, shaft parts) and features to insert in assemblies. Libraries can be either local, or in a shared environment accessed from a central server. The Content Center library data are accessed in the Content Center. See the Help for more information about the library configuration. The basic component in the Content Center library is a family (part family or feature family).
sets of parameter values for one part family. Every set of parameters defines one member of the part family. Working with Content Center You use the Content Center dialog box to navigate in the Content Center library hierarchy. You expand categories in the Category Listing panel, double-click items in the List panel, or use navigation buttons in the toolbar, such as Back, Forward, and Up one Category Level.
Consumer Environment Use the Content Center Consumer environment to use library parts in the design process. The following commands are available: Open from Content Center Place from Content Center Place Feature from Content Center Change size Opens a family .ipt file. Places a feature or a part into an open assembly file. Places a feature into an open part file. Changes the size of a part placed in an assembly.
8 Use the typical placement operation to place the part in assembly. Add constraints as needed to position the part to other geometry. Editor Environment Use the Content Center Editor environment to modify library parts by using one of the following commands: ■ Create, Delete, and Edit Categories. ■ Copy a read-only category or family to a read/write library for editing purposes. ■ Use the Save Copy As command to create a copy of a family in a read/write library. ■ Rename library parts and families.
7 On the Content Center Editor dialog box, click Done. Tips for Using Content Center ■ Use Search to find a part in the Content Center library. You can search for parts with a specified string in the Part Number or Description property, or you can specify conditions for part family or category parameters. ■ Use Content Center Favorites to store frequently used parts or part families. You can create a folder structure in Favorites and order favorite items as you need.
Managing Administrative Tasks You add and remove libraries to and from the active Content Center configuration, using the Configure Content Center Libraries dialog box. The configuration of Content Center libraries is saved in the active project. Libraries must be configured on the Autodesk server before you configure Content Center libraries in the Inventor project. Perform all administrator tasks using Autodesk Server Console. ■ Create a new read/write or read-only library.
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Autodesk Inventor Utilities 16 In this chapter, you learn how to edit a project in Autodesk® Inventor™, resolve missing file links, search rules for library and non library files, and old versions of files. You learn how to copy, move, rename and delete data, and change the file structure in a project. Editing Projects After you create a project, you can use the Project Editor to change some of its options, add or delete file locations, or change its name.
Keep in mind: ■ To add a single folder to a project path, right-click Libraries or Frequently Used Subfolders, and then select Add Path. Browse to the individual folder and add it to the project. ■ To add an editable location for each immediate subfolder of a folder, right-click a search path, and then select Add Paths from Directory. Browse to the root folder and add it to the project.
TRY IT: Edit a project 1 Verify that all Autodesk Inventor files are closed. 2 Use one of these methods to start editing: ■ Click File ➤ Project. ■ On the Microsoft® Windows® Start menu, click Programs ➤ Autodesk Inventor ➤ Tools ➤ Project Editor. ■ On the Microsoft Windows Start menu, click Autodesk ➤ Autodesk Inventor ➤ Tools ➤ Project Editor. ■ In Microsoft® Windows® Explorer, right-click an .ipj file, and then click Edit.
NOTE To review definitions of all project options, click the Help button on the Project Editor dialog box. Legacy Project Types In the Project wizard, semi-isolated and shared project types are unavailable by default. Autodesk® Vault is the recommended solution for managing multi-user projects. If, however, you have legacy projects and have a requirement to create and use them, consider the following points: ■ Click Tools ➤ Application Options ➤ General table.
■ The Using Unique File Names option is No, and the file was renamed, moved to a different subfolder, or one of the project subfolders was renamed. ■ A library was renamed or its location was removed from the project. ■ The file was moved from one library to another or from an editable location. ■ The file was moved from one library subfolder to another. ■ The data set was taken off site without the shared libraries. If it is acceptable, select the Skip All options when the Resolve Link.
Search for Library and Non Library Files Autodesk Inventor searches for referenced files in library locations in the order listed in the Project Editor and then the workspace. If a referenced file is contained in multiple project locations, the reference uses the relative path from the first one found, and stores the path in the reference. If the project location is a library, the name of the library is also stored in the reference.
Search for Non Library Locations In non library locations, Autodesk Inventor appends the relative path stored in the reference to the project location and looks for a file at the resulting full path. If no file is found, the file name stored in the referenced file is appended to the project location folder path and Autodesk Inventor looks there. Use Substitution Rules to Find Missing Files In the Resolve Link dialog box, you can create a substitution rule to search for missing files.
Using the new subfolder path, select the check box, and edit both paths to remove the \yyy\zzz tail as shown in the following image to locate all parts. When you click Open, you indicate that the path is correct. Autodesk Inventor attempts to find part 2.ipt, and each of the other referenced parts, it automatically substitutes DEF for the ABC subfolder portion of the relative path.
the referenced library box contains its name. You can use these boxes to repair references to: ■ A renamed library. ■ Files moved from one library to another. ■ Files moved from a library to an editable location. ■ Files moved from an editable location to a library. NOTE Search for other unresolved references using this location is automatically selected. Clear the check box to avoid creating a substitution rule.
TRY IT: Restore an old version of a file 1 Click File ➤ Open. 2 Browse to the file you want to restore from the OldVersions directory. The Open Version dialog box is displayed. 3 Select one of the options in the Open Version dialog box: Open old version Opens the old version of the file. Because the current file still exists, you cannot save the opened version. Use Save Copy As to save a copy. Restore old version Restores the selected old version as the current to current version version.
NOTE To save memory, Autodesk Inventor loads only the portion of a file that is needed for an operation. Additional information is loaded as needed. Therefore, do not delete an Autodesk Inventor file if there is a chance that someone else is using the file in an active Autodesk Inventor session. You can set the number of versions to keep when you create or edit a project. Each time a file is saved, the previous version is moved to its OldVersions\ folder.
search, you preserve the references, along with annotations and dimensions in the indirect references. ■ Use Design Assistant to move, copy, or rename files and repair the references from referencing files at the same time. After you copy or move files, open them in Autodesk Inventor to verify that all of the links are correct before you give them to a vendor or other designer to use. Zip Files You can use zip files to move data, archive, or copy data sets for vendors.
Temporary Root Folders You can move data, archive, or copy data sets for vendors. When you have no nested folders in your project, you can easily archive or give data sets to vendors. You can move data, archive, or copy data sets for vendors. When you have no nested folders in your project, you can easily archive or give data sets to vendors. TRY IT: Move or copy data using a temporary root folder 1 Create a top-level (root) folder.
copied to the specified location without changing the contents of any of the source files. All referenced files must be resolvable using the current project (.ipj) file. If not, it is important to either open the correct .ipj file and make it current either in Autodesk Inventor or the standalone project editor, or to browse to it in the Pack and Go dialog box in the Project File field.
If the Missing File dialog box is displayed, click the Set Project button. Select the project to use for resolving referenced file locations. Click Open, and then click Start to begin the search. You can click Cancel on the Find Missing File dialog box to cancel the action and display the Pack and Go dialog box without referenced files. You can use Design Assistant to copy an entire assembly file (.iam), including the referenced drawing file (.idw).
All changes are saved and new files (test2.iam and test2.idw) are created. NOTE The newly created (or copied) drawing file (test2.idw) is referenced only to the newly created (or copied) assembly file (test2.iam). All changes made in the original assembly file (test1.iam) is reflected only in the copied test2.idw that references it. Occasionally, annotations for a referenced file of a subassembly may not be visible in a drawing view after you use Design Assistant to move or copy.
You can move or copy the folder containing the project file, browse to and activate the copied project file in the project editor, and then use the design files immediately after you copy them. If one or more of the previous conditions are not met, edit the destination project (.ipj) to specify the new paths for each of the copied folders. Consider using Pack and Go when copying an entire project. You can create a zipped copy on a CD-ROM, for example, and send it to a customer, vendor, or client.
The deleted file is temporarily placed in the Recycle bin and can be restored to its original location if necessary. When you empty your Recycle bin, the file is permanently lost. Changing File Structure Projects often grow over time and the file structure must change to accommodate the complexity. You can more easily change the file structure if you plan it before you start the project, laying it out so that the data is portable.
■ If needed, create a subfolder named Tube_Pipe_Content. Create a library named Tube_Pipe Content. Configure the tube and pipe library to place standard tube and pipe components in that library. 3 Add the paths to the new subfolders of the project as Frequently Used Subfolders. They are listed in the Locations box of the file Open dialog box. 4 For safekeeping, make a copy of all of the data files, before you move them to a new directory or delete old folders.
all engineering and related data, providing design team members with a central and secure collaborative environment. Autodesk Vault is the preferred data management system for Autodesk Inventor. Its capabilities extend beyond the data management scope of projects. After you install Autodesk Vault, use the Project Wizard to create a vault project. Specify a personal workspace where you create and edit files. In addition, you also specify the vault server, its name and the virtual folder stored on the server.
Index A active analysis 100 active project 111, 115 adaptive work planes 158 Analyze Interference tool 173 angle constraint 150 Application Options dialog box 3 assemblies 134–137, 140, 145, 153–154, 157, 160, 165, 173, 178 animating 178 bills of material (BOMs) 140 browser 135 components, creating in place 157 constraining 134, 145, 154 constraints, viewing 153 interference, checking 173 restructuring 137 structures 136 subassemblies, creating 160 tips for working with 140 visibility of components 136 work
degrees of freedom 178 deleting from sketches 36 editing in assemblies 148, 154 insert 152 mate 148 motion, adding 152 showing 33, 153 sketch 32–34 tangent 147, 151 tips for creating 37 tips for managing 154 Content Center 265–271 configuration 266, 271 editor 269 library 266 permissions 265 place component 268 publishing 270 using 267 Content Library in Autodesk Inventor 127 coordinate system 23, 133 assembly 133 sketch 23 Create In-Place Component dialog box 142 Create Parts List dialog box 242 crop opera
tips for creating 45 types, changing 39 displays, graphics window 139 Document Settings dialog box 3 DOF (degrees of freedom) 175 draft styles, Primary Zebra 100 draft views in drawings 220, 232 draft, analyzing 100 drawing dimensions 244 Drawing Resources folder 210 drawing sheets, printing 263 drawing view types 221 drawings 203–205, 211–212, 214, 216, 220, 222, 232, 234, 236, 243, 249–250, 253, 257, 259–260, 262– 263 borders 212 creating 205 dimensions, creating 243, 257 model dimensions, editing 205 mod
old versions, restoring 281 opening in projects 129, 282 proxy 112 referenced locations, finding 115 resolving links 276, 279 templates 2 Files 285 moving and copying 285 Fillet dialog box 79 fillet features 69, 73, 79 folders in projects 113 G Gaussian curvature analysis 100 General Dimension tool 239 geometry, sketch 21 graphics window displays, controlling 139 grid displays, setting 25 Ground Shadow tool 11 grounded components 144 grounded work points 108 H hatch patterns, editing 235 Help system 16–17
O occurrences in patterns, suppressing 94, 99 Open File dialog box 2 Open New File dialog box 2 Open Version dialog box 282 Options dialog box 3 options in projects, setting 123 Ordinate Dimension Set tool 239 Ordinate Dimension tool 239 orthographic camera view 11 P Pack and Go function 286 Pan tool 9 parametric dimensions 38 parent/child parts in models 54, 135 part modeling environment 54 part models 2, 7, 11, 53–55, 58, 66, 69, 90, 205, 244 creating 2, 54 displaying 11 editing in drawings 205, 244 modi
relative paths 113 Resolve Link dialog box 277, 279, 291 restructure assemblies 137 Retrieve Dimensions tool 241, 254 Revision table tool for annotations 241 revolve features 58 Revolve tool 60 rib and web features 58 Rib tool 64 root folders in projects 113 Rotate tool, 3D 10 S SAT files, importing 15 search order in projects 278 search paths 123–125, 129, 275 Autodesk Mechanical Desktop parts 125 library 124, 129 projects, setting 275 workspaces 123 section views in drawings 220, 225 semi-isolated mode 1
deleting 233 editing 221, 253 modifying 232 moving 211, 236 rotating 236 visibility of assembly components 136 W Wireframe Display tool 11 work features 105–107, 109, 158, 165 adaptive planes 158 axes 106 in assemblies 165 modifying 109 planes 106 points 107 workgroups 113 workspaces 113, 123 locations 113 search paths 123 Z zebra analysis 100 Zoom tools 8 Index | 299
