2009
Table Of Contents
- Contents
- 1 Introducing Autodesk Inventor
- 2 Creating Sketches
- 3 Working with Sketched Features
- 4 Creating and Editing Placed Features
- 5 Creating and Editing Work Features
- 6 Using Projects to Organize Data
- 7 Managing Assemblies
- 8 Placing, Moving, and Constraining Components
- 9 Creating Assemblies
- 10 Analyzing Assemblies
- 11 Using Design Accelerator
- 12 Setting Up Drawings
- 13 Creating Drawing Views
- 14 Annotating Drawings
- Annotation Tools
- Using Styles to Format Annotations
- Working with Tables
- Creating Dimensions In Drawings
- Controlling Dimension Styles
- Placing Center Marks and Centerlines
- Adding Notes and Leader Text
- Using Hole and Thread Notes
- Working with Title Blocks
- Working with Dimensions and Annotations
- Printing Drawing Sheets
- Plotting Multiple Sheets
- Tips for Annotating Drawings
- 15 Using Content Center
- 16 Autodesk Inventor Utilities
- Index
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. In subsequent
projected views, only those model dimensions not shown in the base view
are displayed. If it is necessary to move a model dimension from one view to
another, right-click the dimension in the first view and select Move. Click the
second view to move the dimension. As an alternative, you can add a drawing
dimension to the second view.
NOTE If you choose to change the model dimensions in the drawing, make only
minor changes to single dimensions. If there are significant changes, or if you need
to modify dimensions that are referred to by other dimensions, open the part and
edit the sketch or feature there.
To avoid accidentally modifying a standard part, you can prevent the editing
of driven dimensions in read-only parts that are referenced to the drawing
file.
If you change the size of a part that is used multiple times in an assembly or
is used in multiple assemblies, all occurrences of the part are resized. Check
other assemblies to see if the changed size causes interference.
Drawing Dimensions
Drawing dimensions are unidirectional. If the part size changes, the drawing
dimension updates. However, changing a drawing dimension does not affect
the size of a part, unless you specified differently when you installed Autodesk
Inventor. Usually, drawing dimensions are used to document, but not to
control, the size of a feature.
You use the same tools to place drawing dimensions as sketch dimensions.
Linear, angular, radial, and diameter dimensions are all placed by selecting
points, lines, arcs, circles, or ellipses, and then positioning the dimension.
Constraints are inferred to other features as you place drawing dimensions.
Autodesk Inventor displays symbols that indicate the type of dimension being
placed. Visual clues are also used to position dimensions at fixed intervals
from the object.
244 | Chapter 14 Annotating Drawings