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
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. Finally, click in the drawing view to specify the location of each
break line.
Draft Views
A draft view is a special view in a drawing that does not require a representation
of a 3D model. A draft view has one or more associated sketches. You can
place a draft view and construct a drawing without an associated model. You
can also use a draft view to provide detail that is missing in a model.
When you import an AutoCAD file to an Autodesk Inventor drawing, the data
is placed in a draft view. Dimensions, text, and other annotations are placed
on the drawing sheet and geometry is placed in the associated sketch.
Modifying Views and Sections
You can constrain the relative positions of two views. One of the views acts
as the base view. If the base view moves, the aligned view also moves. If a
view is aligned vertically, the position of that view relative to the base view
is constrained to points along the Y axis of the base view. Horizontal alignment
constrains the position to points along the X axis of the base view.
An in-position alignment establishes the relative angular position between
the view and the base view. An auxiliary view is an example of in-position
alignment. The view is constrained to maintain the alignment as the base
view is repositioned.
To remove the constraints between views, select the view from which to
remove the alignment. Right-click, and then select Alignment ➤ Break.
You can restore broken alignments to views. Select the view to align, right-click,
and then select Alignment ➤ Horizontal, Vertical, or In Position. Click the
base view to set the alignment.
NOTE To place a section view without an alignment constraint, press and hold
the CTRL key as you place the view.
232 | Chapter 13 Creating Drawing Views