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
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. You can
also specify that a dimension be driven. The dimension reflects the size of the
item but cannot be used to modify the size of the item.
When you add parametric dimensions to sketch geometry, you are applying
constraints that control the size and position of objects in the sketch. The
sketch is automatically updated when changes are made to the dimension
values.
Examples of dimensioned sketches are shown in the following illustration.
To create dimensions, use the General Dimension tool on the panel bar or on
the 2D Sketch panel toolbar. You select the sketch geometry you want to
dimension, and then click to place the dimension.
The selection of geometry and the placement of the dimension determine the
kind of dimension that is created. For example, if you select the edge of one
circle, a radial dimension is created. If you select the edges of two circles, a
linear dimension is established between their center points.
Place Dimensions
Parametric dimensions define the size of your sketch. After you add a
dimension, you cannot change the size of a line or curve by dragging it. In
Autodesk Inventor, you cannot apply double dimensions to a sketch.
38 | Chapter 2 Creating Sketches