Inserting Model Items
You can insert dimensions, annotations, and reference geometry from
a model document (part or assembly) into a drawing.
You can insert items into a selected feature, an assembly component,
an assembly feature, a drawing view, or all views. When
inserting items into all drawing views, dimensions and annotations appear
in the most appropriate view. Features that appear in partial views, such
as detail or section views, are dimensioned in those views first.
To insert model
items into a lightweight drawing, the drawing view must be set to resolved.
Additionally, you can use the
hide/show pointer 
while the PropertyManager is active.
The left mouse button moves items, and the right mouse button hides/shows
items. When the Model
Items PropertyManager
is displayed, hidden model items are gray.
You can manipulate model items
in the following ways:
Delete.
Use the Delete key to delete model
items.
Drag.
Use the Shift key to drag model
items to another drawing view.
Copy.
Use the Ctrl key to copy model
items to another drawing view.
To insert existing model items
into a drawing:
Click Model Items 
on the Annotation
toolbar, or click Insert, Model Items.
You can also preselect views, features, or components to
which you want to add model items. You can select features or components
from the FeatureManager design tree or the graphics area.
Set options
in the Model
Items PropertyManager.
Dimensions are inserted for unabsorbed model sketches only
if the sketch is visible in the drawing. To insert dimensions for an unabsorbed
sketch, right-click the sketch in the FeatureManager design tree and select
Show before inserting the dimensions.
Dimensions belonging to an unabsorbed sketch are shown or hidden depending
on the state of Show or Hide.
Click OK 
.
When you insert dimensions, the software may provide feedback
to guide you. For example, if all the dimensions are already inserted
in a view, the software suggests a different view, if possible. If additional
dimensions cannot be inserted, the software informs you.
You can toggle
the visibility of individual reference geometry items. Right-click the
item, and select Hide or Show.
Imported annotations
display in the Annotations (Imported)
color; reference annotations (added in the drawing) are displayed in the
Annotations (Non Imported) color.
These colors are specified in Tools,
Options, System
Options, Colors.
Related Topics
Annotations Update
Inserting reference geometry into
drawings