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