Model/Predefined/Empty/Drawing View PropertyManager
This PropertyManager opens when you:
The properties available depend on the type of view you select.
Part/Assembly to Insert
Select a document from Open documents or click Browse.
Thumbnail Preview
View a preview of the model selected in Open documents.
Options
Start command when creating new drawing. Available when inserting a model into a new drawing. The Model View PropertyManager appears whenever you create a new drawing except if you click Make Drawing from Part/Assembly 
.
Auto-start projected view. Allows you to insert projected views of the model after you insert the model view.
Import options
Select Import annotations to all selected types of annotations to be imported from referenced part or assembly documents.
Select annotation import options:
Reference Configuration
Configuration name 
. Lets you change drawing view configurations.
Select Bodies. Lets you select the bodies of a multibody part for inclusion in the drawing view. For flat patterns of multibody sheet metal parts, you can use one body per view.
Show in exploded state. In assemblies and multibody parts that contain an exploded view, select to display a drawing view in an exploded state.
Rename Configuration
For sheet metal flat patterns only.
New name. You can edit the flat pattern configuration name (which appears underneath the model configuration name in the model ConfigurationManager) that appears in the box.
Update. Click to update the configuration name in the Model View PropertyManager and in the model ConfigurationManager.
Orientation
Create multiple views. Lets you select more than one view to insert.
View orientation. Displays standard view orientations of the model:
-
Top 
-
Front 
-
Right 
-
Left 
-
Bottom 
-
Back 
-
Isometric 
Annotation view. Displays annotation views if they were created in the model.
More views 
. Displays additional views such as Current Model View (if the model is currently open), *Trimetric, and *Dimetric.
Preview (available when Create multiple views is cleared). Shows a preview of the model while inserting a view.
For assemblies only.
The hide/show 
display state is supported by all display styles. Other display states (display mode 
, color 
, etc.) are supported by Shaded with Edges 
and Shaded modes 
only.
Flat Pattern Display
For sheet metal flat patterns only.
Angle 
. Lets you display the drawing view at a specific angle.
Flip view. Flips the view horizontally.
Insert Model
For Predefined Views only. Select a model from the list under Part/Assembly of models open in the SolidWorks session or existing in the drawing, or click Browse and browse to a model file.
(Available only if
Display quality for new views
is set to Draft quality.) Select
High quality or Draft quality
to set the display quality of the model. If you select High quality, these options do not appear again.
Cosmetic Thread Display
The following settings override the Cosmetic thread display option from Options 
,
Document Properties, Detailing.
High quality. Displays precise line fonts and trimming in cosmetic threads. If a cosmetic thread is only partially visible, High quality shows only the visible portion.
System performance is slower with High quality cosmetic threads. It is recommended that you clear this option until you finish placing all annotations.
Draft quality. Displays cosmetic threads with less detail. If a cosmetic thread is only partially visible, Draft quality shows the entire feature.