Drawing View Properties

The Drawing View Properties dialog box provides information about the drawing view and its associated model.

To view and edit the Drawing View Properties:

  1. Do one of the following:
    • Right-click in a drawing view and select Properties.
    • From a drawing view PropertyManager, click More Properties.
  2. Edit properties and click OK.
  3. Click Update View tool_Update_View_Drawing.gif (Drawing toolbar) or Rebuild tool_Rebuild_Standard.gif (Standard toolbar).

View Properties

View information Read-only
Model Information Read only. Model information is not available for Detached views.
Configuration information Select one of the following:

Use model’s "in-use" or last saved configuration

Uses the active configuration of the open part or the saved configuration of the closed part.

Use named configuration

Uses a configuration that you previously created. For parent views (such as named and standard 3 views), select Use named configuration and optionally one of the Display States within that configuration.

Show in exploded or model break state

(Only for assemblies and multibody parts with exploded or model break views defined.) Uses a previously defined exploded or model break view.

Display State (For assemblies only.)

For some child views (such as detail and section views) you select display states only within the selected configuration, and therefore the Configuration information is unavailable. Other child views, such as projected and auxiliary views, allow full access to Configuration information.

To access only the list of display states for a parent or child view, select the view and use the Display State settings in the PropertyManager.


Link balloon text to specified table Assigns balloon numbers according to the selected BOM item numbers or weldment cut list item numbers. If you attach a balloon to a component that is not in the BOM configuration, the balloon number appears with an asterisk (*).


Show envelope (For assemblies only.) Displays assembly envelope components in the drawing view.
Align breaks with parent If the view is a break view that was created from another break view, select this check box to align the break gaps in the two views.
Display bounding box Displays the smallest rectangle in which the sheet metal flat pattern fits.
Display sheet metal bend notes Displays bend notes in the drawing.
Show fixed face Displays the fixed face that is defined in the flat pattern feature of the sheet metal part.
To view the fixed face, the flat pattern view must include a bend table.
Show grain direction Displays the grain direction that is defined in the flat pattern feature of the sheet metal part.
To view the grain direction, the flat pattern view must include a bend table.
Cartoon Displays cartoon settings (cartoon edge color and cartoon edge thickness) defined in Options > Document Properties > Model Display > Cartoon Edges.