Reference: Placeholder View reference

In the Placeholder View dialog, you can edit the properties of a placeholder drawing view in the Template contextual environment in the Drawing workspace in Fusion.

Templates

If you plan to reuse title blocks, borders, document settings, or sheet settings across multiple drawings, create a drawing template to save time and apply consistent standards. You can also create placeholder views and placeholder tables that automatically generate drawing views and part lists from the referenced design when you use the template to create a new drawing.

Access the Placeholder View dialog

On the toolbar in the Template contextual environment, click Placeholder Views > Base View Placeholder.

Alternatively, double-click any base view placeholder or projected view placeholder on the current sheet.

Reference (base view only)

Specify whether to create a new reference or associate the new base view with an existing reference.

Create New: Adds a new reference node to the browser.
Existing Reference: Associates the new base view to the selected existing reference node in the browser.

Note: You can only define the reference when you first create a base view. You cannot modify this setting for an existing view.

Representation (base view only)

Specify whether the base view will represent the static design assembly or an animation from a storyboard.

Assembly: Creates a base view that represents a full design assembly.
Component: Creates a base view that represents a single component in the design assembly.
Folded Component: Creates a base view that represents a folded sheet metal component.
Flat Pattern: Creates a base view that represents a flat pattern of a sheet metal component.
Storyboard: Creates a base view that represents an animation.

Note: You can only define the representation when you first create a base view. You cannot modify this setting for an existing view.

Appearance

Adjust the Orientation, Style, Scale, and Name settings.

Orientation (base view only)

Select one of the standard orthographic views or a named view.

Named View: Any named view defined in the design.
Top
Bottom
Left
Right
Front
Back
SW Isometric
SE Isometric
NE Isometric
NW Isometric

Style

Select the view style for the selected drawing view.

From Parent: Inherits the view style from the parent view. (Projected view, section view, and detail view only.)
Visible Edges
Visible Edges and Hidden Edges
Shaded
Shaded with Hidden Edges

Scale

Select the view scale from the dropdown menu or type a custom scale.

By default, Scale is set to Automatic.

Scale Formats	Examples
Ratio	1:48 and 1/4"=1'
Fraction	1/48 and 3/5
Decimal	.125 and 0.25

Edge Visibility

Adjust the Tangent Edges, Interference Edges, and Thread Edges settings.

Tangent Edges

Select a display style for tangent edges.

Full Length
Shortened
Off

Interference Edges

Check to display edges where components intersect.

Thread Edges

Check to display threads on threaded edges.