Model/Predefined/Empty/Drawing View PropertyManager

To open the PropertyManager:

• Insert or select a Model View, a Predefined View, or an Empty View in a drawing.
• Drag a model with annotation views into a drawing.

The properties available depend on the type of view that 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	Inserts projected views of the model after you insert the model view.

Import Options

Reference Configuration

	Configuration name	Select a configuration.
	Select Bodies	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 or model break state	In assemblies and multibody parts that contain an exploded or model break view, select to display a drawing view in the exploded or model break state.

Rename Configuration

For sheet metal flat patterns only.

Orientation

	Create multiple views	Select more than one view to insert.
	Standard views	Displays the standard view orientations of the model: Top Front Right Left Bottom Back Isometric
	Annotation view	Displays annotation views if they are created in the model.
	More views	Displays additional views such as Current Model View (if the model is open), Flat pattern, *Trimetric, and *Dimetric.
	Preview	Shows a preview of the model while inserting a view. Available when Create multiple views is cleared.

Mirror

Mirror view

Displays model, relative to model, and predefined drawing views as mirror views without creating the mirror components. Select Horizontal or Vertical. For example, Original view Mirror view - Horizontal Mirror view - Vertical

Crop View

For crop views only.

No outline	Removes outline of closed sketch used to create crop view. Selected Cleared
Jagged outline	Includes a jagged outline of the crop view. Move the slider to adjust Shape Intensity. Selected

Display State

For assemblies only. Select a display state of the assembly to place in the drawing.

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.

Bend Notes

For sheet metal flat patterns only. Select to display bend notes.

	Bend Direction	Displays the bend direction.
	Supplementary Angle	Displays the supplementary bend angle.
	Complementary Angle	Displays the complementary bend angle.
	Bend Radius	Displays the bend radius.
	Bend Order	Displays the bend order.
	Bend Allowance	Displays the bend allowance.

Flat Pattern Display

For sheet metal flat patterns only.

	Angle	Displays 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.

Display Style

Wireframe	Displays all edges
Hidden Lines Visible	Displays visible and hidden edges as specified in Line Font Options.
Hidden Lines Removed	Displays only edges that are visible at the chosen angle; obscured lines are removed.
Shaded With Edges	Displays items in shaded mode with hidden lines removed. You can specify a color for the edges, and specify whether to use the specified color or a color slightly different from the model color in the System Colors Options. High quality or Draft quality available when you select Shaded With Edges. Select High quality and Shaded With Edges to prevent far side edges from displaying on the near side face of a model.
Shaded	Displays items in shaded mode.

Broken-out Section

For drawing views that include broken-out section views only.

Scale hatch pattern

Applies the view's scale to hatches within the broken-out section view. Selected Cleared

Scale

Select a scale for the drawing view.

Dimension Type

Define Dimension Type.

Cosmetic Thread Display

The following settings override the Cosmetic thread display option in Options > Document Properties > Detailing.

Save View As

Expand Save View As to save a drawing view as a Dxf or Dwg file. Optionally, drag the point manipulator to set the origin in the file and click Save View As DXF/DWG . Set the options in the Save As dialog box.

Export only model geometry ignores other sketch annotations that are associated with the selected view.

Automatic View Update

More Properties

Define Drawing View Properties.