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 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.


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

Import annotations Select Import annotations to select types of annotations to be imported from referenced part or assembly documents.
Select annotation import options:
  • Design annotations
  • DimXpert annotations
  • Include items from hidden features
  • 3D View annotations

Reference Configuration Options

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 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.

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.


  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.


  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

Select to remove outline of closed sketch used to create crop view.

Selected Cleared
Jagged outline

Select to include a jagged outline of the crop view.

Move the slider to adjust Shape Intensity.


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 Lets you display the bend direction.
Supplementary Angle Lets you display the supplementary bend angle.
Complementary Angle Lets you display the complementary bend angle.
Bend Radius Lets you display the bend radius.
Bend Order Lets you display the bend order.
Bend Allowance Lets you display the bend allowance.

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.

Display Style

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.

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 set whether to use the specified color or a color slightly different than 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


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.

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 (it shows precisely what is visible and what is invisible.)
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.

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

Exclude from automatic update Excludes the selected drawing views from automatic updates that occur if the drawing is open, Automatic view update is selected, and you save changes to the model.

More Properties

Define Drawing View Properties.