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.


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

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

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.

New name Edit the flat pattern configuration name that appears in the box. The flat pattern configuration name appears under the configuration name of the model in the ConfigurationManager.


  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 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.


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.
See through transparent components Displays transparent components as transparent in drawing views.

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.

Recommendation: 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 handle 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.