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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.

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 tool_Make_Drawing_Standard.gif.
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 all selected 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

Reference Configuration Options

PM_config_Named_View.gif 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 state In assemblies and multibody parts that contain an exploded view, select to display a drawing view in the exploded 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.

Orientation

  Create multiple views Lets you select more than one view to insert.
  View orientation Displays standard view orientations of the model:
  • pm_orient_top.gif Top
  • pm_orient_front.gif Front
  • pm_orient_right.gif Right
  • pm_orient_left.gif Left
  • pm_orient_bottom.gif Bottom
  • pm_orient_back.gif Back
  • pm_orient_isom.gif Isometric
  Annotation view Displays annotation views if they were created in the model.
PM_orientation.gif 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.

Display State

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

The hide/show display_pane_column_hideshow.gif display state is supported by all display styles. Other display states (display mode display_pane_column_display_mode.gif, color display_pane_appearance.gif, etc.) are supported by Shaded with Edges Tool_Shaded_With_Edges_View.png and Shaded modes Tool_Shaded_View.png only.

Bend Notes

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

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

Flat Pattern Display

For sheet metal flat patterns only.

PM_angle.gif 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.

tool_Wireframe_View.png Wireframe Displays all edges
Tool_Hidden_Lines_Visible_View.png Hidden Lines Visible Displays visible and hidden edges as specified in Line Font Options.
Tool_Hidden_Lines_Removed_View.png Hidden Lines Removed Displays only edges that are visible at the chosen angle; obscured lines are removed.
Tool_Shaded_With_Edges_View.png 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.

Tool_Shaded_View.png Shaded Displays items in shaded mode.

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 Tool_Options_Standard.gif > 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 block_Base_Point.gif to set the origin in the file and click Save View As DXF/DWG Tool_Save_As_Standard.gif. Set the options in the Save As dialog box.
Export only model geometry ignores other sketch annotations that are associated with the selected view.

More Properties

Define Drawing View Properties.



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