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Section View PropertyManager (Drawings)

The Section View PropertyManager opens when you create a section view in a drawing and click Edit sketch in the PropertyManager, or when you select an existing section view.

Section Line

PM_line_settings.gif Flip direction You can also reverse the cut direction by double-clicking the section line.
PM_label.gif Label Edit the letter associated with the section line and section view.
  Font To choose a font for the section line label other than the document's font, clear Document font and click Font. If you change the section line label font, you can apply the new font to the section view label.

Section View

Partial section Creates a section view that is limited by the length of the section line if the line does not span the entire view.
Display only cut faces Shows only the faces cut by the section line.
  Complete section
drw_section_complete.gif
Partial section
drw_section_partial.gif
Display only cut faces
drw_section_surface.gif
Auto hatching Crosshatch patterns alternate between components in assemblies, or between bodies in multibody parts and weldments. The hatch patterns alternate when sectioning an assembly.
auto_hatch.gif
Display surface bodies Shows all surface bodies in the section view of the model.
Hide cutting line shoulders hide-cutting-lines.gif
Foreshorten view foreshortened1.gif
Toggle Alignment Click to change the alignment of the section view.
toggle-alignment-1.gif
toggle-alignment-2.gif

Section Depth

Lets you set the depth of a section view to a distance you specify. This control is only available for section views whose cutting line consists of a single line segment.

Distance section views apply to components, not features.
To set a distance, do one of the following:
  • Set a value for Depth PM_Offset_Distance.gif.
  • Select geometry, such as an edge or an axis, in the parent view for Depth Reference PM_deform_deform_pt.gif.
  • Drag the pink section plane in the graphics area to set the depth of the cut. All components between the section line and section plane will be shown in the section view.
Preview section_view_distance.gif

Import annotation from

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

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.

Display Style

Use parent style Clear to select style and quality settings different from those of the parent view.

Click a display style.

Select High quality or Draft quality to set the display quality of the model. This is available only when Display quality for new views is set to Draft quality. If you select High quality, these options do not appear again.

Scale

Use parent scale Applies the same scale used for the parent view. If you change the scale of a parent view, the scale of all child views that use the parent scale is updated.
Use sheet scale Applies the same scale used for the drawing sheet.
Use custom scale Applies a scale that you define. If you select User Defined, type a scale in the box below in the following format: x:x or x/x. Select Use model text scale to maintain the geometry used in the annotation views in parts.
The pre-set options in Use custom scale differ based on the dimensioning standard.

Dimension Type

Dimensions in drawings are either:
True Accurate model values.
Projected 2D dimensions.

The dimension type is set when you insert a drawing view. You can view and change the dimension type in drawing view PropertyManagers.

The rules for dimension type are:
  • SolidWorks specifies Projected type dimensions for standard and custom orthogonal views and True type dimensions for isometric, dimetric, and trimetric views.
  • If you create a projected or auxiliary view from another view, the new view uses Projected type dimensions, even if the original view used True type dimensions.

Cosmetic Thread Display

The following settings override the Cosmetic thread display option in Tools > Options > Document Properties > Detailing, if there are cosmetic threads in the drawing view.

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.

More Properties

See Drawing View Properties.



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