Section View PropertyManager (Drawings)

To open the Section View PropertyManager:

Create a section view in a drawing and click Edit sketch in the PropertyManager, or select an existing section view.

Cutting Line

Flip direction You can also reverse the cut direction by double-clicking the section line.
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.
Slice section Shows only the faces cut by the section line.
  Complete section

Partial section

Slice section

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.
Randomize scale
Randomizes the hatch scale for the same material in the drawing view. Clear this setting to keep the scale identical for all hatches of multiple parts of the same material.
Scale hatch pattern
Applies the view's scale to hatches within the view.
Selected Cleared
Emphasize outline
Emphasizes the outline of cut faces.
Selected Cleared
Hide cutting line shoulders
Only available on view creation
Foreshorten view
Only available on view creation

Surface Bodies

Display surface bodies Shows a section view of surface bodies from a parent view of a model. You can apply annotations such as notes and dimensions to the cross section of the surface. This setting persists across sessions.
Cut surface bodies Shows only the intersecting line of a surface in a section view.

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 .
  • Select geometry, such as an edge or an axis, in the parent view for Depth Reference .
  • 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.

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 state is supported by all display styles. Other display states (display mode , color , etc.) are supported by Shaded with Edges and Shaded modes only.

Display Style

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

Click a display style.


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, enter 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 preset 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.

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

See Drawing View Properties.