Section View PropertyManager (Models)

This PropertyManager controls section views in part and assembly documents.

To open the Section View PropertyManager:

Click Section View (View toolbar) or View > Display > Section View.

Drawing Section View

The next available section view letter appears automatically. You can change it.

Section Method

Planar Defines a section view when you select one, two, or three planes or planar faces.
Zonal Defines a section view when you select one or more zones. Zones are defined by the intersection of the selected plane or face and the bounding box of the model.

To set bodies and components as transparent, you must select Zonal for the section method.

Planar section method with 1 section plane selected Planar section method with 2 section planes selected
Planar section method with 3 section planes selected Zonal section method

Section Options

Offset Method Indicates the plane from which offset values are calculated.

Offsets can be perpendicular to:

Reference plane

Calculates values normal to the oriented section plane.

Selected plane

Calculates values normal to the plane that you select in Section 1.
Show section cap Displays a section cap with the color specified in the Edit Color box. Clear this option to see inside the model.
Keep cap color Continues to display the section cap with the color specified in the Edit Color box after you close the Section View PropertyManager. The table below shows the display results after you close the PropertyManager for an assembly.
Graphics-only section Provides faster results with limited selection capabilities.
You cannot select a sectioned face or edge. Retain the section cap color in a graphics-only section view. Pixels that lay within the same plane as the section plane or face are not hidden.

Section 1, Section 2, Section 3

Section 3 appears after you select Section 2. Use Section 2 and Section 3 to section the view with additional planes or faces.

  Section plane/face Specifies a plane or face, or click Front Plane , Top Plane , or Right Plane , to create the section view. Reverse Section Direction changes the direction of the cut.
Offset Distance Specifies an offset distance for the section cut from the plane or face.
X Rotation Rotates the reference section along the X-axis.
Y Rotation Rotates the reference section along the Y-axis.
  Edit Color Changes the color of the section view.

Section views hidden Show section cap and Keep cap color selected

Show section cap and Keep cap color cleared Show section cap selected and Keep cap color cleared

Section by Body or Component

Components or bodies to include or exclude from the section view Lists selected components or bodies.
Exclude selected Does not section the selected bodies or components. All other bodies or components are sectioned.
Include selected Sections the selected bodies or components. Other bodies or components are not sectioned.

Transparently Section Bodies or Components

  Components or bodies to include or exclude from the transparent sectioning Lists selected components or bodies.
  Exclude selected Does not change the transparency of the selected bodies or components.
  Include selected Changes the transparency of the selected bodies or components.
Section Transparency Specifies the amount of transparency. Enter a value or move the slider.
Enable selection plane Shows a selection plane with the triad at the center of the plane. Use the triad to control the position and angle of the selection plane.

Available when you click Section by Body or Component or Transparently Section Bodies or Components.

Preview

Shows a graphics-only preview of the section results based on the section plane location and the components or bodies that you select in Selected components or Selected bodies. Hides the section planes, reference planes or faces outlines, and the selection plane.

Save

Click to save the section view, then specify the following options in the Save As dialog box and click Save:

View orientation Saves the section view as a named view in the Orientation dialog box. The view is not available in drawings.
Drawing annotation view

Creates an annotation view for the section view and includes the section view on the View Palette in drawings. The name of the section view appears under Annotations .

When you save with this option, the Section Annotation View Props dialog box appears to let you specify components to leave uncut. Specify the following options and click OK.

Excluded components

Leaves selected components uncut.

Auto hatching

Automatically adjusts for neighboring components with the same crosshatch pattern. The hatch patterns alternate when sectioning an assembly.

Exclude fasteners

Excludes fasteners from being sectioned. Fasteners include any item inserted from SOLIDWORKS Toolbox except for structural members. You can designate any component as a fastener.
To designate any component as a fastener, open the component and click File > Properties. In the dialog box on the Custom tab, select IsFastener in Property Name, and enter 1 for Value/Text Expression.
View name Enter a name for the section view.