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 Select Planar to define a section view by selecting one, two, or three planes or planar faces.
Zonal Select Zonal to define a section view by selecting one or more zones. Zones are defined by the intersection of the selected plane or face and the bounding box of the model.
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 Option

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

Offsets can be perpendicular to:

  • Reference Plane

    Values are calculated normal to the currently oriented section plane.

  • Selected plane

    Values are calculated 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. This property has no effect while the PropertyManager is open. 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 Select 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 selected and Keep cap color cleared

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

Selected bodies or components

Selected bodies Select bodies in the graphics area or the flyout FeatureManager design tree to add them to Selected bodies.
Selected components Select components in the graphics area or the flyout FeatureManager design tree to add them to Selected components.
Components or bodies to include or exclude from the section view Lists components or bodies that you select from the graphics area or the flyout FeatureManager design tree. To delete all assemblies or parts, right-click, and click Clear Selections. To remove a body or component, select it in the graphics area or the FeatureManager design tree, or right-click it in the selection list, and click Delete.
Exclude selected Available when you click Selected bodies or Selected components. The selected bodies or components are not sectioned. All other bodies or components are sectioned.
Include selected Available when you click Selected bodies or Selected components. The selected bodies or components are sectioned. Other bodies or components are not sectioned.
Enable selection plane Available when you click Selected bodies or Selected components. 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.

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

Select components to leave uncut in the graphics area or in the FeatureManager design tree. To remove a component from the list, select the component again, or select it in the Excluded components list and click Delete.

Auto hatching

Select to automatically adjust for neighboring components with the same crosshatch pattern. The hatch patterns alternate when sectioning an assembly.

Exclude fasteners

Select to exclude 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.