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Section View PropertyManager (Models)

This PropertyManager controls section views in part and assembly documents.

The Section View PropertyManager appears when you create or edit a section view in a part or assembly document.

Drawing section view

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

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.

  Reference Section Plane/Face Select a plane or face, or click Front PM_front.gif, Top PM_top.gif, or Right PM_right.gif, to create the section view. Reverse Section Direction PM_reverse_direction.gif changes the direction of the cut.
PM_Offset_Distance.gif Offset Distance Sets an offset distance for the section cut from the plane or face
PM_angle_x.gif X Rotation Rotates the reference section along the X-axis.
PM_angle_Y.gif Y Rotation Rotates the reference section along the Y-axis.
  Edit Color Changes the color of the section view.
  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.
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.

Save

Click to save the section view, then set 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 FM_annotations.gif.

When you save with this option, the Section Annotation View Props dialog box appears to let you specify components to leave uncut. Set 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 press 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 (nuts, bolts, washers, and so on) except for structural members. You can also 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 type 1 for Value/Text Expression.
  View name Type a name for the section view.


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