To Insert a Half View
Half views cut the model at a plane, erasing one portion of it, and displaying the rest.
1. Open a drawing with one or more views.
2. Double-click an existing view. Alternatively, select a view, right-click and click Properties on the shortcut menu. The Drawing View dialog box opens.
3. Click the Visible Area category. The Visible area options display in the dialog box.
4. Select Half View from the View visibility list. The options for defining the view area display.
5. Select the reference that will divide the view. The cutting plane may be a planar surface or a datum, but it must be perpendicular to the screen in the new view. The selected reference highlights and is listed in the Half view reference plane collector.
6. Define which half of the model to display by clicking the single red arrow, which displays from the reference plane pointing toward the side that will be displayed. The arrow will be displayed just after a planar surface or datum is selected or after the 
is clicked. The view itself will not change until you click Apply or Ok. The arrow is no longer displayed.
is clicked. The view itself will not change until you click Apply or Ok. The arrow is no longer displayed.7. Using the Symmetry line standard list, define how to indicate the split in the half view:
◦ No line
◦ Solid line
◦ Symmetry line
◦ Symmetry line ISO
◦ Symmetry line ASME
8. You can specify a plane parallel to the screen and exclude all graphics behind it by clicking Clip view in Z-direction and select an edge, surface, or datum plane clipping reference that is parallel to the view. When you perform Z-Clipping in a view, keep in mind the following:
◦ If the reference for the clipping plane cannot be regenerated, Z-Clipping does not take effect for the view (an error message appears).
◦ The Z-Clipping of a detailed view is always the same as that of its parent. You cannot modify it individually.
9. To continue defining other attributes of the drawing view, click Apply and then select the appropriate category. If you have completely defined the drawing view, click OK.
 | Each half view can display its own symmetry line differently. You can format the half view line using the half_view_line Detail option. When changing a view to half view, the default symmetry line standard to use in the view will be decided by the above Detail option value. |