Chapter 21: Working with Drawing Views
Tip
The best way to create this view is to either create two configurations used exclusively for the Alternate
Position View or to have two configurations where you know that parts will not be moved, suppressed, or hid-
den. The main idea is that you need to ensure that these configurations remain in the same position or are
changed intentionally, knowing that it will alter this drawing view. n
To delete an Alternate Position View, select it in the drawing FeatureManager, and press Delete.Pre-defined View
Pre-defined Views are discussed in depth in Chapter 20, and are primarily used as views on draw-
ing templates.
Empty View
Empty Views are just that — empty. The reasons for creating an Empty View can include making a
view from a sketch, making a schematic from blocks, or combining several elements — such as
blocks, sketches, imported drawing geometry, annotations, and symbols — into an entity that can
be moved as a group on a drawing.
Custom View
You can create Custom Views by orienting the view in the model document and saving the view.
Remember that views can be saved in the View Orientation window, which you can access by press-
ing the spacebar. Custom Views are placed on the drawing using the Named View functionality.While not appropriate for showing dimensions, views using perspective are most useful for picto-
rial or illustrative views. The only way to get a perspective view on a drawing is to save a custom
view in the model with perspective selected. You can access the Perspective option by choosing
View ➪ Display ➪ Perspective, and you can edit the amount of perspective by choosing
View ➪ Modify ➪ Perspective.Relative View
The Relative View enables you to create a view that does not necessarily correspond to any of the
standard orthogonal views or named views. This type of view is very similar to using the Normal
To tool. First select the face that is to be presented square to the view, and then select the face that
represents the top of the view. When this view type is initiated, SolidWorks opens the 3D model
window to allow you to select the faces needed to define the view.
This type of view is particularly useful when a part has a face that is at an odd angle to the standard
planes of the part. It is in some ways similar to the Auxiliary View, except that in the Auxiliary
View you cannot select which face is the top.