Chapter 7: Selecting Features
Understanding Instant 3D
Instant 3D is the tool that enables you to use the mouse to pull arrows or handles on the screen to
establish various dimension parameters for features like extrude, revolve, fillet, and even move
face. Not every dimension feature parameter is editable in this way. In some cases Instant 3D offers
you convenient ways to edit geometry without needing to figure out which feature is responsible
for which faces. With Instant 3D, you simply pull on handles on the screen to move and resize
sketches, and features including fillets.
Creating extrudes with Instant 3D .................................................................
Instant 3D enables you to select a sketch or a sketch contour and drag the Instant 3D arrow to create
either a blind extruded boss or cut. The workflow when using this function requires that the sketch
be closed. Instant 3D cannot be used to create a thin feature, and any sketch or contour that it uses
must be a closed loop. Sketches must also be shown (not hidden) in order to be used with Instant 3D.Note
Even though the words “Instant 3D” suggest that you should be able to instantly create 3D geometry from a
sketch that you may have just created, you do have to close the sketch first to get instant functionality. In this
case, Instant 3D requires the sketch to be closed (as in not active) and closed (as in not an open loop. n
Figure 7.6 shows Instant 3D arrows for extruding a sketch into a solid and the ruler to establish
blind extrusion depth. These extrusions were done from a single sketch with three concentric cir-
cles, using contour selection.Even after you create an extruded boss, you can use Instant 3D to drag it in the other direction to
change the boss into an extruded cut. When you do this, the symbol on the feature changes, but
the name does not.If you have a sketch that requires contour selection, SolidWorks automatically hides the sketch,
and to continue with Instant 3D functionality using additional contours selected from that sketch,
you will have to show the sketch again. This interrupts the workflow and makes using this func-
tionality less fluid than it might otherwise be. I only mention it here so that you are aware of what
is happening when the sketch disappears and the Instant 3D functionality disappears with it.If geometry already exists in the part, and you drag a new feature into the existing solid,
SolidWorks assumes you want to make a cut. However, maybe you are really trying to make a boss
that comes out the other side of the part. These heads-up display icons enable you to do this.
Options include boss, cut, and draft. The draft option enables you to add draft to a feature created
with Instant 3D.While Instant 3D can only create extruded bosses and cuts, it can edit revolves. If you create a
revolved feature revolving the sketch, say, 270°, the face created at the angle can be edited by
Instant 3D dragging. You can also drag faces created by any underdefined sketch elements.