Chapter 4: Creating Simple Parts, Assemblies, and Drawings
Using Instant 3D
Instant 3D enables you to pull handles to create extrusions and to drag model faces to change the
size and location of features. Several feature types enable you to use arrows to adjust elements visu-
ally of parametric features and sketches. The function largely replaces and expands on the older
functionality called Move/Size Features. Figure 4.3 shows the arrows added by Instant 3D, which
are the handles that you pull on to create a solid from a sketch or edit an existing feature. Notice
also that you can make cut features with Instant 3D. In fact, you can change a boss feature into a
cut. I’m sure this is a neat sales demo trick, but I’m not aware of any practical application of chang-
ing a boss into a cut.
One of the attractive things about Instant 3D is that it allows you to make changes to parts quickly
without any consideration for how the part was made. For example, the cylindrical part was made
from a series of extrudes, with a hole cut through it with draft on the cut feature. The flat faces can
be moved, and the cylindrical faces offset. Behind the scenes, SolidWorks figures out which
sketches or feature parameters of which features have to be edited. This saves you time searching
the FeatureManager to figure out which features or sketches control a given face. As you work
through more complex parts, you will see how handy this can be at times. You can activate or
deactivate Instant 3D using the icon on the Features toolbar.Note
When combined with the sketch setting Override Dims on Drag, Instant 3D can be a powerful concepting tool,
even on fully dimensioned sketches. n
Contour selection
Contour selection enables you to select areas completely bounded by sketch entities for use with fea-
tures such as Extrude. For example, you could use a sketch like the number sign (#). Although it breaks
the rule and cannot be used with regular extrusion methods, you can use contour selection to select the
box in the center, which is completely bound by sketch elements.SolidWorks works best when the sketches are neat and clean, when nothing overlaps, and when no
extra entities exist. However, when you need to use a sketch that does not meet these criteria, you can
use this alternative method.Best Practice
I believe this feature was introduced into SolidWorks only to keep up with other CAD packages, not
because it is a great feature. I do not recommend using contour selection on production models. It is use-
ful for creating quick models, but the selection is too unstable for any data that you may want to rely on
in the future. The main problem is that if the sketch changes, the selected area may also change, or
SolidWorks may lose track of it entirely. n