SolidWorks 2010 Bible

Part I: SolidWorks Basics

FIGURE 4.5

Methods for creating the groove

With a thin feature cut, you sketch the centerline, and in the Cut-Extrude feature, select the Thin

Feature option and assign a width and depth. The option on the right is what is called a “nested

loop,” because it has a loop around the outside of the slot and another around the inside. Only the

material between the loops is cut away. The method in the center is a sweep where the cross sec-

tion of the slot is swept around a path to make the cut.

Another potential option could include a large pocket being cut out, with a boss adding material

back in the middle. Each option is appropriate for a specific situation. The thin feature cut is prob-

ably the fastest to create, but also the least commonly used technique for a feature of this type.

Most users tend to use the nested loop option (one loop inside another).

Relative size or direct dimensions ..................................................................

You can control the size of the groove as an offset from the edges of the existing part or you can

drive them independently. Again, this depends on the type of changes you anticipate. If the groove

will always depend on the size of the part, the decision is easy. If the groove changes indepen-

dently from the part, you will need to re-create relations within the sketch to reflect different

design intent. To create a groove, you can create a rectangle by offsetting the block shape and use

sketch fillets to round the corners.

Creating the offset .........................................................................................

You need to consider one more thing before you create the sketch. What should you use to create the

offset — the actual block edges or the original sketch? The answer to this is a Best Practice issue.

Best Practice
When creating relations that need to adapt to the biggest range of changes to the model, it is best to go as far
back in the model history as you can to pick up those relations. In most cases, this means creating relations to
sketches or reference geometry rather than to edges of the model. Model edges can be fickle, especially with
the use of fillets, chamfers, and drafts. The technique of relating features to driving layout sketches helps you
create models that do not fail through the widest range of changes. n