SolidWorks 2010 Bible

Chapter 26: Modeling Multi-bodies

Creating Multi-bodies

In the first section in this chapter, I raised the questions of if or when multi-bodies should be used,

and in the second section, I raised the question of why multi-bodies should be used. In this sec-

tion, I simply ask, or rather answer, how they should be used.

Using disjoint sketches

The easiest way to create multiple bodies is to simply create what SolidWorks classifies as multiple

disjoint closed contours. What that means is simply two circles or rectangles that do not touch or

overlap. If these are created in the same sketch, then when extruded, they will create as many bod-

ies as there are closed loops in the sketch.

If the part has an existing solid, then creating a sketch that does not touch the solid can also create

a separate body. You cannot make Multiple Thin features in a single sketch. This is presumably

because the interface has no way to identify different thickness directions for different open pro-

files. This holds true whether or not the Multiple Thin features create multiple bodies.

If a solid feature other than a mirror or pattern touches a solid body, then the new and the old

bodies will be merged into a single body.

Turning off the Merge Result option

You can prevent a feature from automatically combining with other bodies by deselecting the

Merge Result option. This holds true between features, but not across all bodies in a part. For

example, if an extrude feature uses the Merge result option, all the bodies that it touches become

merged together, but if the original extrude feature does not touch a body, it will not be merged.

This option is shown in Figure 26.15 and is found on all features that create new solid bodies

except for the Patterns, Rib, and Move/Copy Bodies features.

FIGURE 26.15

The Merge result option