Page 259 - Mastering SolidWorks

|
understanding Fillet tyPes 231

◆ The cutting tool must be definable with a revolved feature.
◆ The cutting tool must be made of simple analytical faces (sphere, torus, cylinder, and cone;
no splines).

◆ You cannot use a guide curve with a solid profile cut (because you cannot control alignment).
◆ The cut can intersect itself, but the path cannot cross itself.
You can create many useful shapes with the solid-profile-cut sweep, but because of some of
the limitations I’ve listed, some shapes are more difficult to create than others. For these shapes,
you might choose to use regular Cut Sweep features.

Workflow
Use the following general steps to create Sweep features:
1. Create the path first. It may be tempting to create the profile first, but as a general rule,
things work out better if you make the path first.
2. Create guide curves. Again, these work out better if you create them before the profile.

3. Create the profile (sweep cross section) and relate it to the path with a Pierce sketch
relation. Select a point in the sweep profile that you want to be driven down the path, as a
bead follows a string.

4. Make sure that, as the profile is driven down the path (with the profile sketch plane
maintaining its original relationship with the path), the profile has the flexibility to change
the way it needs to change. The sketch is reevaluated at each point along the path. Use
relative relations (parallel, perpendicular, and so on) instead of absolute ones (horizontal,
vertical, or fixed).
5. Start the Sweep feature from the toolbar or menu. All sketches must be closed.

6. Select the profile first and then the path. SolidWorks automatically toggles from the profile
selection box to the path selection box as soon as a profile is selected, so take advantage of
this automation to help you work quickly. Note that for circular profiles centered on the
path, there is no longer a need to create a sketch.
CAUTION Pay attention to any tool tip warnings or error messages that come up. if you are unable
to select something, it is usually because something about that entity is inappropriate for the purpose
you are trying to assign to it.

7. Use the preview to check that it is performing the way you want. Click OK when you are
satisfied with the result.

Understanding Fillet Types

SolidWorks offers very powerful filleting functions. The Fillet feature comprises various types of
fillets and blends. Simple fillets on straight and round edges are handled differently from
variable-radius fillets, which are handled differently from the single or double hold-line fillet or
setback fillets. After you click the OK button to create a fillet as a certain type, you cannot switch
it to another type. You can switch types only before you actually create the feature.