SolidWorks 2011 Parts Bible - Matt Lombard [314]
Using thin features
Thin feature extrusions are sometimes used in place of ribs. Thin features do not have all the specialized options available with the Rib feature, but they do offer simplicity as the main attraction. Thin features can substitute for Rib features when the rib is a stand-alone rib that doesn't touch the side walls of the part. They can be used to sketch and extrude from the bottom of the rib or from the top. When extruding a thin feature with draft, the end (thickness) faces get drafted as well, which might cause a problem if you are trying to attach the rib to a wall. Extruding a thin feature down from the top of the rib can replace a plan view rib, but it will not enable you to break sketch rules like the plan view rib.
I personally prefer to use Rib features, except for free-standing ribs where you do not want the sides extended up to the next wall.
Using Draft
SolidWorks Draft is surprisingly powerful for as simple as it is. All the aspects of working with Draft could take up an entire chapter all on its own. I will try to hit the most important points in this brief synopsis. The Draft feature creates three types of draft:
• Neutral Plane draft. Drafts faces from a plane or planar face where the intersection of the drafted face and the neutral plane is what the draft pivots about.
• Parting Line draft. Drafts faces pivot edge on selected edges.
• Step draft. Drafts faces from parting line edges and can create a step at the parting line. (similar to pivot draft in other software).
Figure 24.11 shows the PropertyManager of the draft feature, including the DraftXpert, which is mentioned later in this section.
FIGURE 24.11
Draft and DraftXpert PropertyManagers
Neutral Plane draft
The workflow for Neutral Plane draft is as follows:
1. Select Neutral Plane — plane or planar face at which the intersection of the drafted face does not move. The direction of pull is always normal to the Neutral Plane.
2. Set the draft angle — how many degrees from the direction of pull vector selected faces should be tilted. This is not a cumulative angle, so applying 3 degrees of draft to a face that is already drafted 5 degrees results in 3 degrees rather than 8 degrees.
3. Select the Direction — one side or the other side of the Neutral Plane. The arrow points in the direction of decreasing material. If you are drafting a surface body, the “decreasing material” concept does not apply, so you just have to experiment to see which direction is the one you intend. The Draft feature does not have a preview option.
4. Select faces to draft — use face propagation options. Inner/Outer faces refer to inside or outside loops around the Neutral Plane face. All means all faces that have an edge on the Neutral Plane face.
Parting Line draft
The workflow for Parting Line draft is as follows:
1. Select a direction of pull — this can be an edge, axis, sketch line, plane, or planar face. You also have to set the direction to positive or negative along the selected direction.
2. Select the parting lines — these are edges of the faces you want to draft. The parting line edges remain stationary while the rest of the face tilts. Along with the parting line selection, you may also need to use the Other Face option. Every edge is adjacent to two different faces. The Draft feature automatically selects the face it thinks you want to draft, but it does not always get it right. Other Face enables you to intervene when the automatic selection is incorrect.
3. Set the draft angle — remember that you can use the Allow Reduced Angle option if you need to.
Step draft
The most complex of the types of draft that SolidWorks creates is the Step draft. Step draft is used on non-planar parting lines when Parting Line draft would cause the drafted faces to be split into multiple faces.
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