Page 163 - Mastering SolidWorks

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132 CHAPTER 4 Creating Simple partS and drawingS

5. Dimension the angled line such that it is 2.025 inches from the first line.
6. Use the same technique as in step 1 to make a closed loop, and extrude the feature using
the Through All end condition so that it will always match the previous extrusion.

Using the Hole Wizard
The next features that you will apply are a pair of counterbored holes. SolidWorks has a special
tool called the Hole Wizard that you can use to create common hole types. The Hole Wizard
helps you create standard hole types using standard or custom sizes. You can place holes on any
face of a 3D model or constrain them to a single 2D plane or face. A single feature created by the
Hole Wizard may create a single hole or multiple holes, and a feature that is not constrained to a
single plane can create individual holes originating from multiple faces, nonparallel faces, and
even nonplanar faces (holes may go in different directions). All holes in a single feature that you
create by using the Hole Wizard must be the same type and size. If you want multiple sizes or
types, you must create multiple Hole Wizard features.
To apply counterbored holes to your part, follow these steps:
1. Select the face that the groove feature was created on, and click the Hole Wizard tool on
the Features toolbar. Then set the hole to Counterbored, the Standard to ANSI Inch, the
type to Socket Head Cap Screw, the size to one-quarter, and the end condition to Through
All, as shown in Figure 4.22.
2. Click to select the Positions tab at the top of the PropertyManager. This is where you place
the centerpoints of the holes using sketch points. It is often useful to create construction
geometry to help line up and place the sketch points. Make sure the plane or face that the
holes originate from is selected in the Positions tab.
3. Draw two colinear construction lines, horizontally across the part, with Coincident
relations to each side. Select both lines, and give them an Equal relation. The point of this
step is to use parametric relations to evenly space holes across the part without dimen-
sions or equations. Refer to Figure 4.23.
TIP although several methods exist to make multiple selections, a box or window selection technique
may be useful in this situation. if the box is dragged from left to right, only the items completely
within the box are selected. if the box is dragged from right to left, any item that is at least partially in
the box is selected. Selecting the common point of the two lines applies an equal relation.

4. Place sketch points at the midpoint of each of the construction lines. If there is a sketch
point other than the two that you want to make into actual holes, delete the extra points.
Dimension one of the lines down from the top of the part, as shown in Figure 4.23. All the
sketch relation icons are displayed for reference. Click OK to accept the feature after you
are happy with all the settings, locations, relations, and dimensions.