Chapter 4: Creating Simple Parts, Assemblies, and Drawings
FIGURE 4.10
The Hole Wizard Hole Specification interface- Next, 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. - Draw two 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 evenly space holes across the part without dimensions or equations.
Tip
Although several methods exist to make multiple selections, a box or window selection technique may be use-
ful 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. n
Tip
SolidWorks displays an error if you try to place a sketch point where there is an existing sketch entity endpoint.
If you build construction geometry in a sketch and want to place a sketch point at the end of a sketch entity,
you have to create the sketch point to the side where it does not pick up other incompatible automatic sketch
relations, and then drag it onto the endpoint. n
- Place sketch points at the midpoint of each of the construction lines. If there is
another 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 4.11. All the sketch relation icons display for reference. Click OK to accept the
feature once you are happy with all the settings, locations, relations, and dimensions.