SolidWorks 2010 Bible

Part IV: Creating and Using Libraries

sketches are still available and still useful, but because they are so much more difficult to use and

rarely truly needed, SolidWorks decided to change the default to a 2D sketch.

3D placement sketches are needed for Hole Wizard holes if you have a set of similar holes that are

placed on different levels or are always perpendicular to non-planar surfaces. If you need 3D place-

ment sketches, they are still available, but they are no longer the default.

For most people who have learned to pre-select a face before opening the Hole Wizard, this change

will have no effect. It will have a positive effect on new users and those who frequently forget to

pre-select.

Advantages and limitations of the 2D sketch

The main advantages of the 2D sketch method are the simplicity and completeness of the available

tools. Everyone knows how to manage 2D sketches, sketch planes, dimensions, and construction

geometry.

A limitation of the 2D sketch is that the holes that you create through this method are limited to a

single planar face, and the holes will all be perpendicular to that face. Sometimes this creates a

great limitation, while other times it does not matter.

Advantages and limitations of the 3D sketch

The obvious advantage of the 3D placement sketch is that it can put a set of holes on any set of

solid faces, regardless of whether they are at different levels, are non-parallel, or are even non-pla-

nar. This function offers multiple holes, multiple faces, and multiple directions. In situations where

that is what you need, nothing else will do.

A limitation of the 3D sketch is that it can be fairly cumbersome. Dimensions work very differently

in 3D sketches compared to 2D sketches. For example, to create and place a hole in a specific posi-

tion on a cylinder, you need to follow these steps:

1. Begin with a circle with a diameter of one inch, drawn on the Top plane and
   extruded using the Mid-plane option one inch.


2. Start the Hole Wizard without any pre-selection, either through the Features tool-
   bar or by choosing Insert ➪ Features ➪ Hole ➪ Wizard.


3. Set the interface to use an ANSI inch, one-quarter-inch, and counterbored hole for a
   socket head cap screw. Use a Normal fit and Through All for the End Condition, with a
   .100-inch head clearance (in the Options panel) and no custom sizing changes. These
   settings are shown in Figure 17.4.


4. Click the Positions tab, which is located at the top of the PropertyManager window.
   The interface asks you to select a face where you would like to put the holes or to select
   the 3D sketch option. In this case, click the 3D Sketch button.

Note
Be careful with clicking when the Point tool is turned on. For example, if you click in a blank space, the Point
tool places a point off the part. SolidWorks will try to use the point later to create a hole in empty space,
which usually causes an error. n