SolidWorks 2011 Parts Bible - Matt Lombard [187]
For most people who have learned SolidWorks software prior to the 2010 version, it may already be instinctive 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.
Understanding the 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.
Understanding the 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-planar. 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 position on a cylinder, you need to follow these steps:
1. Begin with a circle with a diameter of 1 inch, drawn on the Top plane and extruded using the Mid-plane option 1 inch.
2. Start the Hole Wizard without any pre-selection, either through the Features toolbar 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 13.4.
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.
Figure 13.4
The Hole Wizard settings for the socket head cap screw
5. Click the cylindrical surface of the part. The surface appears orange when you move the cursor over it to indicate that an OnSurface sketch relation will be created between the sketch point and the cylindrical surface.
6. The hole should be positioned from one end of the cylinder. Using the SmartDimension tool, click one flat end face of the cylinder and the sketch point. Place the dimension and give it a value of .300 inches, as shown in Figure 13.5.
Locating the point angularly around the cylinder is more difficult. You can use several methods to do this, but this example shows one using construction sketch geometry.
Figure 13.5
Dimensioning the 3D Placement sketch point
Tip
To force a 3D dimension to have a certain orientation, dimension from a plane or planar face rather than from an edge, vertex, or sketch entity. A dimension from a plane is always measured in a direction perpendicular to the plane, but a dimension from a line or point is always measured by the shortest distance between the entities. Two-dimensional sketches can force dimensions to be horizontal or vertical, but 3D sketches cannot.
7. With the Line tool activated while still in the 3D sketch, Ctrl+click the flat end face that the previous dimension referenced. This moves the red “space handle” origin to the selected face and