SolidWorks 2011 Parts Bible - Matt Lombard [188]
8. Select the Temporary Axes view by choosing View⇒Temporary Axes.
9. Place the cursor near the center of the activated end face; a small, black circle appears, indicating that the end point of the line will pick up a coincident relation to the temporary axis. Draw the line so that it picks up an AlongX sketch relation. The cursor shows the relations about to be applied, just like in a 2D sketch.
10. Draw a second line again from the center, but this time do not pick up any automatic relations. This line should also be on the flat end face.
Note
Although you can set these lines to display as construction lines if you like, this is not required for the feature to work; the lines also work as regular solid lines.
11. Put an angle dimension between the lines and change the angle to 30 degrees. To be thorough (which is always recommended in 3D sketches, which have a tendency to handle underconstrained sketch geometry unpredictably), constrain the ends of the lines to the circular edge of the cylinder. At this point, the part looks like Figure 13.6.
Figure 13.6
The example part at the end of Step 11
12. Create an AlongY sketch relation between the points indicated in Figure 13.7. The hole centerpoint on the cylindrical face is one of the points, as well as the endpoint of the angled line. Change the angle dimension to ensure that it is controlling the sketch point as expected. Click the green check in the upper-right corner of the graphics window to accept the result and exit the command.
Figure 13.7
Control the placement of the 3D sketch point around the cylinder.
On the DVD
You can find the finished part from this example on the DVD with the filename Chapter 13 3D Hole Placement.sldprt.
Cross-Reference
Chapters 6 and 8 contain more information on general 3D sketch tools and techniques.
Making and using favorites
Hole Wizard Favorites store types of holes that you use frequently so that you can simply recall a favorite, rather than manually making all the changes every time you use the same hole. Favorites are saved to a database named Default.mdb as you create them, and are immediately available from all other part documents connected to that database. You can also save favorites to a special file type with the extension *.sldhwfvt. Other users can then load these files and add your favorites to their Default.mdb databases. This is a convenient way to create company standards for hole features.
Shared Toolbox installations share a SWBrowser.mdb between several users, making Hole Wizard Favorites available to everyone. I cover how to set up shared Toolbox installations later in this chapter.
Creating a Hole Wizard Favorite
To create a Hole Wizard Favorite, set up a Hole Wizard hole as you normally would, and then use the Add Favorite button to add it to the Favorites database. The Hole Wizard Favorite panel contains five buttons:
• Apply Defaults/No Favorites. Removes favorite settings from the current interface, setting all values back to their defaults.
• Add or Update Favorites. Either adds a new favorite to the database or changes the name or other settings for an existing favorite.
• Delete Favorite. Removes a favorite from the database.
• Save Favorite. Saves a favorite to an external file with the extension *.sldhwfvt, which can be loaded by other users and added to their databases.
• Load Favorite. Loads a saved favorite file.
Storing custom holes
You can use Hole Wizard Favorites to store custom holes. Create the hole with its custom sizes, and then add the favorite and give it a recognizable name. The custom hole will now be available to anyone who connects to the same database file.
Administering Hole Wizard Favorites
The database file is typically found in the Data subdirectory of the SolidWorks installation directory, but an