Strategy tab (Drilling)

You can use the Strategy tab of the Hole Feature Properties dialog to edit the machining strategy of a Hole feature.

Combine with similar holes into canned cycle — By default, a tool retracts to the Z rapid plane between operations. Enable this option and then select whether to Retract to the Z rapid plane or the lower Plunge clearance plane after drilling each hole. This option also creates more efficient NC code by entering the canned cycle mode only once.

Machining Type — Select from:

• Drill only — All Hole features are drilled in the traditional way using a drill that is the same size as the hole diameter.
• Drill/Mill — This option allows Hole features to be drilled or milled, to minimize the number of tools needed.
Note: When using Drill/Mill, FeatureCAM adds a rough operation to the tree view and you can access the Stepovers and Milling tabs.

Spot Drill — Enable this option to add a spot drill operation to the Hole feature.

Attempt chamfer w/ spot — Enable this option to try to cut the chamfer during spot drilling. If no available tool can spot and chamfer without gouging the hole, a separate chamfer operation is created.

Pilot Drill — Enable this option to add a pilot drill operation to the Hole feature.

Drill — Enable this option to add a drilling operation to the manufacture of the hole. This operation is usually undersized in preparation for later reaming or boring.

Drill large counterdrill first — For Counter Drill holes, select this option to do the counterdrill operation before the drill operation.

Ream — Enable this option to add a Ream operation to the Hole feature. This option drills a Hole undersized and then reams it to size. The diameter of the drill is between 93% and 97% of the final Hole diameter.

Ream before chamfer — Enable this option to do the Ream operation before the Chamfer operation. This avoids pushing any kind of burr or edge back up onto the chamfer if the chamfer is a sealing surface.

Tap type — This option is available for Tapped Hole features. Select the type of tap from:

• Cutting — The tool cuts the threads into the material.
• Rolled — The tool presses or forms the threads into the material.
• Helicoil — The size of the Drill and Tap operations are larger to fit the helicoil insert.

Bore — Enable this option to add a Bore operation to the Hole feature. Boring places a hole accurately.

Note: The options on this tab are the same as the options on New Feature - Strategies page for a Hole feature in the New Feature wizard.