Hole: Tool Selection

The first step of drilling a Hole is to determine what kind of hole it is. Then collect a list of operations to produce that hole. After the analysis, FeatureCAM picks tools. The table below shows the tooling types that can be used for each operation type.

Operation type	Automatically selected tool	Possible user overrides	Notes
spotdrill	Spot or Center Drill	spotdrill, centerdrill, countersink	Automatic behavior is dependent on the prefer spotdrill or prefer centerdrill attributes.
chamfer	Countersink	spotdrill, centerdrill, countersink, chamfer	If the tool diameter is smaller than the hole diameter, circular interpolation is performed. You can override the automatically selected tool with a tool that does not have a 90 degree included angle, but the chamfer is not a 90 degree chamfer. The tool diameter is found by multiplying the chamfer's outer diameter by 1.1 to ensure the end of the chamfer tool is not used for cutting.
twistdrill	Twist drill	twistdrills, endmills	No circular interpolation is performed with endmills, even if the diameter is smaller than the hole's. See Step Bore feature if you want to mill a circular pocket.
bore	Boring bar	boringbar
counterbore	Counter bore	counterbore, endmill	Circular interpolation is performed if the tool's diameter is smaller than the counterbore's.
ream	Ream	ream
tap	Tap	tap	For blind holes a fast spiral, plug tap is preferred. Through holes require a gun style plug tap.

For drilling, the most important criteria are diameter and length. If a tool can't be found that satisfies the criteria, then you receive a tool selection error.

The size of the tool selected may be affected by the Tool diameter tolerance attribute on the Tool Selection page of the Machining Attributes dialog.

See also:

Tool Groups for details on the different tooling types