Shaped Cutters in Milling Operations

(ball-nosed, bull-nosed, chamfer cutters, corner-rounders, Dovetail, etc)

This short article is intended to clarify how toolpath is calculated for tools with a shape. Additional information can be found in the Mill Module manual by looking up Tapered Tools in the index.

Before any toolpath is generated the depth of cut is calculated. This is figured by comparing the Start Z position in the machining process to the End Z. The distance between these values is the depth of cut for this process. A measurement is then taken from the bottom of the tool the distance of the depth of cut. The diameter of the tool at this position is the diameter used to offset the tool in the machining being performed. When the depth of cut places the tangency somewhere on the shaped portion of the cutter the offset amount will be different from the full diameter of the cut.


Ball- and bull-nosed end mills - The most common problem with this type of cutter is when a fillet is being applied to the bottom of a pocket where it has already been roughed out using a flat end mill. Your best option is to increase your Start Z in the contour process so that the depth of cut equals or exceeds the corner radius of the tool.

Corner-rounders - These can be tricky. The first step is to carefully define your tool. The value needed to correctly calculate toolpath is the distance from the bottom of the tool to the top of the fillet radius in the tool definition. When defining your contour it is important that the depth of cut equal this number. The last step is to enter a negative stock value in the Stock field. This will be a negative value equal to the radius created by your corner-rounder.

Chamfers - The starting depth is important for this type of cut. Be sure it is set to the Z-value of the top of your chamfer. Your finish depth can be deeper than the bottom of the chamfer in order to avoid cutting right on the top of the cutter. If the geometry being selecting is the line representing where the sharp corner would be if not for the chamfer you will need to enter a negative stock value equal to the size of your chamfer. If the line or shape selected represents the top edge of your chamfer your stock field would be set to 0.