Strategy - Specifies a roughing strategy:
Pocket - Generates a roughing areaclear cycle using a concentric toolpath strategy, starting from the inside and working towards the outer edges of the profile.
External Boss - Generates a series of offset toolpaths from the inner shape clipped to the outer shape. The toolpaths always start from the outside.
Mill Type - Select from a list containing None, Climb and Conventional. If Constant Cut has NOT been checked, the None option is assumed (lacing).
Link Control - Specifies a link move strategy between islands:
Retract - The tool rapids to the clearance plane, rapids in the workplane to the start of the next toolpath element and then feeds down to depth.
Shortest - The tool feeds directly (using the shortest route, avoiding islands) to the next toolpath element, remaining at depth the whole time.
Mill Type - Similar to the Shortest link strategy, but the link is controlled by the Mill Type for the cycle (Climb or Conventional).
Direction - There are two possible ways for a series of concentric toolpaths to be cut:
Inside Out - Start the cycle with the innermost toolpath first. The tool plunges into material unless start holes are pre-drilled. This is the most commonly used method, and should be used if any parameters are set on the Approach tab.
Outside In - Start the cycle with the outermost path first. This should only be used when the Approach Strategy is set to Plunge, as the tool cannot perform a helical or zigzag approach starting from the boundary.
Feedrate - Specifies the rate of movement in the workplane.
Plunge Feed - Specifies the rate of movement in the direction of the tool axis.
Speed - Specifies the tool spindle speed.
Offset - Specifies the toolpath offset from the surface. Note that this is a three dimensional offset from the surface. The offset can be positive, but if negative, the offset must be smaller than the tool radius.
Tolerance - Controls the accuracy to which the surface is machined. A small value results in a more accurate surface finish but takes longer to generate the toolpath.
Cut Increment - Specifies the depth of each successive cut. This must be a positive value. The cut increment value sets the vertical distance between successive waterline planes.
% Stepover - Specifies the tool stepover distance between each pass as a percentage of the tool diameter.
Feature Name - Enter a name here to allow labelling of digitised information for this cycle to enable "pickup" of this information in another (similar) cycle.