www.kxcad.net Home > CAM Index > EdgeCAM Index >
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.
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. The offset can be positive, but if negative, the offset must be smaller than the tool radius.
Island Offset - Specifies the distance the tool is offset from any specified islands, in addition to the tool radius.
% Stepover - Specifies the exact maximum spacing between each pass as a percentage of the tool diameter. Entering a value of 100 would, for example, represent a distance of 100% of the tool diameter, and so the consecutive passes would be no more than one tool diameter apart. The Areaclear cycle can completely clear pockets at up to 100% stepover, without affecting the outer wall of the pocket. Intelligent pocket clearing routines insert a specially calculated "twizzle" move at the corner of each toolpath. A stepover of 70%-80% tends to be fastest.
Mill Type - Select between 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 will plunge into material unless you pre-drill start holes. 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.
Link Control - If the profiles are complicated and islands are present, the system inserts link moves into Areaclear cycles to take the tool from one area to another. The parameter that controls this is Link Control, and it provides you with these linking strategies:
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).
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.
Lace Cut - (External Boss only) Check to keep the tool at depth, cutting regions in a lacing pattern.