Here is a collection of canned cycles for common pocket and hole milling.
Except for the deep hole milling, these cycles are 2-D. The tool must be located at the center and at the desired Z before starting.
Tool radius is included in the cycles and therefore tool radius comp should not be activated. The tool radius is taken from the tool table.
Usually current tool is always known to the program but if not then g40 t_ should be programmed somewhere before the pocket is called.
Note: For the examples below, tool radius is 10 mm.
For all pockets:
A pocket is generated by successive cuts, based on a percentage of the tool diameter.
Tool radius cannot be zero.
n – percentage of tool diameter per cut, cannot be zero.
k – finish cut, may be zero.
The finish cut is entered by a tangent arc from the previous cut and left by a tangent arc to the center. The last move also raises the tool 1 mm (0.04").
If the finish cut is zero the last cut repeats twice.
Rotation can be used. Scale shouldn't be used.
Note: Even numbers cut CW, odd numbers cut CCW.
g x y z5 g1 z-11 f200 g213 r120 n50 k2 f1000
g x y z5 g1 z-11 f200 g215 i100 j120 r25 n50 k2 f1000
g x y z5 g1 z-10 f200 g203 r100 f1000
g x y z22 g1 z20 f200 g202.1 r100 z-20 k4 f1000