Numeryx Home > User/Programmer

Pocket Milling

An-104, Copyright © by Gil Hagiz
Last updated Jan-23-2006
For version 5.11 and higher


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.

Pocket G-codes

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.

Circular pocket, G212/213

G213 r_ n_ k_ f_
r is the desired radius.

g x y z5
g1 z-11 f200
g213 r120 n50 k2 f1000

Rectangular pocket, G214/215

G215 i_ j_ r_ n_ k_ f_
ij are half the width and the height.
r is a fillet, may be zero.

g x y z5
g1 z-11 f200
g215 i100 j120 r25 n50 k2 f1000

Hole milling

These cycles cut a circular path. The path is entered and left by tangent arcs.

Circular hole, G202/203

G203 r_ f_
r is the radius.

g x y z5
g1 z-10 f200
g203 r100 f1000

Deep hole, G202.1/203.1, G202.2/203.2

These codes spiral down at a programmed step.
G203.1 r_ z_ k_ f_
r is the radius.
z is the bottom of the hole (absolute).
k is the spiraling down step per turn.

For g20x.2 there is additional turn without spiraling Z at the bottom (for blind holes).

g x y z22
g1 z20 f200
g202.1 r100 z-20 k4 f1000