Instructions

1. Move the z-axis only at the current feed rate downward by delta or to the z-
position, whichever is less deep.
2. Retract at traverse rate to clear z
3. Repeat steps above until the z-position is reached.
4. Retract the z-axis at traverse rate to clear z.
Example using a ¼" drill and putting 3-holes in 1.00" deep:
%
g00 g40 g20 g90 g80 z2
x0 y0
g83 x1 y1 z-1 r0.010 q.25 f2
x2
x3
g00 g80 x0 y0
%
The new command to learn is q.
The g84 command
G84 is intended for right-hand tapping. The Sherline CNC system doesn’t have any
provision to accomplish this.
The g85 command
G85 is intended for boring, which is a motion very similar to G81 except it adds feed
out. Usually you use a feed rate around 0.001" per revolution.
Therefore, 1000 RPM = 1-inch feed rate and so on. The reason you want to feed a boring
tool out is to eliminate a spiral tool mark that would result from a rapid retract; therefore,
the tool will feed out at the same rate as it was fed in. The tool will usually take a second
cut as it is withdrawn because a different cutting edge is cutting on the way out. For an
explanation of why you bore holes rather than drill them see the boring head instructions
at http://www.sherline.com/3054inst.htm.
Example:
%
g90 g40 g80 g00 g20 z2
x0 y0
g85 x2 y1 z-0.50 r0.010 f3
g00 g80 x0 y0
%
The g86, g87 and g88 commands
G86, g87 and g88 are intended for boring with starts or stops of the spindle, so these
are not used for the Sherline CNC system because Sherline machines do not have spindle
motor control.
70