CNC Drilling Programming Hints

Milling and Drilling Programming
Program Notes: (Fig. 26)
• Program in the absolute mode starting at the tool change
position at the top left corner of the print.
• The material is aluminum (300 CS), feedrate 10 in/min.
• The cutting tool is a .250 in. diameter high speed steel 2-flute
end mill.
• Mill the 1 in. square slot.
• Drill the two .250 in. diameter holes, .250 in. deep.
• Mill the .250 in. wide angular slot, .125 in. deep.
• Mill the .250 in. wide circular groove, .125 in. deep.
• After the job is completed, return to the tool change position.
Programming:
% (rewind stop code / parity check)
2000 (program number)
N5 G92 X-1.000 Y1.000 Z1.000
G92 programmed offset of reference point (tool change
position)
X-1.000 tool set at 1.000 to the left of the part.
Y1.000 tool set at 1.000 above the top edge of the part.
Z1.000 the end of the cutter is 1.000 above the top surface
of the part.
N10 G20 G90
G20 inch data input.
G90 absolute programming mode.
N15 M06 T01
M06 tool change command.
T01 tool no. 1 (.250 diameter, 2-flute end mill).
N20 S2000 M03
S2000 spindle speed set at 2000 r/min.
M03 spindle on clockwise.

N25 G00 X0 Y0 Z.100
G00 rapid traverse rate to X0 Y0 at the top left corner of
the part.
Z.100 tool rapids down to within .100 of the work surface.
Machining the square groove
N30 X.375 Y-.375
tool rapids to position A.
N35 G01 Z-.125 F10
G01 linear interpolation.
Z-.125 tool feeds .125 below the work surface.
F10 feed rate set at 10 in./min.
N40 X1.625 Y-.375
X1.625 top groove cut to the right hand end.
Y-.375 measurement did not change because it was set in
block N30.
N45 Y-1.625
Y-1.625 right hand side of the groove cut.
N50 X.375
X.375 bottom groove cut to the left side.
N55 Y-.375
Y-.375 left-hand side of groove cut; this completes the
groove.
N60 G00 Z.100
G00 rapid traverse mode.
Z.100 tool rapids to .100 above work surface.
Hole Drilling
N65 G00 X.875 Y-.750
tool rapids to the top left hole location.

36
N70 G01 Z-.250 F10
tool feeds .250 into work at 10 in./min. to drill the
first hole.
N75 G00 Z.100
tool rapids out of hole to .100 above work surface.
N80 X1.250 Y-1.125
tool rapids to second hole location.
N85 G01 Z-.250 F10
tool feeds .250 into work at 10 in./min. to drill the
second hole.
N90 G00 Z.100
tool rapids out of hole to .100 above work surface.
Machining the Angular Slot
N95 X1.125 Y-.875 (location B)
tool rapids to the start of the angular slot.
N100 G01 Z-.125 F10
G01 linear interpolation.
Z-.125 tool feeds to .125 below the work surface.
F10 feed rate set at 10 in./min.
N105 X1.250 Y-.750
angular slot cut to top right corner.
N110 G00 Z.100
tool rapids to .100 above work surface.
Machining the Circular Groove
N115 X.750 Y-1.000 (location C)
tool rapids to start of circular groove.
N120 G01 Z-.125 F10
tool feeds to .125 below the work surface.
N125 G03 X1.000 Y-1.250 R.250
G03 circular interpolation counterclockwise
X & Y location of end of circular groove.
R.250 radius of arc is .250.
N130 G00 Z.100
tool rapids to .100 above work surface.
N135 X-1.000 Y1.000
tool rapids back to tool change position.
N140 M05
M05 spindle turned off.
N145 M30
M30 end of program

Post a Comment

Previous Post Next Post