4200T CNC Programming and Operations Manual
P/N 70000412F - Canned Cycles
All rights reserved. Subject to change without notice. 5-3
31-July-05
Table 5-2, G73 Part Program
Program Block Description
N1 G70 G90 G0 X0 Z0 T0 Sets Inch/MM Mode and
Absolute Mode. Places
machine at X0,Z0 with no tool
offsets active.
N2 X3.7 (93.9) Z0 T1 Activates T1, rapids to X start
position (.2” standoff).
N3 G1 X-.03 (-1) G95 F.008
(0.2)
Faces to X-0.03" (X-1mm) past
centerline at 0.008" (.2mm) per
revolution.
N4 G0 X3.7 (93.9) Z.1 (2.0) Rapids to start position of Area
Clearance Cycle.
N5 G73 W9 A.2 (5) R.02 (.5)
S.005 (.1) C1 B1 J.02 (.5)
K.01 (.25)
Sets parameters for G73 and
activates cycle.
N6 T0 X0 Z0 Cancels T1 offsets, rapids to
home position.
N7 M2 Ends Program, returns to block
N1.
N8 Blank for easy distinction
between Main and Sub-
programs.
The following subprogram describes the part profile called into the
main program above. The CNC calculates actual moves based
on the profile described in the subroutine.
N10 O9 (Subprogram) Establishes name of
Subprogram (O9).
N11 G0 X1 (X25.4) Z.1 (2) Rapids to start point of profile.
N12 Z-1 (-25.4) Feeds to Z-1" (Z-25.4mm).
N13 X2 (50.8) Z-1.5 (-38.1) Feeds up angle to X2 Z-1.5
(X50.8 Z-38.1).
N14 Z-2.25 (-57.15) Feeds to start of radius.
N15 G3 X3.5 (88.9) Z-3 (-
76.2) R.75 (19.05)
Feeds around radius CCW.
N16 G1 X3.7 (93.9) Feeds away from part
diameter to clear the part.
N17 M99 Ends Subprogram.
NOTE: All variables are sign (+/-) dependent. Moves can be defined as
Outer Diameter/Inner Diameter, and toward or away from the
chuck or part centerline. The positive/negative direction (sign of
the variable) determines what kind of move is made by the CNC.
Ensure that the appropriate sign (+/-) is programmed.
To Next Page
Loading...
