Operator`s manual

Advanced Haas Mill Programming Techniques Training Manual Page 70
The G94 command is used with the servo controller to control simultaneous angular motion of the indexer
with axis motion of the mill. G94 in the control program is followed by degrees of rotation and the feed
rate in degrees per second in the next step of the program.
STEP STEP SIZE FEED RATE LOOP COUNT G CODE
01 0 270.000 1 [94]
02 [-787.32] [48.35] 1 1 [91]
03 0 270.000 1 [88]
04 0 270.000 1 [99]
G94 pulses the MFIN relay and allows the CNC to proceed.
The program in the CNC mill:
N1 G54 G90 G00 X-.0937 Y0 (rapid to start position in X and Y)
N2 M03 S9932
N3 G43 H1 Z.100 M08
N4 G01 Z-.06 F22.38 (feed to depth)
N5 G00 G91 (rapid in incremental mode)
N6 G01 F10. Z-.06 (feed down to Z depth)
N7 M21 (to start indexing program above at Step 1)
N8 X2.0935 F22.38 (index head and mill move at same time here)
N9 G00 Z1.0 (rapid back in Z axis)
N10 M21 (return indexer home at Step 3)
N11 G0 G53 Z0
N11 M30
In Full Fourth Integration with the Haas Mill the indexer is hooked into the fourth axis port. In the Haas mill
the feed rate in the program is always in in/min. or mm/min. To obtain an angular feed rate in the 4
th
axis
setting #34 is used. The diameter in setting #34 is used to determine the angular feed rate by the Haas
control to correspond to the feed rate given in inch/min.
The program in Haas mill: (setting #34 = .88 inch)
T1M6
N1 G54 G90 G00 X-.0937 Y0 (rapid to start position in X and Y)
N2 M03 S9932
N3 G43 H1 Z.100 M08
N4 G01 Z-.06 F23.8 (feed to depth)
N5 G01 F23.8 Z-.06 (feed down to Z depth)
N6 X2.0935 F23.8 A-787.32 (index head and mill move at same time here)
N7 G00 Z1.0 (rapid back in Z axis)
N8 G0 G53 Z0
N9 M30
Note the direction of the rotation of the head is in the negative direction.