CNC 8035 - Programming manual - Fagor Automation

9.6 G83. Axial drilling and tapping canned cycle
This cycle may be used to carry out axial drilling or axial tapping. Whether one operation or the other
will be performed depends on the format being used. For tapping, set parameter "B=0", and for axial
drilling, set "B>0".
The basic block structure for each operation is:
X±5.5
Defines the X coordinate where the cycle is to be run. It must be programmed in absolute coordinates
and in the active units, radius or diameter.
Z±5.5
Defines the Z coordinate where the cycle will be run. It must be programmed in absolute coordinates.
I±5.5
Defines the total depth. It is referred to the drilling point (X, Z); thus, it will have a positive value when
drilling in the negative Z direction and vice versa.
If programmed with a 0 value, the CNC will display the corresponding error message.
B5.5
Defines the type of operation to be run.
D5.5
If B=0, the CNC will carry out an axial tapping.
If B>0 it will carry out an axial drilling where B indicates the drilling step.
Defines the safety distance and it indicates at what distance the tool is positioned in the approach
move. If not programmed, a value of 0 is assumed.
K5
Defines the dwell, in hundredths of a second, at the bottom of the hole before starting the withdrawal.
If not programmed, a value of 0 is assumed.
H5.5
Defines the withdrawal distance after each drilling step (in G00). If not programmed or programmed
a value of 0, it will withdraw to the approach point.
C5.5
Axial drilling G83 X Z I B D K H C L R
Axial tapping G83 X Z I B0 D K R
Defines the approach distance along Z from the previous drilling step to start the next drilling step
(in G00). If not programmed, a value of 1 millimeter.
Programming manual
CANNED CYCLES
G83. Axial drilling and tapping canned cycle 9.
CNC 8035
·T· MODEL
(SOFT V16.3X)
·183·