Programming manual
CNC 8070
CANNED CYCLES
G85. Reaming canned cycle
10.
(SOFT V02.0X)
195
10.6 G85. Reaming canned cycle
Programming format in Cartesian coordinates:
G85 Z I K
Parameter definition:
Basic operation:
1. If the spindle was previously running, it maintains the turning
direction. If it is stopped, it starts clockwise (M03).
2. Rapid movement (G0) of the longitudinal axis from the starting
plane (Zi) to the reference plane (Z).
3. Reaming the hole. Movement of the longitudinal axis at work
feedrate, to the bottom of the hole programmed in "I".
4. Dwell, in seconds, if it has been programmed.
5. Withdrawal, at work feedrate (G01) up to the reference plane (Z).
6. If function G98 is active, rapid withdraw to the starting plane (Zi).
Z Reference plane.
In G90, coordinate referred to part zero.
In G91, coordinate referred to starting plane (Zi).
If not programmed, it assumes as reference plane the current
position of the tool (Z=Zi).
I Reaming depth.
In G90, coordinate referred to part zero.
In G91, coordinate referred to reference plane (Z).
K Delay, in seconds, between the reaming and the withdrawal
movement.
If not programmed, it assumes K0.
To Next Page
Loading...
