5238-E P-176
SECTION 8 LATHE AUTO-PROGRAMMING FUNCTION (LAP)
5.
Bar Turning Cycle (G85)
[Program format]
LE33013R0301000050001
[Function]
With the commands above, the control starts searching for the contour definition program beginning
with the sequence name NAT01. After assigning the parameter data of D, F, U, W and G84 to
NAT01, the control starts the bar turning cycle.
[Supplement]
•
Do not designate an S, T, or M code in the G85 block.
•
The D word is used to specify depth of cut in the rough turning cycle. When a G84 command
indicating change of cutting conditions is designated, the D word is effective up to the point
where the change is made, XA and ZA.
A D word must be always be designated in the G85 block, with a value greater than "0". Illegal
designation will cause an alarm.
•
The F word is used to specify the feedrate in a rough turning cycle. When a G84 command
indicating change of cutting conditions is designated, the F word is effective up to the point
where the change is made, XA and ZA.
•
If no F word is designated in the G85 block, the feedrate which was effective before the
execution of the G85 block is effective.
The F word must be positive. If not, an alarm occurs.
•
When a U and/or W word is not designated, U and/or W is assumed to be "0".
U and W words must be positive or zero. If not, an alarm occurs.
N0103
D
F
U
W
G84
Sequence number
G85
G code calling out bar turning cycle
To be designated right after sequence number (name).
NAT01
Sequence name in the first block of contour defining blocks
Enter either tab or space code.
Depth of cut in rough turning cycle
Feedrate in rough turning cycle
Stock removal in finish turning cycle,
X component
Stock removal in finish turning cycle,
Z component
Change of rough
turning conditions
