FANUC Series 16/18/160/180-Model C for Lathe Operator Manual

PROGRAMMING
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
B–62754EN/01
172
1. In the blocks where the multiple repetitive cycle are commanded, the
addresses P, Q, X, Z, U, W, and R should be specified correctly for each
block.
2. In the block which is specified by address P of G71, G72 or G73, G00
or G01 group should be commanded. If it is not commanded, P/S
alarm No.65 is generated.
3. In MDI mode, G70, G71, G72, or G73 cannot be commanded. If it is
commanded, P/S alarm No. 67 is generated. G74, G75, and G76 can
be commanded in MDI mode.
4. In the blocks in which G70, G71, G72, or G73 are commanded and
between the sequence number specified by P and Q, M98 (subprogram
call) and M99 (subprogram end) cannot be commanded.
5. In the blocks between the sequence number specified by P and Q, the
following commands cannot be specified.
One shot G code except for G04 (dwell)
01 group G code except for G00, G01, G02, and G03
06 group G code
M98 / M99
6. While a multiple repetitive cycle (G70AG76) is being executed, it is
possible to stop the cycle and to perform manual operation. But, when
the cycle operation is restarted, the tool should be returned to the
position where the cycle operation is stopped.
If the cycle operation is restarted without returning to the stop position,
the movement in manual operation is added to the absolute value, and
the tool path is shifted by the movement amount in manual operation.
7. When G70, G71, G72, or G73 is executed, the sequence number
specified by address P and Q should not be specified twice or more in
the same program.
8. Do not program so that the final movement command of the finishing
shape block group designated with P and Q for G70, G71, G72, and
G73 finishes with chamfering or corner rounding. If it is specified,P/S
alarm No. 69 is generated.
14.2.8
Notes on Multiple
Repetitive Cycle
(G70–G76)

Leave a Reply

Your email address will not be published. Required fields are marked *