PROGRAMMING
13. FUNCTIONS TO SIMPLIFY
PROGRAMMING
B–63604EN/01
158
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. The blocks between the sequence number specified by P and Q on the
multiple repetitive cycle must not be programmed by using “Direct
Drawing Dimensions Programming” or “Chamfering and Corner R”.
9 G74, G75, and G76 also do not support the input of a decimal point
for P or Q. The least input increments are used as the units in which
the amount of travel and depth of cut are specified.
10 When #1 = 2500 is executed using a custom macro, 2500.000 is
assigned to #1. In such a case, P#1 is equivalent to P2500.
11 Tool nose radius compensation cannot be applied to G71, G72, G73,
G74, G75, G76, or G78.
12.The multiple repetitive cycle cannot be executing during DNC
operation.
13.Interruption type custom macro cannot be executed during executing
the multiple repetitive cycle.
14.The multiple repetitive cycle cannot be executing during Advanced
Preview Control mode.
13.2.8
Notes on Multiple
Repetitive Cycle
(G70 – G76)