B–63604EN/01
19. AXIS CONTROL FUNCTIONPROGRAMMING
337
Example)
When the first, second, and third programs are started by M40, M41,
and M42, respectively
O1234. ;
:
:
M40 ; M code for starting the first program
M41 ; M code for starting the second program
M42 ; M code for starting the third program
M40 ; M code for starting the first program
M41 ; M code for starting the second program
:
:
M30 ;
As M41 is specified while the program started by M40 is being executed,
the second program is automatically started upon termination of the first
program.
M42, M40, and M41, specified during execution of the first program, are
stored such that the corresponding programs are executed in the same
order as that in which the M codes are specified.
If six or more M codes for starting the programs are specified while a
program is being executed, P/S alarm 5038 is output.
The amount of travel along the B–axis can be specified in either absolute
or incremental mode. In absolute mode, the end point of travel along the
B–axis is programmed. In incremental mode, the amount of travel along
the B–axis is programmed directly.
The ABS bit (bit 6 of parameter 8240) is used to set absolute or
incremental mode. When the ABS bit is set to 1, absolute mode is
selected. When the ABS bit is set to 0, incremental mode is selected. The
mode is specified with this parameter when the program is registered.
The T**; command shifts the end point of the specified B–axis travel, in
either the positive or negative direction, by the amount specified with the
B–axis offset screen. If this function is used to set the difference between
the programmed tool position and actual tool position in machining, the
program need not be modified to correct the tool position.
The value specified with parameter 8257 is assigned to the auxiliary
function to cancel the offset. The subsequent nine numbers are assigned
to the tool offset functions. These auxiliary function numbers are
displayed on the B–axis offset screen. For details, see “OPERATION.”
If a G110 block is specified, a single–motion operation along the B–axis
can be specified and executed. In single–motion operation mode, a single
block results in a single operation. The single–motion operation is
executed immediately provided if it is specified before the B–axis
operation is started. If the operation is specified while a registered
program is being executed, the operation is executed once that program
has terminated.
After the specified single–motion operation has been executed, the next
block is executed.
D Specifying absolute or
incremental mode
D Specifying a tool offset
D Single–motion operation