
4.AUTOMATIC OPERATION OPERATION B-63324EN-1/03
- 132 -
Codes are displayed in the order in which they are specified. All
codes are cleared by a program restart command or cycle start in
the reset state.
2 Turn the program restart switch OFF.
3 Check the screen for M, S, T and B codes to be executed. If they
are found, enter the MDI mode, then execute the M, S, T and B
functions. After execution, restore the previous mode.
These codes are not displayed on the program restart screen.
4 Check that the distance indicated under DISTANCE TO GO is
correct. Also check whether or not there is the possibility that the
tool might hit a workpiece or other objects when it moves to the
machining restart position. If there is this possibility, move the
tool manually to a position from where the tool can move to the
machining restart position without hitting any objects.
5 Press the Cycle Start button. The moves to the machining restart
position at the dry run feedrate sequentially along axes in the
order specified by parameter setting No. 7110. Machining is then
restarted.
Explanation
- Block number
When the CNC is stopped, the number of executed blocks is displayed
on the program screen or program restart screen. The operator can
specify the number of the block from which the program is to be
restarted, by referencing the number displayed on the CRT. The
displayed number indicates the number of the block that was executed
most recently. For example, to restart the program from the block at
which execution stopped, specify the displayed number, plus one.
The number of blocks is counted from the start of machining, assuming
one NC line of a CNC program to be one block.
< Example 1 >
CNC Program Number of blocks
O 0001 ;
G90 G92 X0 Y0 Z0 ;
G01 X100. F100 ;
G03 X01 -50. F50 ;
M30 ;
1
2
3
4
5
< Example 2 >
CNC Program Number of blocks
O 0001 ;
G90 G92 X0 Y0 Z0 ;
G90 G00 Z100. ;
G81 X100. Y0. Z120. R-80. F50. ;
#1=#1+1 ;
#2=#2+1 ;
#3=#3+1 ;
G00 X0 Z0 ;
M30 ;
1
2
3
4
4
4
4
5
6
Macro statements are not counted as blocks.