Mitsubishi Electric M700V Series Programming Manual page 249

12. Tool Compensation Functions
Detailed description
(1) Program error (P171) will occur if this command is input when the specifications are not
available.
(2) G10 is an unmodal command and is valid only in the commanded block.
(3) The G10 command does not contain movement, but must not be used with G commands other
than G54 to G59, G90 or G91.
(4) Do not command G10 in the same block as the fixed cycle and sub-program call command.
This will cause malfunctioning and program errors.
(5) The workpiece offset input command (L2 or L20) should not issued in the same block as the
tool compensation input command (L10).
(6) If an illegal L No. or compensation No. is commanded, the program errors (P172 and P170)
will occur respectively.
If the offset amount exceeds the maximum command value, the program error (P35) will occur.
(7) Decimal point inputs can be used for the offset amount.
(8) The offset amounts for the external workpiece coordinate system and the workpiece
coordinate system are commanded as distances from the basic machine coordinate system
zero point.
(9) The workpiece coordinate system updated by inputting the workpiece coordinate system will
follow the previous modal (G54 to G59) or the modal (G54 to G59) in the same block.
(10) L2 (or L20) can be omitted when the workpiece offset is input.
(11) If the P command is omitted at the workpiece offset input, the currently selected workpiece
offset will be handled as the input.
(12) When the "P" to designate the compensation No. is commanded in the same block as G22.1
or G23.1, the tool compensation data will not be input. "P" will be regarded as the number of
repetition of subprogram call, that will cause an illegal operation.
Example of program
(1) Input the compensation amount
•••••• ; G10L10P10R–12345
H10=-12345 H05=98765 H30=2468
(2) Updating of compensation amount
(Example 1) Assume that H10 = -1000 is already set.
12.7 Programmed Compensation Input; G10, G11.1
; G10L10P05R98765
N1 G01 G90 G43 Z - 100000 H10;
N2 G28 Z0;
N3 G91 G10 L10 P10R - 500 ;
N4 G01 G90 G43 Z - 100000 H10 ;
237
; G10L10P30R2468 ; •••
(Z = -101000)
(The mode is the G91 mode, so -500
is added.)
(Z = -101500)