List Of Instructions; A.18 List Of Instructions - Siemens SINUMERIK 808D ADVANCED Programming And Operating Manual

Word order
If there are several instructions in a block, the following order is recommended:
N... G... X... Z... F... S... T... D... M... H...
Note regarding block numbers
First select the block numbers in steps of 5 or 10. Thus, you can later insert blocks and nevertheless observe the ascending
order of block numbers.
Block skip
Blocks of a program, which are to be executed not with each program run, can be marked by a slash / in front of the block
number.
The block skip itself is activated via Operation (program control: "SKP") or by the programmable controller (signal). A section
can be skipped by several blocks in succession using " / ".
If a block must be skipped during program execution, all program blocks marked with " / " are not executed. All instructions
contained in the blocks concerned will not be considered. The program is continued with the next block without marking.
Comment, remark
The instructions in the blocks of a program can be explained using comments (remarks). A comment always starts with a
semicolon " ; " and ends with end-of-block.
Comments are displayed together with the contents of the remaining block in the current block display.
Messages
Messages are programmed in a separate block. A message is displayed in a special field and remains active until a block
with a new message is executed or until the end of the program is reached. Up to 65 characters can be displayed in
message texts.
A message without message text cancels a previous message.
MSG ("THIS IS THE MESSAGE TEXT")
Programming example
N10
N20
N30
N40 MSG("DRAWING NO.: 123677")
:50 G54 F4.7 S220 D2 M3
N60 G0 G90 X100 Z200
N70 G1 Z185.6
N80 X112
/N90 X118 Z180
N100 X118 Z120
N110 G0 G90 X200
N120 M2
A.18

List of instructions

The functions marked with an asterisk (*) are active at the start of the program in the CNC milling variant, unless otherwise
they are programmed or the machine manufacturer has preserved the default settings for the "milling" technology.
Address Significance
D Tool offset number
F Feedrate
258
Value assignments Information
0 ... 9, only integer, Contains compensation data
no sign for a particular tool T... ; D0-
>compensation values= 0,
max. 9 D numbers for one tool
0.001 ... 99 999.999 Path velocity of a
tool/workpiece;
unit: mm/min or mm/revolution
depending on G94 or G95
; G&S company, order no. 12A71
; Pump part 17, drawing no.: 123 677
; Program created by H. Adam, Dept. TV 4
;Main block
; Block can be suppressed
; End of program
Programming and Operating Manual (Milling)
Programming
D...
F...
6FC5398-4DP10-0BA1, 01/2014