DIN/ISO programming | Programming in ISO Mode
4
236
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
NC blocks of the DIN/ISO program
An NC block contains NC commands such as positioning, switching
or organizational commands. Traversing and switching commands
begin with G or M followed by a number (G1, G2, G81, M3, M30, ...)
and the address parameters. Organizational commands consist of
key words (WHILE , RETURN, etc.) or of a combination of letters/
numbers.
You can also program NC blocks containing only variable calculations.
You can program several NC commands in one NC block, provided
they have different address letters and do not have opposing
functions.
Examples:
Permissible combination: N10 G1 X100 Z2 M8
Non-permissible combination: N10 G1 X100 Z2 G2 X100 Z2 R30
– same address letters are used more than once or N10 M3 M4 –
opposing functionality
To describe workpiece blanks and auxiliary workpiece blanks, use:
G20 "Blank part macro" for standard parts (cylinder, hollow
cylinder)
G21 "Cast-part macro" for blank-part contours based on finished-
part contours G21 is only used for describing workpiece blanks
Individual contour elements (such as are used for finished-part
contours) where use of G20 or G21 is not possible
NC address parameters – the address parameters consist of 1 or 2
letters followed by:
A value
A mathematical expression
A question mark (VGP simplified geometry programming)
A letter i to designate incremental address parameters (examples:
Xi..., Ci..., XKi..., YKi..., etc.)
A # variable
A constant (_constname)
Examples:
X20 [Absolute dimension]
Zi–35.675 [Incremental dimension]
X? [Simplified geometry programming]
X#l1 [Variable programming]
X(#g12+1) [Variable programming]
X(37+2)*SIN (30) [Mathematical expression]
X(20*_pi) [Expression with constant]
To Next Page
Loading...
