HEIDENHAIN TNC 320 - ENGRAVING (Cycle 225, DIN;ISO: G225); Cycle Run; Please Note While Programming

Cycles: Special Functions
11.6 ENGRAVING (Cycle 225, DIN/ISO: G225)
11
282
HEIDENHAIN | TNC 320 | User’s manual for cycle programming | 9/2016
11.6 ENGRAVING (Cycle 225,
DIN/ISO: G225)
Cycle run
This cycle is used to engrave texts on a flat surface of the
workpiece. The texts can be arranged in a straight line or along an
arc.
1 The TNC positions the tool in the working plane to the starting
point of the first character.
2 The tool plunges perpendicularly to the engraving floor and mills
the character. The TNC retracts the tool to the set-up clearance
between the characters when required. After machining
the character, the tool is at the set-up clearance above the
workpiece surface.
3 This process is repeated for all characters to be engraved.
4 Finally, the TNC retracts the tool to the 2nd set-up clearance.
Please note while programming:
The algebraic sign for the cycle parameter DEPTH
determines the working direction. If you program
DEPTH=0, the cycle will not be executed.
The text to be engraved can also be transferred with
a string variable (QS).
Parameter Q347 influences the rotational position of
the letters.
If Q374=0° to 180°, the characters are engraved from
left to right.
If Q374 is greater than 180°, the direction of
engraving is reversed.
When engraving on a circular arc, the starting point
is at bottom left, above the first character to be
engraved. (With older software versions there was
sometimes a pre-positioning to the center of the
circle.)