·132·
Programming manual
CNC 8055
CNC 8055i
8.
TOOL COMPENSATION
·M· & ·EN· MODELS
SOFT: V02.2X
Tool radius compensation (G40, G41, G42)
8.1 Tool radius compensation (G40, G41, G42)
In normal milling operations, it is necessary to calculate and define the path of the tool taking its
radius into account so that the required dimensions of the part are achieved.
Tool radius compensation allows the direct programming of part contouring and of the tool radius
without taking the dimensions of the tool into account.
The CNC automatically calculates the path the tool should follow based on the contour of the part
and the tool radius value stored in the tool offset table.
There are three preparatory functions for tool radius compensation:
G40: Cancellation of tool radius compensation
G41: Left-hand tool radius compensation.
G42: Tool radius compensation to the right of the part.
G41 The tool is to the left of the part, depending on the machining direction.
G42 The tool is to the right of the part, depending on the machining direction.
Tool values R, L, I, K should be stored in the tool offset table before starting machining, or should
be loaded at the beginning of the program via assignments to variables TOR, TOL, TOI, TOK.
Once the plane in which compensation will be applied has been chosen via codes G16, G17, G18,
or G19, this is put into effect by G41 or G42, assuming the value of the tool offset selected via code
D, or (in its absence) by the tool offset shown in the tool table for the selected tool (T).
Functions G41 and G42 are modal and incompatible to each other. They are cancelled by G40, G04
(interruption of block preparation), G53 (programming with reference to machine zero), G74 (home
search), machining canned cycles (G81, G82, G83, G84, G85, G86, G87, G88, G89) and also on
power-up, after executing M02, M30 or after EMERGENCY or RESET.
To Next Page
Loading...
