Programming manual
CNC 8070
GEOMETRY ASSISTANCE
Tangential exit (G38)
7.
(SOFT V02.0X)
135
7.7 Tangential exit (G38)
Function G38 may be used to end machining with a tangential exit of
the tool without having to calculate the intersection points.
Programming
Tangential exit must be programmed alone in the block and before the
block whose path is to be modified; this path must be a straight line
(G00 or G01).
The programming format is "G38 I<radius>", where the radius value
is programmed in millimeters or in inches, depending on which are the
active units.
The linear path after the tangential exit must have a length equal to
or greater than twice the exit radius. Likewise, the radius must be
positive and when working with tool radius compensation, it must be
greater than the tool radius.
Considerations
The "I" value of the tangential exit radius remains active until another
value is programmed, therefore, it won't be necessary to program it
in successive tangential exits with the same radius.
The "I" value of the exit radius is also used by functions:
G36 (Corner rounding) as rounding radius.
G37 (Tangential entry) as entry radius.
G39 (corner chamfering) as size of the chamfer.
This means that the exit radius set in G38 will be the new value of the
entry radius, rounding radius or chamfer size when programming
these functions or vice versa.
Properties of the function
Function G38 is not modal, therefore, it must be programmed every
time a tangential exit is to be carried out.
G02 X60 Y40 I20 J0 F800
G01 X100
G02 X60 Y40 I20 J0 F800
G38 I10
G01 X100
To Next Page
Loading...
