Programming manual
144
CNC 8070
7.
GEOMETRY ASSISTANCE
Tangential entry (G37)
(SOFT V02.0X)
134
7.6 Tangential entry (G37)
Function G37 may be used to begin machining with a tangential entry
of the tool without having to calculate the intersection points.
Programming
Tangential entry must be programmed alone in the block and after the
block whose path is to be modified; this path must be a straight line
(G00 or G01).
The programming format is "G37 I<radius>", where the radius value
is programmed in millimeters or in inches, depending on which are the
active units.
The linear path before the tangential entry must have a length equal
to or greater than twice the entry 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 entry radius remains active until another
value is programmed, therefore, it won't be necessary to program it
in successive tangential entries with the same radius.
The "I" value of the entry radius is also used by functions:
G36 (Corner rounding) as rounding radius.
G38 (Tangential exit) as exit radius.
G39 (corner chamfering) as size of the chamfer.
This means that the entry radius set in G37 will be the new value of
the exit radius, rounding radius or chamfer size when programming
these functions or vice versa.
Properties of the function
Function G37 is not modal, therefore, it must be programmed every
time a tangential entry is to be carried out.
G01 G90 X40 Y50 F800
G02 X70 Y20 I30 J0
G01 G90 X40 Y50 F800
G37 I10
G02 X70 Y20 I30 J0
To Next Page
Loading...
