Programming manual
CNC 8055
CNC 8055i
CANNED CYCLES
9.
·M· & ·EN· MODELS
SOFT: V02.2X
·199·
G211. Inside thread milling cycle
9.17 G211. Inside thread milling cycle
This cycle may be used to make an inside thread through a helical movement of the tool.
Working in Cartesian coordinates, the basic structure of the block is as follows:
G211 G98/G99 X Y Z D I J K B C L A E Q
[ G98/G99 ] Withdrawal plane
G98 The tool withdraws to the Initial Plane, once the hole has been milled.
G99 The tool withdraws to the Reference Plane, once the hole has been milled.
[X±5.5] Hole center coordinate along the abscissa axis.
It defines the hole center coordinate along the X axis. If not programmed, it will assume the current
tool position on that axis.
[ Y±5.5 ] Hole center coordinate along the ordinate axis
It defines the hole center coordinate along the Y axis. If not programmed, it will assume the current
tool position on that axis.
[ Z±5.5 ] Reference plane
Defines the reference plane coordinate. It may be programmed either in absolute or incremental
coordinates, in which case it will be referred to the starting plane.
If not programmed, it assumes as reference plane the current position of the tool.
[D5] Safety distance
Defines the distance between the reference plane and the surface of the part where the milling is
to be done. If not programmed, it assumes 0.
[ I±5.5 ] Machining depth
Defines the threading depth. It may be programmed either in absolute or incremental coordinates,
in which case it will be referred to the reference plane.
If not programmed, the CNC issues the corresponding error.
[ J±5.5 ] Thread diameter
Defines the nominal diameter of the thread The sign indicates the machining direction of the thread
(positive if clockwise and negative if counterclockwise).
If not programmed, the CNC issues the corresponding error.
J
Z
D
I
B
K
L
A
G00
G01
M03
M04
G98
G99
To Next Page
Loading...
