Programming manual
CNC 8055
CNC 8055i
IRREGULAR POCKET CANNED CYCLE
11.
·M· & ·EN· MODELS
SOFT: V02.2X
·233·
2D pockets
[ I±5.5 ] Pocket depth
Defines the total depth of the pocket and is programmed in absolute coordinates.
• If the island has a roughing operation, it is not necessary to define this parameter since it has
been programmed in that operation. However, if programmed in both operations, the canned
cycle will assume the particular depth indicated for each operation.
• If the island has no roughing operation, it is necessary to define this parameter.
[ R±5.5 ] Reference plane
Defines the reference plane coordinate and is programmed in absolute coordinates.
• If the island has a roughing operation, it is not necessary to define this parameter since it has
been programmed in that operation. However, if programmed in both operations, the canned
cycle will assume the particular depth indicated for each operation.
• If the island has no roughing operation, it is necessary to define this parameter.
[ K1 ] Type of profile intersection
Defines the type of profile intersection to be used.
K=0 Basic profile intersection.
K=1 Advanced profile intersection.
If the island has a roughing operation, it is not necessary to define this parameter since it has been
programmed in that operation. However, if programmed in both operations, the canned cycle will
assume the one defined for the roughing operation.
If no roughing operation has been defined and this parameter is not programmed, the canned cycle
will assume a K0 value. Both types of intersection are described later on.
[ V5.5 ] Penetration feedrate
Defines the tool penetrating feedrate.
If not programmed or programmed with a 0 value, it assumes 50% of the feedrate in the plane (F).
[ F5.5 ] Machining feedrate
Optional. It sets the machining feedrate in the plane.
[ S5.5 ] Spindle speed
Optional. It sets the spindle speed.
[ T4 ] Tool number
Defines the tool used for the roughing operation. It must be programmed.
[ D4 ] Tool offset
Optional. Defines the tool offset number.
[ M ] Auxiliary (miscellaneous) functions
Optional. Up to 7 miscellaneous M functions can be programmed.
This operation allows M06 with an associated subroutine to be defined, and the tool change is
performed before beginning the roughing operation.
To Next Page
Loading...
