Fagor 8055 EN, Programming Manual

Page: 256 / 482

·256·
Programming manual
CNC 8055
CNC 8055i
11.
IRREGULAR POC
K
ET CANNED CYCLE
·M· & ·EN· M
ODELS
S
OFT
: V02.2
X
3D pockets
[ J5.5 ] Tool tip radius
Indicates the tool tip radius and, therefore, the type of finishing tool being used.
Depending on the radius assigned to the tool in the tool offset table (of the CNC variables: "TOR"
+ "TOI") and the value of assigned to this parameter, three tool types may be defined.
FLAT If J is not programmed or J = 0.
SPHERICAL If J = R.
TORIC If J other than 0 and J smaller than R.
[ I±5.5 ] Pocket depth
Defines the total depth of the pocket and is programmed in absolute coordinates.
• If defined, the cycle will take it into account during the finishing operation.
• If not defined and the pocket has a roughing operation, the cycle will assume the value defined
for the roughing operation.
• If not defined and the pocket has no roughing operation, but it has a semi-finishing operation,
the cycle will assume the one define in the semi-finishing operation.
• If the pocket has neither roughing nor semi-finishing operation, this parameter must be defined.
[ R±5.5 ] Reference plane
Defines the reference plane coordinate and is programmed in absolute coordinates.
• If defined, the cycle will take it into account during the finishing operation.
• If not defined and the pocket has a roughing operation, the cycle will assume the value defined
for the roughing operation.
• If not defined and the pocket has no roughing operation, but it has a semi-finishing operation,
the cycle will assume the one define in the semi-finishing operation.
• If the pocket has neither roughing nor semi-finishing operation, this parameter must be defined.
[ 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 finishing 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.