Tapping Axial - HEIDENHAIN 548431-05 User Manual

Teach-in | Drilling cycles

Tapping axial

Select Drilling
Select Tapping axial
This cycle is used to tap a thread on the face of a workpiece.
Meaning of Retract length: Use this parameter for floating tap
holders. The cycle calculates a new nominal pitch on the basis
of the thread depth, the programmed pitch, and the retraction
length. The nominal pitch is somewhat smaller than the pitch of the
tap. During tapping, the drill is pulled away from the chuck by the
retraction length. With this method you can achieve higher service
life from the taps.
Cycle parameters:
X, Z: Start point
C: Spindle angle – C-axis position
Z1: Start point drill (default: drilling starts from Z)
Z2: End point drill
F1: Thread pitch (default: feed rate from tool definition)
B: Run-in lgth, to achieve the programmed speed and feed rate
(default: 2 * Thread pitch F1)
SR: Return speed for enabling rapid retraction (default: same
spindle speed as for tapping)
L: Retract length with use of floating tap holders (default: 0)
CB: Brake off (1)
SCK: Safety clearance
Further information:
Page 180
G60: Deactivate Protection zone for the drilling operation
0: Active
1: Inactive
T: Tool number – turret pocket number
G14: Tool change point
Further information:
ID: ID no.
S: Cutting speed or Constant speed
SP: Chip breaking depth
SI: Retraction distance
MT: M after T: M function that is executed after the tool call T
MFS: M at beginning: M function that is executed at the
beginning of the machining step
MFE: M at end: M function that is executed at the end of the
machining step
WP: No. of spindle – Displays which workpiece spindle is used
to execute the cycle (machine-dependent)
Main drive
Opposing spindle for rear-face machining
BW: Angle in the B axis (machine-dependent)
HEIDENHAIN | MANUALplus 620 | User's Manual | 12/2017
"Safety clearances SCI and SCK",
"Tool change point G14", Page 180
5
353