Tapping (G63)
Syntax example of tapping in Z direction: | |
G63 Z.. F.. <spindle_name>.. | modal |
G63 | Thread tapping |
Z.. | Thread depth (target point) in the tapping axis in [mm, inch] |
F.. | Feed rate in [mm/min, m/min, inch/min] |
<spindle_name>.. | Spindle speed consisting of spindle name according to P-CHAN-00053 and speed value in [rpm] |
With this kind of tapping (G63) the position-controlled spindle is tracked by the CNC synchronously to the path motion. In this case the spindle and the feed motion of the participating axes are matched precisely and dynamically. A compensatory chuck is not required. The programmed feed rate must match the programmed spindle speed and the thread pitch and is calculated as follows:
Feed rate F [mm/min] = speed S [rpm] * pitch [mm/rev]
G63 is deselected by the selecting a different modal block type (e.g. linear motion G01). A non-modal block type (e.g. dwell time with G04) does not deactivate G63.
The path feed rate (F word) and spindle speed (S word) do not necessarily need to be specified in the same NC block as G63. The feed rate calculation must always be based on the last values programmed.
An error message is output if the path feed rate or spindle speed are equal to zero with G63 is selected.
M03, M04, M05, M19 cannot be programmed in combination with G331/G332.
Notice | |
The spindle (or the thread tapping drill) must be at standstill when G63 is selected. This can be achieved by previously programming M05 (Stop spindle) or M19 with S.POS (Position spindle). |
Cutting a left-hand thread or movement out of a thread hole is programmed with a negative S value.
In C axis mode, the gear stage can be defined using the parameter P-AXIS-00052.
Programming Example
Tapping (G63)
Tap a right-hand thread with pitch 1.25 mm, thread depth 50 mm. At a programmed spindle speed S of 200 rpm the calculated feedrate is:
F = 200*1.25 = 250 mm/min
Programming Example
Tapping (G63)