Programming Repeat Rigid Tapping on a CNC Machine Tool

Dear Answer Man,

Is there a special G-code program for doing rigid tapping on my Haas VF-2? If I hold a tap in a regular collet holder, and use rigid tapping, can I tap a deep hole in two steps (i.e., tap 3/8″ deep, clear chips, and then tap 3/4″ deep)? Will the spindle orient and pick up a thread in the same spot? If I’m tapping four deep holes, do I peck tap each hole at two depths before moving on to the next hole? Or do I tap all four holes first at a 3/8″ depth, and then at a 3/4″ depth? Will the machine pick up the thread in both cases?

Steve Hann

Dear Steve:

Yes, you will be able to pick up threads at the same spot in both cases. Rigid tapping is a standard feature on all of our machines, except the Mini Mill and Toolroom Mill. Turn on Setting 133 (REPEAT RIGID TAP). Now you’re able to peck tap a hole by using multiple G84 commands at the same location. The first depth will be at Z-0.375; the next will be at Z-0.75 to the final depth. Then move to the next location and repeat the sequence for each hole.

G00 X0.5 Y-0.5

G43 H04 Z0.1

S650 (G84 Turns on spindle)

G84 G99 Z-0.375 R0.1 F32.5 (Hole 1)

G84 Z-0.75

G84 X1.5 Y-1.5 Z-0.375 (Hole 2)

G84 Z-0.75

etc.

Sincerely, Answer Man

|| More
, , , ,