Haas VF Series, Operator'S Manual

Page: 400 / 564

400
OPTIONS
96-8000
June 1999
11.8 T
APPING
W
ITH
T
HE
VF-S
ERIES
CNC M
ILL
Making tapped holes with the VF Series CNC Mill can be made with several devices. Threads may be gener-
ated with a tap held in a rigid tool holder (called rigid tapping), a floating tap holder, a reversing tapping head, or
helical thread milling. Each method has distinct advantages.
Tapping is done using canned cycles. You must select the tapping RPM and, using the pitch (threads per
inch), calculate the feed rate that is entered in the F command. The HELP/CALC page will compute these
numbers for you.
R
IGID
T
APPING
Rigid Tapping eliminates the cost of special tap holders since taps can be held in drill collet holders. The
spindle is accurately synchronized with the Z-axis feed, thereby producing threads as accurately as a lead
screw tapper. No side forces are generated on the flanks of the threads and tighter thread tolerances are
produced. Rigid tapping also eliminates the pullout and distortion of the first thread that occurs on all spring
compression/tension devices and tapping heads. While this is not usually a problem on medium to coarse
threads, small diameter, fine pitch or soft material tapped holes can have their last thread damaged when the
tap pops out of the hole. You can also re-tap a hole without cross-threading provided the tap and Z depths have
not been changed. Rigid tapping is used with canned cycles G74 and G84 and is an extra cost factory in-
stalled option. Example:
N100 G84 Z-1. R.3 F37.5 (for a 20 pitch thread at 750 RPM)
A word of caution on Rigid Tapping: As the term implies, the tap is rigidly held in place. This requires that
runout be less than .001 TIR or the tap will generate an oversized thread. This problem can be minimized by
using a small diameter drill extension to provide flex, a radial floating tool holder, or specially-designed chucks
for holding taps, because tap shanks are not common collet sizes.
U
SING
F
LOATING
T
AP
H
OLDERS
Floating tap holders are probably the most common method of tapping holes. The tap is held in a quick change
holder that can float up and down slightly. This is done to allow the tap to follow the hole it is tapping and
compensate for differences in the accel and decel of the spindle versus the feed of the Z-axis. Upon reaching
the bottom of the hole, the feed stops and the spindle reverses, if you watch closely, you will see the tap pull
the floating holder out slightly. Upon reversal, the tap will be pushed back into the holder.
If the holder is pulled out or pushed in to it’s mechanical limits while tapping, you can break the tap, damage
the threaded part, or pull the tap completely out of the holder. Carefully watch for this condition when setting up
a job because it usually becomes a problem after the job has been running a while. Also tapping of diameters
less than 5/16 of an inch while below 1201 rpm (low gear shift point par 142) should be done in high gear.
Spindle reversal is quicker in high gear and will minimize tap pullout. This is done by putting an M42 code with
the speed command such as: M42 S900. Tapping is done with G74 and G84 cycles which automatically
reverse the spindle at Z depth. The feed rate can be calculated by using the HELP display and paging down to
the tapping calculator and inputting your speed and tap pitch into the control to obtain your feed rate that is
then input to the F command of the cycle. Example:
N100 G84 Z-1.0 R.3 F46.875 (for 32 pitch tap at 1500 RPM)