are three programming methods available for programming on Fanuc
based controls. We’ll look at the benefits of each method in the
next few articles of Shop Talk.
The production of an external or internal
thread requires several passes with a single-point threading tool.
The deeper the thread, the greater the number of passes required to
produce that thread.
The traditional threading method uses
G32/G33 codes. These commands require four lines of program code for
each thread pass. For example, machining a 3/4 - 10 external thread
could require 10 - 14 threading passes resulting in 40 - 56 lines of
Typically in a single pass threading
routine the depth is reduced in each pass as the diameter gets
smaller. Reducing the depth in this manner is necessary to balance
the load on the insert. As the insert goes deeper into the material
the area of contact between the tool and the part increases. To
minimize this contact area, smaller pass depths are programmed as
the insert approaches its final depth. Your insert supplier’s
catalog has information regarding the number of passes needed for a
There are two alternative programming
methods to reduce the programming effort. Today we’ll review G76;
this canned cycle method is very popular and suitable for many
threading applications. Only 1-2 lines of information must be
programmed, depending upon the type of control.
A Fanuc 0/18/21 control is often programmed
with 2 lines of code as follows. Let’s use a 7/8 - 9 TPI thread in
a modal program as an example. First, use the Machinist Handbook to
determine the major (outside) and minor (root) diameter of the
thread. Then, calculate the thread depth as follows.
thread depth = (major ø - minor ø ) ÷ 2
1111 (thread 7/8 - 9 TPI) ;
N10 G00 G40 G99 ;
N20 G97 S1090 M13
; (spindle direction & coolant)
N30 T0303 ; (tool
N40 X0.955 Z0.444
; (start position)
N50 G76 P010060 Q0050 R0.0005 ;
N60 G76 X0.7387 Z-1.50 P0.06815
N70 G00 X1. Z1. M09 ;
this 7 line program, 2 lines of code produce the 7/8-9 thread. Let’s
review each segment of these codes, we’ll start with program line
N50 = program line identification
G76 = canned cycle routine
The first two digits (P010060)
represent the number of spring (finish) passes. In this example,
there is one finish pass.
The second two digits (P010060)
represent the chamfer amount pull out. The 00 in this example
program a straight pull out.
To calculate the chamfer pull out,
multiplying the two-digit value by the thread pitch. Ex: P010560
= 05 x 0.111 = 0.0556 chamfer length.
The final two digits (P010060)
represent the thread angle. This value can be changed to suit the
thread angle required. A 00 would represent a plunge (straight)
Q0050 = minimum pass depth
value is programmed without a decimal point.
R0.0005 = depth of last threading pass
N60 = program line identification
G76 = canned cycle routine
X0.7387 = minor diameter from machinist
Z-1.500 = ending Z axis position
P0.06815 = total thread depth (amount per
Q0080 = maximum pass depth
programmed without a decimal point.
F0.1111 = lead of thread pitch = 1 ÷ 9
The Z start position (shown in line N40) is
recommended as Z0.300 or a minimum of 4 multiplied by the pitch
dimension. Ex: 7/8 - 9 TPI thread = 4 x 0.111 = Z0.444 dimension.
This approach allows the machine to accelerate to the correct axis
velocity before the insert enters the material.
An alternative method of thread programming
is to use the G92/G76 commands. Check back next month when we
discuss use of these codes and programming tapered pipe threads.