Looking for a program to do a 3/4"-14 npt exterior thread on a lathe. I cannot figure out from the machinery's handbook how to figure out the "x" number in the 2nd G76 line......

Would someone explain how to come up the the "x" in the G76 cycle for both inside and outside threads. I can figure out the tapers to rough turn or bore the stock to. I can also figure out the "r" value in the G76 line, but not the x......

THANKS!

2. Here is a blurb on G76 threading. If you are doing an NPT thread you will have to use the R(i) value to taper the thread. The value is an interger number with 1 being equal to .0001" and is the difference in radius from Z start to Z finish. Hope this helps you out.

G76 P(m)(r)(a) Q(min) R(fin)
G76 X(Øfin) Z(len) R(i) P(k) Q(1st) F(L)

WHERE
m = SPRING CUTS (01)
r = CHAMFER AMOUNT(00)
a = TOOL ANGLE (80 60 55 30 29 0)
min = MINIMUM DEPTH OF CUT
fin = FINISHING ALLOWANCE
Øfin = ROOT DIAMETER
1st = 1ST CUT DEPTH

which program are you using to drive your lathe..Turbocnc mach3 etc...

4. Programs are for a 45 degree chamfer at .890 diameter.

.016R finishing tool

X.8539Z0
G3X.8836Z-.0062R.021
G1X1.0288Z-.0787
X1.05Z-.42
Z-?

.031R finishing tool

X.8239Z0
G3X.8748Z-.0105R.036
G1X1.0284Z-.0873
X1.05Z-.4348
Z-?

Threading cycle for a machine such as a Hardinge, Daewoo, Mori, etc.

X1.08Z.3
G76P000155Q30
G76X.9575Z-.85P570Q130R-.0358F.0714

Threading cycle for an older machine

X1.08Z.3
G76X.9575Z-.85I-.0358K.057D150F.0714A50.

This should get you in the ballpark.

Posting Permissions

• You may not post new threads
• You may not post replies
• You may not post attachments
• You may not edit your posts
•