[darrellx]

I am new to g-code programing and am having a problem programing a 3/4-16 left hand thread. Would anybody be willing to share a sample code for left hand threading.

Thank you in advance for your help.

Darrell

[deadlykitten]

hy as long as there are no interferences : flip a right tool 180* + reverse spindle sense + feed towards chuck; pls find attached variants; sorry, i can't provide codes

if you can program a normal thread, then i think you should have no worries with it / kindly

[darrellx]

Thank you for your reply Deadlykitten.

[g-codeguy]

Had to look up tolerances Online as I never did try to memorize thread specs. Way too much other chit on my mind. And easy to find the specs in the Machinery's Handbook.

Major O.D. = .7500/.7406
Max minor diameter = .6733

I couldn't thread using the O.D. tool as deadlykitten suggested. The tool would be hitting the part behind the thread on the parts we machine. Use a Left Hand O.D. threading tool. An alternative if the thread isn't too long is to use a Right Hand internal tool as shown in the lower left hand thumbnail that deadlykitten posted except, of course, you would be using it on the O.D.

The following is a basic Fanuc thread cycle. I show the spindle RPM only to show the direction it will be turning. The second 'P' is based on turning the O.D. to .746 diameter and with a .670 root diameter. The cycle is also based on not having a clearance under-cut behind the thread.

G97S1000M4

G0X.78Z.3
G76P000129Q30R.001
G76X.67Z-.875P380Q100F.0625

If there was an under-cut behind the thread, then I would change P000129 to P000029. This keeps the insert down all the way to Z-.875. The 01 withdraws the tool at the shortest possible distance before reaching Z-.875. Increasing the 01 will increase the distance it takes to withdraw the tool, Not something I've ever needed to do in over 37 years.

P000029 used with no thread under-cut will leave a ring at the rear as the insert stays in the cut at Z-.875 before withdrawing.