I need to program od threads for the first time. I need to thread 12MM x 1.75 6G. Don't know what 6G stands for. I have tried to read about threading but it seems to go over my head when they talk about leads and angles. Any that can explain this in simple english?

And they need to be .403-.463 in length.

6g refers to a class for an external thread. We don't do a lot of metric threads, but 6g seems to be the standard we make. Another external metric thread standard is 4g6g. Major diameter is the same for both classes. It is the pitch and minor diameter that are different. 4g6g has less toerance for the pitch, and a larger minor diameter.

In your case major diameter is .4711/.4607, pitch diameter is .4263/.4202 and the minor should be about .378. I never worry about the minor diameter. I use it only as a starting point. It is what it is based on the radius of the insert. Pitch is what has to be held. Once I get the pitch on the mean, I measure the root diameter, and change my program to match it if necessary.

Edit: Since this is the first time you've programmed threads, maybe I should also mention that the lead will be .0689

Thanks for the info g-codeguy. It's still quite a bit over my head. I tried to make some today but no luck.
This is everything i'm not sure of? We machine everything in inches.

G97 SXXX M33 P1
G0 X.__ __ __ Z-.XXX SXXX
G76 PXXXXXX QXXXX RXXXX
G76 X__ __ __ Z.XXX PXXXX QXXXX F.XXX
M98 P1

Thread length is .433".

M98P1 (THREAD)
T0101S1800M33
X.5Z.3
G76P000155Q30R.001
G76X.378Z-.46P445Q120F.0689
M98P1
------

I'm assuming P1 is a safe index subprogram. If it is, then there should be a G0 in it making it unnecessary to have one on the approach move. S1800 is about 212 SFM...pretty slow, but I don't know what the maximum feed for threading is on your machine. Machine's maximum thread feed is usually the limiter for small diameter threads. Vary Z-.46 to get the desired depth. I'm also assuming no shoulder or thread under-cut.

P445 is based on OD of .467 & root of .378. It will take .012 DOC for the first pass. It shouldn't take any less than .003 DOC until the last pass when it will take .001 DOC. Compound infeed is 55 degree. Thread pull-out is .1x.0689 for about .007. This will vary according to the RPM. Higher the RPM, the longer the pull-out will be. Only way to get it to .007 would be to drop down to about S900.

Edit: Normally I never use the R for controlling the last pass. If I am machining work-hardening materials, and having trouble with tool life, I may insert R.003 to maintain a decent DOC.

here is a example thread for my hardinge t42 maybe it will help. also with my lathe if i want to program in metric i need to program G21 in place of G20 at the start of the program.

N05(4"-8 OD THREAD)
G97S1000M13
M98P1
T0505
X4.300Z.500S960
G76P010055Q0015R0.
G76X3.8439Z-.980P0767Q0212F.125
M98P1
M01

Thanks for the help guys. I'm learning a little more each day :). I punched in your plan today g-codeguy. I finally made chips. But it made a smooth cut all the way. No threads! I double checked my typing and it all LOOKS good. I know how hard it is to explain to somebody instead of showing.

Thanks for the help guys. I'm learning a little more each day :). I punched in your plan today g-codeguy. I finally made chips. But it made a smooth cut all the way. No threads! I double checked my typing and it all LOOKS good. I know how hard it is to explain to somebody instead of showing.

Are you sure it is a 2-block G76 call? I've been programming threads for over 20 years. Nothing wrong with the example I gave you. Pretty hard to turn a smooth OD with a feedrate of F.0689!! :confused:

EDIT: Hate to ask this....BUT....Are you sure you are using the correct insert. On more than one occasion I have seen guys put a 16UN insert in a 16ER holder. Does a good job of turning, but no threads. :D

That is ok about asking about the insert. When you've had as much trouble as i've had to make these threads anything is possible:). The insert was the correct one though. I did finally get them to work with the assistance from you guys and we sat down at work and read the book over and over. Like i said it's working good now, but honestly i still don't understand all the calculations and coding. I will try to remember tomorrow to bring home what we came up with and maybe you can understand why the difference.

you know i was wondering what would happen if i neglected to place the point in the feed. (F0689 vs F.0689)? Although i don't remember now it sure is possible.

you know i was wondering what would happen if i neglected to place the point in the feed. (F0689 vs F.0689)? Although i don't remember now it sure is possible.

Pretty sure it should have been threading at F.00689 if you forgot the decimal point.