I'm doing some CNC threading on a lathe. I'm spending alot of time playing with the depth of cut to get things to come out right. I do understand that some time will be required playing to get it just right, but I'm spending too much.

I almost always cut non standard threads.

I have a ton of formulas to use, and I'm confused.

1 formula from the Machinist Handbook for tap drill size is:

Major dia. - (1.29904 * % of thread / TPI ) = tap drill size.

1 formula from CNC Programmers handbook by Peter Smid is for how deep to cut external threads is:

.613 / TPI = final depth of cut.

The internal formula from his book is .541 / TPI.

For 30 TPI, the sharp V thread is .0288 deep, but going from Smids formula, I should cut .0204 deep. Using 100% of thread and the formula from the MH, I should be cutting .0216 deep.

If I want a .600 x 30 TPI nut and bolt essentially, what methods do programmers use to figure:

1. how deep to cut the external threads
2. how deep to cut the internal threads
3. what size to bore the hole in the nut prior to threading?

Thanks

I cut a lot of non-standard threads when I am making tooling and fixtures for our own use; here is what I finally (sort of) standardized on.

I use threading inserts that are not the full profile type; they are supposed to be suitable for threads from 30tpi to 8tpi (or something like that). When you think about this, obviously the tip profile, if it is okay for 30tpi, is much sharper, i.e. it has a much smaller nose radius, than a full profile insert made just for 8tpi would have. This means that it is going to cut deeper than a full profile insert for any thread coarser than 30tpi. Which means that the formulae for calculating your ID, OD and depth of cut are maybe not going to give results that work. I decided to 'calibrate' my inserts and did some sample threads at 16tpi. My results where that the difference in diameter between my external thread OD and internal thread ID needed to be 0.065" and my threading depth for both needed to be 0.080" to 0.085".

This calibration seems to work, at least for my purposes. If I want to make a 2.1" OD 16tpi thread I make the OD 2.100" +0.000, -0.002, and cut the thread to 2.015". I bore the ID for the internal thread to 2.035" and then thread to 2.120" and can get a nice fitting thread first time.

I normally use G92 for threading because it is easy to tweak the diameter for the final pass; normally I tend to leave things a bit on the tight side and then just edit the final pass and run the threading cycle again. I use Haas and it is dead simple to do a program restart just for the threading cycle.

I have scaled this calibrations up and down for tpi; ie, for 20tpi just multiple the 0.065 and 0.85 by 16/20 and it comes pretty close. But it does not work if I switch to a full profile insert; then I have to go by the book.