Cutting threads from scratch (without a mating thread) can be confusing. You do not have a mating thread so you must work to the proper measurements. But, what are the proper measurements and how do you verify them.
First, I would start with the male (outside) thread because it is the easiest to measure. Here are the steps I would take:
1. Grind the 60° tool with a 12.5% flat (1/8 H) at it's tip. This flat will cut the root of the male thread and the values (12.5%) are at the low limit. So this tool will still be valid as it wears. It is optional, but I like to round the edges of this flat as that reduces the stress at the sharp corners that a true flat would have. This is completely within the thread specs.
2. Machine the area to be threaded to the proper OD. This can be found in the tables in MH (Machinery Handbook) for your diameter. It is NOT the nominal OD. In your case it would be between 1.4981" and 1.4809".
3. Set your lathe for 12 TPI.
4. Calculate the depth of the thread (12 TPI). 1/12" x 0.75 = 0.0625" That is the straight in (perpendicular) depth, taking the root and crest flats into account (12.5% for each). If you are using the 29.5° in-feed angle on the compound, then you need to divide that by the cosine or that angle: 0.0625" / cos(29.5) = 0.0718" That is the in-feed at 29.5°
5. Make a few rough passes stopping a few thousandths short of the calculated in-feed. Watch the flats at the crests to be sure you don't go too deep. Use a brass wire brush or extra fine sandpaper to clean any burrs from the thread: this is important as you don't want to measure burrs.
6. Now you MUST measure the pitch diameter. The OD or Major Diameter and the Minor Diameter are of NO USE at this point. There are too many ways that they can be deceiving. There are two ways of measuring the pitch diameter: thread micrometer and three wire method. Thread micrometers are the easiest, but $$$$$. Thread wires are inexpensive and you can even make your own and do the math for the size of wire that you use. (Note 2)
7. Continue taking light cuts (your tool must be dead sharp) until you reach the proper pitch diameter. De-burr the thread (step 5) before each measurement.
8. Check the OD again and bring it back to the numbers from step 2 above if necessary.
That's it. That should produce a 1.5" - 12 TPI thread to specs. Please note that the diameter that counts is the Pitch Diameter. It and it only determines the fit between the male/outside threads and the female/internal threads. The OD or Major Diameter and the Minor Diameter have a broad range of acceptable values and CAN NOT be used to gauge the thread being cut. Neither of them will guarantee the proper Pitch Diameter or the proper fit.
For the female/internal thread you will need to gauge it. If you only need the two parts to assemble properly with each other, you can cut that thread until the previously cut male/external thread fits with enough clearance for assembly. If these parts must mate with others that are made elsewhere or at other times, then you will need to make GO and NO GO male gauges using the above procedure but with pitch diameters adjusted to the minimum and maximum values (OK, a few tenths inside of) of the female/internal thread specs for 1.5" - 12. These Pitch Diameter limits can also be found in MH. MH shows 1.4459" and 1.4584" but I would use something like 1.4469" and 1.4574" to allow for tolerances in making the gauges: that still allows an acceptable range of 0.0105" so hitting it when making the internal thread should not be very difficult.
Oh, and your internal threading tool would also be made with that same, 12.5% (1/8 H) flat at it's tip.
Note 1: Part of the reason why OD or Minor diameters can not be used for creating a thread is the difficulty of grinding those 12.5% (1/8 H) flats on the cutting tools. For a 12 TPI thread those flats would measure 0.0104" wide. I don't know about you, but I would be hard pressed to grind and measure that with a decent tolerance. I think a high quality optical comparator would be needed ($$$$$). In practice I would just ensure that it was at least that big and go with whatever actual size I wound up with: perhaps a +0.004" / -0.000" range. You MUST use the Pitch Diameter for accurate measurements.
Note 2: The three wire method has been described in detail many times. You can search this board or the internet in general for these descriptions.
I'm new to single point threading. I've made a few before, but I just kinda did whatever untill it fit. Now I'm making a Inch and a half, 12 thread. Male and Female.
The problem is I don't understand the geometry
View attachment 253469
This is a CAD file I drew of my thread.
The OD and ID of both the Nut and Bolt make sense and align up like they should, but the threads are too wide. I set every measurement to what it says in the book. (30 machinery handbook).
I used the flat sizes for the major diameter on the nut and minor diameter on the bolt because that's what I have control over when I grind my cutting bit.
Does that make sense? When I'm cutting threads I'm cutting into the roots of the threads. The crests end up being how ever wide they end up. So that's how I drew my picture.
Please explain. I'm doing this for my work. I am the machinist department. (no formal training on it) I'm learning as much as I can. I've read a lot on these forums and youtube for my knowlege.
