OK, I am not an expert but I have cut a number of threads on my lathe (and others) and have also done a lot of reading, dare I say research, on threads and cutting them. I see three ways for cutting a thread to match an existing, non-standard thread on a part.
1. Find the OEM's specs for that thread and work from there. I do not mean a simple DIAMETER - TPI spec. like 1/4"-20, but a real spec. with things like tolerances and class of fit. This IS the way that threads are made to fit each other, but in a working shop, chances are you are not going to have either the time or the where-with-all for this.
2. MEASURE the PITCH diameter and the thread pitch with a thread gauge. This is not a trivial process. In today's English/metric world, you need to check the pitch with BOTH English (inch) and metric thread gauges. And you often need to use a good magnifier to look for small amounts of daylight between the gauge and the thread.
The pitch diameter is the key. It is the pitch diameter that determines the fit between the internal and external threads, NOT the OD or the Minor Diameter, both of which are determined FROM the pitch diameter, not vice-versa. If you look carefully at the specs for a standard, Unified thread form, you will see that the OD can vary by a large amount. Generally, it will not be over the nominal OD, but it can be a significant amount smaller. On a 1.16" - 16 thread like yours, that could be as much as 0.010", 0.015" or even more. This is due to the allowances and tolerances on the size of the top land of the thread form. You can NOT measure the OD of a non-standard thread and come to any conclusion about it's true pitch diameter. You MUST actually measure the pitch diameter.
There are several ways of measuring the pitch diameter. The thread micrometer is probably the fastest and easiest to use. But it is also the most expensive as different anvils are needed for each thread pitch (or for a small range of thread pitches). And you must consult the proper tables for that thread mike to convert the reading to the pitch diameter. The three wire method is another way. It uses three identical wires that fit in the space between the thread flanks and a micrometer reading of the overall distance across them. It can yield accurate pitch diameter readings. But you need either tables or some math to convert the micrometer reading to the pitch diameter.
Once you have the correct thread pitch (TPI) and an accurate pitch diameter, you can set the lathe up to cut that thread. The OD for external threads or the minor diameter for internal threads can be calculated from the pitch diameter using tables or formulae found in standard references, like Machinery's Handbook. More below.
When cutting threads to a known pitch diameter measurement is of the essense. The three wire method will work for external threads, but for internal threads you will need another method. One possible way is to make a pair of GO and NO GO gauges. Or at least the GO gauge.
3. Use the existing part to cut a thread that mates with it. This may sound simple, but it is not totally so. I made that assumption some years ago but soon found out that there were complications.
The main complication is that pesky flat on the crest of the thread which is nominally 1/8 of the height of the thread. This flat is there to allow the crest of the thread to fit into the valley of the mating thread, which will also have some fill. So the crest of the thread can not be a sharp Vee if a good, close fit is to be had. And here is the strange thing, the flat at the crest is nominally 1/8 or 12.5% of the height of the thread while the root fill is shown as being between 1/8 and 1/4 or 12.5% and 25% of that thread height. On the face of it, this seems to be contradictory as a 1/8 flat would interfere with a 1/4 fill. Two things happen here; first, there are allowances for different classes of threads and that allowance can take up that difference. Second, in my experience almost no manufacturer of threaded devices seems to actually use that 1/4 fill which, technically is allowed. They all seem to shoot for the 1/8 root fill to match the 1/8 crest flat. Generally speaking, if you stick with the 1/8 or 12.5% figures for both, things seem to work well.
But the real complication when cutting a thread "to fit" an existing one that is used as a gauge is that when you cut a thread with a Vee shaped tool, the crest is not flat. It is a sharp Vee that sits above the flat that would match the present pitch diameter. AND, I don't know about the alloys that you are threading, but each and every alloy (steel, brass, and aluminum) that I have ever threaded has had a burr on that top edge after each pass of the threading tool. So you are fighting both the sharp Vee AND the burr when you are doing cut and try.
You can calculate the OD for an external thread or the minor diameter for an internal thread and cut/drill/ream those before you start threading. In fact, this is a very good idea as they provide excellent starting points and you can calculate the in-feed from there. But that does not guarantee that this calculated diameter will be correct for every instance of cut and try and it still leaves the problem of the burr.
So, if you are using the cut and try technique, you MUST insure that the flat on the thread crest is/remains there after each trial cut AND you MUST insure that all burrs are removed before you try the fit. This can be very time consuming and may make the cut and try method slower than actually measuring the pitch diameter.
Common to all the above:
You must ensure that the threading tool has the proper sized flat on it's tip as it will be forming the fill in the valley of the threads being cut. A tool for a 40 TPI thread is a lot different than one for an 8 TPI one.
With a known size flat on the cutting tool and a known OD or minor diameter, you can calculate the in-feed needed to cut to the proper pitch diameter. This is good, but in practice, I have found that it can be prone to error. Fortunately, the error is usually on the positive (too much material remaining) side and a proper measurement yields the amount of material that remains to be removed.
Always deburr before any measurements or checks of the fit are made. ALWAYS!
Remember that all classes of thread fit have an allowance between the pitch diameters of the internal and external threads. You do not want the exact same pitch diameters for both. Again, there are tables and formulae in sources like Machinery's Handbook for these allowances. If you must "wing it" you can use about 1% of the thread pitch for a minimum allowance and, perhaps 4% or 5% for a looser fit. Example: 20 TPI = 0.050" pitch and 1% or that is 0.0005" for the allowance. 4% would be a looser fit and about 0.002" for the allowance. With coarser threads you could probably get away with even more than 5%.
