@Anonymous wrote:
While looking for answer I stumble on 2D threading, which I have honestly not used yet. I just started single point threading.
*Pitch Diameter offsett*- what is the purpose of this function? Why would you use it?
If using a .160 Diameter cutter for .25 I understand I could use a negative stock to leave value to increase the size from not using a "dedicated 1/4 size tool"
The 2D threading that you're looking at is more for milling than turning. In fact, I don't know that it would even work for a turning operation, but I'm really not sure. It's intended for use with thread mills, which come in a variety of shapes and sizes, but the ones that I use look like this, and with just a couple sizes I can cut any 60-degree thread that I need, all the way from about a #6 up to 1.5" or so. (I could get bigger ones to do bigger sizes, but I just haven't ever had the need to do it.) There are other types as well, that can only cut a single thread pitch, but those are not as flexible as I'd like so I don't bother with them.
The way that these thread milling cutters work is that you drill a hole and then you run the tool around in a spiral of whatever pitch and diameter you like so that you can have milled threads at the end. (This does require that your mill is in good shape, though, because if there's a lot of backlash then you wind up not getting the threads cut properly.)
Because these thread mills can do many different thread pitches and diameters, you need to specify your thread pitch (which you already understand) and you need to specify your diameter offset, which is the part you had a question about.
Pitch Diameter Offset is, theoretically, the difference between the major and minor diameter of your threads. This is accurate... but only to a point, and when you're using thread mills you're going to find that the major and minor diameters are NOT necessarily what you think they are.
Let's do an example. Say that you want a 1/2-32 thread, and you're using that thread mill that I linked above from MSC. It has a minimum thread pitch of 32 TPI. This means that the tip of the cutter (P/8 in your diagram) is small enough that it can make the profile for 32 TPI accurately, which would make it about .004".
We'll assume for the sake of the example that the cutter exactly matches the profile at the nominal thread major diameter, and that we drilled the hole at .416. The pitch diameter offset is, then, .5-.416, which equals .084", and therefore the thread mill will spiral up through the hole cutting a circle whose diameter is .084" greater than the drilled hole.
But what if I want to do a 1/2-13 hole instead, using that same cutter? Well, in this case the nominal major diameter will not work, because the tip of the cutter is .008" thick, while P/8 for 13 TPI is almost .01". The threads will be cut too shallow and your bolt will not fit the hole, if you cut using the same .084" pitch diameter offset. In order to get the P/8 dimension accurate at the nominal major diameter of .500", using a tool that has a tip thickness of .004", you would need to add 5 thou to your cut depth, which means 10 thou to the nominal major diameter. So, your pitch diameter offset calculation becomes .500" - .416" = .094".
I'm not at a computer with CAD available right now, but I can draw up something for you later with a more visual explanation, if you need it.
Rusty
