Internal threads, how do I know how deep?

[Investigator]

Actually I'm working on some hot rolled from the hardware store, just because it's what I had on hand.

 

[extropic]

It doesn't matter which one you make first. IIUC, you are making a matched set, not working to any standard dimensional requirements. They just need to fit together. Make which ever one you want first, then make the other one fit.

The poor finish you mention may be because of not high grade material.

 

[whitmore]

The 'cut external threads on cap until sharp crest' step is not recommended,
unless you want sharp thread form (which is awkward to cut and easy to damage);
usually you want a small flat (the tolerance for end-of-cutter wear when making
the mating thread). That means three-wire thread measure instead.

If you DO cut sharp threads, to nominal size, you might deburr with
another lathe skim cut, making the OD of the plug last.

 

[Just for fun]

I'm with the crowd to make the cap first. The hot rolled steel is not going to cut smooth. But shallow cuts and lots of oil will help. And also make sure your threading tool is on center.

 

[kered]

For 36 or 28 TPI, aim for a depth of about 1.5 times the pitch. After cutting, test the cap in the tube. If it fits snugly but isn’t too tight, you’re good.

 

[Jake M]

So, How do I know how deep to cut the threads, when its deep enough and not too deep?

To answer the obvious question, I will make a threaded 'cap' to fit the tube. The cap will have external threads of course and I will have the tube to use as a gauge for the cap.

So, you've got this part solved, the cap (which you can see and measure more easily) gets done first, and makes a gauge for the internal threads, which are impractical to measure otherwise.

Making a non-standard thread without a gauge is not trivial. First, you have "theoretical" dimensions to work from. That is, the major diameter is is based on a theoretical "sharp" thread form. An absolutely perfect triangle with theoretically perfect sharp points. The root and the crest are both "truncated", or "rounded over". Thus the minor diameter is never actually the listed minor diameter, because the "point" in the bottom of the groove is rounded over. That means your tool "touches" the work, and you're already "some" distance in against the theoretical depth of cut. So if you go in the theoretical distance, you're too deep.
And the crests- They're given a theoretical height, but in fact it's cut short of that. Because this is custom, one of a kind stuff (or any thread if it's just regular tolerance stuff, general hardware type precision, then once you have your major "nominal" diameter decided (however random that might be), take your desired diameter, and reduce that diameter by 10 percent of the thread pitch.

For the plug, If I picked 28tpi out of your two choices (neither choice is wrong, I just picked one), that's 28 threads per inch, or 28 threads per 1000 thousandths of an inch. 1000/28 is 35.7 thousandths per thread. Ten percent of that is 0.0036. Call it 4. So your "blank" diameter would be four thousandths less than whatever nominal diameter you settled on. And the threads won't come to a "point". Dang friggen close, but not quite.

The same thing goes for an internal thread, except inside out. What you'd do in practice is work out (from your male thread), what the theoretical root diameter is, enlarge that "slightly) by the same three and a half or four thousandths, and start threading into that. And when it starts to look like a thread, but is not "quite" there, that's when you start with the cap that is also the thread gauge. Start screwing it in, see if it goes. When it's pretty close to going in, but "not quite", start with scotch brite or other abrasive, buff the nasties off of it. Those will greatly affect the fit of fine threads. And might easily take an "almost fits" thread all the way to a "fits good" thread.

Tip- There are all kinds of blogs and videos all over the internet telling you it's OK to polish internal threads with hand held abrasives. In some cases they're not "wrong" but there is a LOT of judgement involved that never gets discussed, and there's a lot of bad judgement. Your (approximmately) 7/8 hole... That's EXACTLY the right size to bind up between your finger and an abrasive pad or stick..... Don't do that one under power. Just don't. Hand turning the chuck is fine, but you could imagine, right.......

And... Presuming the thread boring bar is decent, not crap, not industrial.... Make the last SEVERAL passes at a small, but consistant infeed. Perhaps (if it'll cut this shallow) 0.002 on diameter/ 0.001 on the radius. Making CONSISTANT changes in depths gets CONSISTANT cuts. Driving in at 0.006 per pass, and trying to take 0.002 is difficult at best. Maybe part way in, play with the spring passes (repeating a cut at the same setting as the previous cut), to see just how far the tool is deflecting. It IS deflecting, the question is just how much. That last little pass when you're trying to cut just a whisker to free it up just a little... That's not the time to find out how much spring is in the bar, on this day, with this insert, in this material....

Actually I'm working on some hot rolled from the hardware store, just because it's what I had on hand.

That stuff is crap. Very useful crap, I've been known to get it on purpose, but it's crap. It turns very poorly. Expect that, be prepared with flexible or pad type abrasives to "smooth up" the surface. It'll make very functional threads (not structural, but very functional), but it wants a little babysitting during the process, the tool finish is not great. And of course clean up the little nasties before test fitting, as each and every little "ugly" is actually a raised bit of metal, that'll interfere with the fits of the threads. It needs to be dealt with (to whatever degree is practical for the intention of the final product), before test fitting, as a good fit with rough looking threads will be a loose fit once you smooth them up.

 

[mksj]

Depends on the material as to ugly vs. clean turning/threading. Metal from hardware stores tends to be crap any way you turn it. I would recommend you start out on perfecting your threading technique doing external threads, just easier to do and if you have thread wires/gauge you can test your technique. I find that the dial increment for depth is always greater than the minor diameter, and starting out with the major diameter to big will result in ragged peaks that need to be knocked down if using a partial threading insert. In cases like these I make some go-no go external and internal threaded pieces out of scrap stock, this allows me to test parts threaded together and gives me the thread depth on the dial. I did this recently for some mill jack stands, I used a scrap piece of hot rolled 1045 turned to .995" with a 20 TPI thread and matched this against an internal thread cut in a ring of aluminum cut with the same internal thread.

Bigger lathes you can thread with the cross slide, smaller lathes the compound set to ~29-29.5 degrees. If you are getting crappy threads then either you have a technique issue, threading tool or the material is poor (assuming your lathe is in good working order and nothing is moving). I recommend zeroing your feed dial for advancing the cutter when the tip just engages the maternal, you can do a light scratch cut to verify the TPI, then a deeper cut usually 0.01" increments until close to target, then 1/2 that, and then a final dimension cut followed by a spring pass at the same diameter. You will always find that the actual thread depth will be greater than what the thread tables tell you. You also need to knock down the thread crests when using partial threading inserts.Once I have done a particular thread, I can do future threads of the same TPI with a high degree of repeatability. I print up the threading tables and then do notations as to the actual thread depth for my setup.

 

[SLK001]

I agree with the "cut the cap first" crowd. It is going to be the easiest way to have yourself a "standard" for the internal cut. Take care and do the cap thread depth properly (here's an online thread calculator) that will give you the proper numbers. Use the three-wire method (or thread micrometer) to measure the depth.

Chase the threads with a triangle file and a wire brush before measuring, especially with gummy metal. A bur not removed can really screw up a thread measurement. For HR steel, don't use a carbide insert, but instead use a very sharp HSS bit, honed to a razor edge. I would limit the DOC for a 28 to 32 TPI thread to initially 0.005" at first, then drop to 0.002" or even 0.001" as you near your target. Use spring passes until very little material is removed by your bit.

For the internal thread, you are limited to chasing the threads with a wire brush (I would use a stainless steel brush) - hopefully, your ID is large enough to accommodate a brush. If ID is too small for a brush, run a spring pass after every cutting pass before you test with your cap.

 

[Jimsehr]

I'm needing to cut threads inside a 1" tube. Actual ID is .875"
My plan is to take a small skim cut on the ID, and then cut either 36 or 28 TPI. Since this is not a standard piece, I have nothing to use as a gauge to thread in and see how it fits.
So, How do I know how deep to cut the threads, when its deep enough and not too deep?

To answer the obvious question, I will make a threaded 'cap' to fit the tube. The cap will have external threads of course and I will have the tube to use as a gauge for the cap.

I don’t cut a lot of threads . But after machining for more then 70 years I know you don’t have to use the compound at ALL.
You can buy a FULL PROFILE threading insert. These inserts are made to cut the full profile of thread . That means when you cut the last pass on thread depth
The insert cuts the crest of finished size. And also deburs the thread crest . You need to buy the insert that matches the thread pitch you are cutting.
I don’t put the compound on my logan lathe. I use the production cross slide.
And just dial in too thread depth .

Google full profile thread Id inserts.
Jim