Another threading thread!

[devils4ever]

So, I plan on cutting my first thread on my mini-lathe and I'm looking for some info.

I'm making a captured nut puzzle with a 5/8"-11 thread and I'm trying to determine the depth of cut. Since the thread in the middle of the work piece, I can't keep trying a nut to see when the depth is correct.

I've read various websites on cutting threads and their depths, but the info seems confusing. I plan on moving the compound rest to 29.5 or 30 degrees.

Is the formula 0.75/TPI correct for how far to move the compound rest in? For example, for my thread would it be 0.75/11 = 0.068"?

 

[jbobb1]

I was given a formula several years ago that was similar (.7426/11). Never really used it, so I'd suggest making a test piece you can check. Keep in mind, any difference in O.D you're starting with will have an effect on the outcome.

 

[T Bredehoft]

I'd suggest making a test piece you can check.

Yes, make a short piece of 5/8, chase your threads, check with a nut, record final depth reading on the compound dial, repeat on puzzle piece.

 

[higgite]

When you get close to the correct thread depth, just unscrew the outboard half of the puzzle, leaving the other half in the chuck, and try the nut for fit. If not there yet, screw it back together and make another pass. Rinse and repeat until the nut fits.

29.5 degrees from perpendicular to the work piece is the correct angle for the compound. 60.5 degrees to the work piece. Have fun. That's a fun puzzle to make.

Tom

 

[RJSakowski]

Use pitch wires to determine the pitch diameter. The root diameter isn't all that critical as long as it is less than the specification. Check on Wikipedia for thread geometry. https://en.wikipedia.org/wiki/Unified_Thread_Standard.
If you don't have pitch wires, you could easily make an impromptu set from some piano wire.

 

[mikey]

The .750/tpi works.

A more accurate formula is: (Major Dia. – Minor Dia.)/2. This second formula will give you the total depth of cut when feeding straight in with the cross slide and with the compound set at 29.5 degrees. However, most of us feed in with the compound lead screw and this formula will underestimate the actual depth needed when using your compound. To calculate your actual depth required when feeding in with the compound, multiply the results from above formula by 1.1433.

For example, for your 5/8-11 thread, Dmaj = 0.625"; Dmin = 0.5135 for an 11 pitch thread. So, you have (0.625 - 0.5135)/2 = 0.05575" infeed with the cross slide. You have 0.05575 X 1.1433 = 0.0637" total depth of cut when using the compound feed.

Like all of these formulas, they are estimates that need to be confirmed either with a trial fit as you cut or with thread pitch wires or a thread micrometer. I usually start to check fits about 0.005 - 0.007" before I reach the estimated depth of cut for a class 2 thread. For a class 3 fit, I start checking about 0.010" before. For precision fits, go slow and remember to take a spring pass every pass or two to make sure you don't over shoot.

 

[devils4ever]

Thanks for all the responses.

Tom: I'm reluctant to unscrew the outboard end fearing loss of registration.

mikey: Where does the 1.1433 number come from? 1/cos(29.5)?

 

[mikey]

Yup, the reciprocal of cos 29 degrees. Its been a long time since high school Trig for me.

I hope you realize that formulas are formula; they are gross estimations and in no way precise. This is because there are SOOO many variables to consider when threading. Each thread has a root truncation (P/8), every tool differs in the accuracy to which it is ground or is worn, nobody ever gets their compound at exactly 29.5 degrees and on and on and on. Not to mention that there is a tolerance range for both major diameters and pitch diameters. This thread cutting business, if taken to extremes, can get really complicated.

Personally, when cutting threads I focus on just a few things:

• I turn the blank to the Dmaj tolerance range for the class of thread I'm shooting for.
• I use a sharp, accurately ground HSS tool most of the time and get it dead on center height and perpendicular to the work.
• I calculate an estimated total depth of cut with those formulas but do not trust them to be precise. The precision comes from the operator, not the formula. I start checking pitch diameters early and often and cut until I get the pitch diameter in the range appropriate for that thread. Nothing fancy, nothing anal, just practical.

If you follow all the formulas and calculations for every thread you cut it will take you forever to cut a thread; look in Machinery's Handbook and see what I mean. I suggest you buy some thread pitch wires or a thread micrometer and use the values found in the chart I'm attaching. It will make life a whole lot easier for you.

Find the class of thread you want, then look for the Dmaj range to see the diameter for the blank. Then cut the threads until you measure a pitch diameter that is called out for that thread and you're done. Don't forget to create a thread relief whenever you can so you have a place to end the thread; this relief should be about 2-3 threads wide and about 0.003" - 0.005" deeper than the Dmin diameter. Also include a 30 degree chamfer at the end of the blank so your threads have a clean place to start.

None of this is difficult once you sort out how to do it.

 

[MarkM]

If your feeding in straight with the crossslide it s .6134/tpi. Having your compound set at 29.5 degrees and feeding with your crosslide has no bearing on the 29.5 degrees. Your still plunge threading with the crosslide.
Keep it simple .75/tpi for threading with the compound set on anything less than 30 to 29 degrees.
I tend to differ regarding formulas being correct and using them with a grain of salt. Carbide threading tooling is very specific with dimensions and if you can grind a tool and are set up or know how to check your flats and such there really isn t much grey area unless you have other issues.
Good to learn both ways for those times you have no choice but to plunge. Keep it simple!

 

[higgite]

Thanks for all the responses.

Tom: I'm reluctant to unscrew the outboard end fearing loss of registration.

It shouldn’t lose registration as long as you don’t disturb the the half that’s in the chuck. When you screw the two halves back together, the thread should line right back up. No different than when you have to unscrew the two halves of the finished bolt to put the nut on it. Just make sure the two halves are screwed snugly together before and during threading and don't disturb the half that's in the chuck until you have finished threading.

Tom