All -

Earlier this week my son and I made a four-flute thread mill out of 1/2" drill rod (using the Tormach as a vertical lathe), then torch hardened it and tempered it in the toaster oven. I have made several cutting tools this way so far, and they work well enough for me to keep making them.

Anyway, today I finally took the time to make the part I have wanted for a while now; it's a 1"-8 threaded TTS adapter for my 4" lathe chucks. I turned a TTS blank to 1" O.D. (again using the Tormach as a vertical lathe), then clamped the blank in the vise and ran the Mach-3 threadmill wizard. Since it's a close-fitting thread, I spent several hours making it, finally creeping up on the correct thread depth. It's a happy moment after that last pass changes the thread from no-go to go!

I have an old Craftsman (Atlas) 6" lathe, and I rarely use it for anything that requires precision or repeatability due to the frustration involved. Now I can use the 3- and 4-jaw chucks on the Tormach and get a precision, repeatable job on stock larger than 1/2".

I still have another TTS blank, but I don't know what I plan to do with it yet. Any suggestions?

Regards,

- Just Gary

The thread mill is very impressive. Have you tried it yet? How do the threads come out? I make a bunch of parts and have been tapping the 12. npt holes by hand .... labor intensive to say the least. I've shopped around for a threading bar or indexable cutter but without trying them out I'm hesitant to spend the $80-$350 .... you may have solved my problem.

No ideas what to do with your last blank .... but I'm sure something will come up :)

levelzero -

It was late last night as I was typing, so I didn't make myself clear. Sorry.

The threadmill (the first image) was what I used to make the 1"-8 thread on the chuck adapter (the second image).

It is actually the second threadmill I have made. I made the first one because my brother saw the Tormach and asked, "so have you made your left-hand nut and bolt yet?" Over the next several weeks I thought about it and decided that I'd learn more by making a threadmill than buying one. The end result was a left-hand 1/2"-20 aluminum bolt and twin stacked nuts for him, and more knowledge for me. Just to get his attention, the bolt head is also engraved with his email address. I didn't get a photo before I sent it to him.

I had to make a new threadmill for the chuck adapter because the first one would not cut deep enough for 1" threads (since it was for inside and outside milling of a 1/2" hole, I made it from 3/8" drill rod). The new one (from 1/2" rod) is a little too long to keep from flexing while cutting, and I didn't harden the whole shaft this time. I think I will harden it properly next time to help control flexure (and reduce the number of passes required to finish the job). They really are easy to make, so I don't have a problem with making a new one to fit the job every time.

Regards,

- Just Gary

very cool!

I have a tooling plate to make that will have hundreds of 1/4-20 holes and a thread mill is the perfect solution but they have always been too expensive. Would you mind posting some more detail on how you made the thread mill? Maybe some of the g-code you used to form the profile and how you ground the cutting edges. I'm impressed with the finish on the threads they look spotless. I can't see a single chatter mark.

thackman -

I'm not totally happy with the finish I got, but then again it was the first time I cut tool steel with a homemade cutter. I took so many light passes at the end that it probably work-hardened the part for me. The threads look as good as a die would have done, for sure.

The mills were pretty easy to make. Of course, for internal threads, yours has to be small enough to fit into the hole. You can flat-top or radius the tips of the cutters if you want (to match a true UN thread profile), but since I won't get inspected I don't really worry about it. Start by looking on Wikipedia (http://en.wikipedia.org/wiki/Unified_Thread_Standard) if you really have to care about the profile of your threads.

Grab a length of drill rod and lock it into a "spare" TTS set screw holder (I grind a flat first for the set screw). Both times I had to put the rod in a drill chuck first and sand down the diameter slightly to get it into the holder. Actually, the first attempt ended poorly when I tried to turn the part in a drill chuck. When the chuck popped off of the Jacobs Taper I figured out why I didn't like that method. You could get away with it if you only turn the part moving up the shaft. Anyway, get the rod mounted somehow. I like the idea of turning it in the same holder I'll use with it later.

I use a 3/8" lathe tool set that uses triangle inserts for turning. I mount it in a groove in a block of aluminum using set screws, then clamp the block in the vise. With a straight insert, it's pretty easy to get the 60 degree thread angle on your new threadmill. I did use SprutCAM to write the G-Code, but you could almost just step in by hand to cut the top and bottom of the V, then work up the shaft to cut the relief section.

Once you have the appropriate profile on your new tool (see the first image), chuck it in a horizontal rotary head (or figure out how to index four horizontal cuts at 90 degrees). I use a 3/8" end mill to cut each flute. Make the cut so that the bottom of the endmill cuts halfway (or maybe just a tiny bit past) through the part (to make the cutting face; see the third image), and far enough into the shank so that the new tooth will have a little chip clearance. After cutting the four flutes you should have something that looks (from the end) like the second image. I don't use G-Code for this, I just do all four flutes the same way.

Now get your favorite file and a good pair of glasses and file some relief angle into the backs of each cutting tooth. If you work from the back of the tooth to the front, you can watch the line left by the file as it moves forward with each stroke. Keep the line parallel to the tooth face, and stop just before it gets to the front of the tooth. Leave that last tiny edge for your final sharpening (after you harden the tool). Don't forget to do the top and bottom of each tooth, and maybe a little extra on the outside edge. You can profile a flat or radius on the outsides now, too, if you want them. The threadmill is more universal without profiled tips, since it will make a wider range of thread sizes. Note: It is possible to do all of this on your mill with a rotary table, but I don't fear files and I'm too lazy to figure out the complex angle to use, so I do it all by hand. It's not that critical as long as you get enough relief.

Harden the tool using your favorite method. I hold it vertically (cutter down) in vise-grips and heat it with an oxy-acetylene torch with the flame pointing mostly up. Try to get the thing a uniform deep red without overheating it (especially the cutting end). Remember, it is a small tool, and I am happy with limited cutting life, so I just do my best and go by color. Quench the part vertically to help reduce warpage. Temper to light straw or so (my toaster oven will eventually get there when set on broil, so I use it. My wife *hardly* complains at all).

Now stone the cutting faces and dress the last little bit of relief angle into the teeth using any decent stone or diamond block. Use a loupe if you have one to watch your progress. A test cut will quickly tell you if you got it right or need to stone in more relief somewhere.

Definitely test on scrap to adjust the cut before you begin your tooling plate...

Post questions, or more importantly, your progress, so we can see how you do!

Regards,

- Just Gary

P.S. If I can find a photo, I'll show you the six-flute taper reamer I made pretty much the same way. It warped a little when I hardened it, but it works fine for my application, and I couldn't buy one with the angle I wanted.

Not to rain on your parade, but you can buy those from micro 100, and they are carbide.

Just Gary, wonderful work! And thank you for the great and comprehensive DIY information. Thread milling is something I've been wanting to try for a good while but not wanting to spend the $$ for a carbide bit I'm likely to break on the first try... ;)

Randy

Just Gary, wonderful work! And thank you for the great and comprehensive DIY information. Thread milling is something I've been wanting to try for a good while but not wanting to spend the $$ for a carbide bit I'm likely to break on the first try... ;)

Randy

no guts, no glory!

...but that is exactly where i am at with thread milling. maybe i'll break down this week and buy a thread mill i can't afford. i have a project that needs one. unfortunately the one i need is probably going to be the most expensive. i need to thread 5/8-24 from z-.9 to z-1.5. it looks like micro 100 has one that will work with that depth. now i need to figure out how to buy one.

Absolutely fantastic write up. I'm nut sure I'd use home made tools for production work but for one offs or in a pinch this would be perfect. It would also be great for those time you need to make a single part with a very oddball thread pitch.

Not to rain on your parade, but you can buy those from micro 100, and they are carbide.

Whats the price though? I think the reason many avoid thread mills is the cost. Thread milling is great compared to hand tapping but sometimes you have to balance time/cost and when it comes to experimenting with new tooling I know personally I'm not always willing to risk hundreds of dollars on the hope that it saves me a few minutes. The other problem is with machining operations you've never done before the chance of breaking things is much higher so now instead of buying one tool you may have to buy 2-3 until you fingure things out.

Randy -

Thanks for the kind words. When you get around to trying thread milling, just remember that the load on each tooth grows with every pass since you are cutting a triangle. You could do it like on a lathe where you also step down the thread just a bit, but that's too much thinking. I took lighter cuts as I went deeper to help balance the load.

I used far too many passes since I didn't want to waste a part learning the right depth (and I wanted a tight thread), but you could quickly learn how to do it in only two or three passes if you had some practice material.

DSL PWR:

On the contrary. I have seen them for sale, and I probably spent more than $50 in my time making each of them, but I got at least four things out of them:

I got to learn more about my machine and cutting small parts out of tool steel (and I do need the practice);

I got a working thread mill in a few hours rather than waiting for several days (and no shipping cost!);

I got the confidence of knowing that if I break one or need a different size I can make another if I choose to (which is a *very* liberating feeling);

and, perhaps most importantly, I got some quality time with my son while he was home from college (worth all of the others combined).

Besides, if I hadn't made them, I wouldn't have posted this thread, and you would not have told me about Micro 100. They also have some good programs and tips for thread milling on their site. Thanks!

Regards,

- Just Gary

P.S. If I had hundreds of holes to thread in a tooling plate (especially if it were a steel plate), I would seriously consider buying a carbide threadmill for $50. Wait! What am I saying? Of course I'd still make my own!

What's funny to me is that I posted this for the lathe chuck idea. I can't wait to get to use it for lathe projects, or to hold round stock repeatably in the milling vise.

I just figured that you guys were all old hands a thread milling, and reluctantly decided to show my home made one. You just never know what someone else might like to see...

I'm glad you enjoyed it!

- Just Gary

300sniper -

I could almost swear that I have also seen carbide threadmills in the MSC Big Book (for pretty much the same price), and they have a 35% discount on cutting tools going on right now. If so, you could save about $15 on one.

Regards,

- Just Gary

300sniper -

I could almost swear that I have also seen carbide threadmills in the MSC Big Book (for pretty much the same price), and they have a 35% discount on cutting tools going on right now. If so, you could save about $15 on one.

Regards,

- Just Gary


just about all the suppliers sell carbide thread mills. i hadn't seen one that could reach 1.5" deep into an internal thread until i looked at the micro 100 site.

thanks again for your post on making your thread mill. now i know it can be done if i do need something special. i need to start studying up on the hardening process. what grade drill rod did you use?

Thanks for the info Gary that was just what I needed. I've been confused as to why commercial thread mills (single tooth) were often only listed for a single thread size and reading through this cleared that up. It's because of the tip radius changes w/ thread size. You would want want a much larger root radius on a 2" bolt vs #6 screw.

The multi-tooth indexable threadmills seem to be fairly common (and expensive) but I haven't seen many like this. Enco has a few but they only go down to .250 which is too large for 1/4-20. I checked Micro 100's site and it looks like their threadmills are between $50 and $200. Which is far to expensive for me to experiment with but certainly reasonable for production. I'm going to make a few and get the process down and if it works out I'm going to try making one or two for ACME thread forms.

Does it matter if the thread root is rounded or flat? Most of the illustrations I've seen show rounded roots but the Micro 100 mills have flats.

300sniper -

The first tools (smaller threadmill and a taper reamer) were made from water-hardening drill rod. The bigger threadmill is oil-hardening, but I quenched it in water anyway (it is small, and would have quenched about the same in oil). I switched to oil hardening to try to help control warpage during the quench. Ideally, I guess you would want to grind to size after hardening.

I have some old peanut oil I plan to use for quenching whenever I figure that it really matters. It should smell good, at least.

thackman -

The shape doesn't really matter, but you could argue that a rounded edge will be stronger than a sharp corner. If you are after maximum strength, you probably want to round them. Sometimes (like dirty conditions) you want a little extra room at the tips of the threads so the junk has a place to go.

Remember to post pictures!

Regards,

- Just Gary

Very nice thread, thank you for sharing it!

Best,

BW