View Full Version : Powered threadcutting!

Doc Nickel
05-24-2004, 12:11 AM
I had to do up thirty pieces with a coarse, short internal thread with a shoulder. Standard threading with a short bar was becoming time-consuming (and wasteful) since turning too slow (so I didn't over-run) left a poor, ratty finish, and turning faster gave me little or no reaction time- I'd either over-run, crashing the part, or I'd under-run, so the threads wouldn't be deep enough.

So, in one of those cases where making a time-saving tool cost more time than it saved, I made up a "powered cutterhead" so I could cut the threads to nearly full depth in a single pass, slowly and carefully.

First, I made a mount for my wedge-type toolpost:


That holds an air die-grinder like so:


I removed the hand lever, and the "button" is just tucked inside one of the clamping rings. The input air now has a flow control (quick and dirty speed regulation) and a 1/4-turn shutoff.

I turned myself a 1/4" shank threadmill out of 3/8" 01 drill rod and just gave it a quick hardening with a torch:


It all fits together like so:


I found the best system was to run the carrige up, lock in the threading lever, and just turn the chuck by hand. (It's a small lathe, and easy to do.) I turned it at probably four to six RPM, and got nearly-full-depth threads in a single pass. I then used a sharp bottoming tap to give each one a very light cleanup.


Six or seven hours to design and make the mount, the cutter and misc. plumbing (plus a run to the hardware store for the valve and throttle) and less than twenty minutes to run all thirty parts, and another ten to cleanup with the tap. Talk about a time-saver! http://bbs.homeshopmachinist.net//biggrin.gif

The head can also be used as a toolpost grinder (something else I've needed) and more importantly, with a set of the metric interpolation gears I got off Ebay a while back, I should be able to do metric threads in a single pass, and not have to worry as much about the threading dial.


Mike W
05-24-2004, 12:48 AM
Pretty slick Doc! Nice pictures too.

05-24-2004, 12:49 AM
Nice Doc. I did something similar a while back. I tried cutting outside threads using a slitting saw which I ground 30 degrees on each side, then ground clearance on each tooth. I know I didn't get the geometry right, since that was all done by eye, but it worked. My spindle mount can rock a few degrees each way, so I can set it to match the angle of the thread being cut. The cutter itself strays from center height, but the thread itself still comes out fine. It looks to me from your pix that the depth of cut is adjusted vertically, with the cutting action being in the bottom of the tube in the chuck, and not at center height. If the cutter's angle is set by rotating the mount on your toolpost, then the cutter centered front to back in the bore, it would seem an easy way to get the angles needed. Maybe not so easy to feed in the cutter without a vertical leadscrew, though. Just wondering if any of what I'm saying happens to jive with how you set it up.

05-24-2004, 12:53 AM
South Bend model A? Nice trick. Ground threads. I wouldn't have thunk that. Cool.

Doc Nickel
05-24-2004, 01:00 AM
Actually, no, the cutting takes place at 9 o'clock (looking at the chuck) just like usual.

I didn't think about having to angle the cutter to match the thread pitch until I'd already built the mount. I toyed with remilling the dovetail to match the necessary angle, but again, this was a customer run and time was getting short.

I "built in" the center height to the mounting block, there is no adjustment at the moment. When cutting, I simply left the depth-of-cut a tad shallow, and let the cleanup tap make sure the thread form was correct.

I had thought about tweaking the toolpost itself a bit, and either cutting at the top or bottom, but due to the slack in the geartrain, that recut a partial thread on the backout (I experimented with a piece of scrap) and ruined it.

It wasn't perfect, but it worked, and the threads are correct as near as I can tell. I may whip up another one eventually, with a bit of angle adjustment for the thread pitch, or even put some sort of adjustment into this one. In any case, the job got done and I can ship in the morning. http://bbs.homeshopmachinist.net//biggrin.gif


05-24-2004, 01:04 AM
I misspoke when I said ground threads. I did wonder about the helix angle, but if it gets the job done then it's good.

Doc Nickel
05-24-2004, 01:07 AM
<font face="Verdana, Arial" size="2">Originally posted by Evan:
South Bend model A?</font>

11" Logan, actually. Model 950 I believe? Used to be a "production" turret lathe, and it's got the nicks and scars to prove it. Works great! Came with the Buck "Set Tru" six-jaw, which has thoroughly spoiled me with it's concentricity (when adjusted) and holding power.


Forrest Addy
05-24-2004, 01:29 AM
Yup. That's called "thread milling" and you can do it on internal threads and external.

Thread milling on machining centers is common. The cutter looks like a tap but the teeth are annular instead of following a lead. The machined positions, infeed to thread depth, circular interpolates the tool path as the axial feed follows the thread lead. The cutter is over traveled slightly to pick up the lap, dials clear and retracted for the next operation. Dazzling to watch but don't blink or you'll miss it.

Ideally you have the cutter tilted to the helix angle but most common threads have a small helix angle (less than 5 degrees) so the generated flank angle error is slight.

You done good.

05-24-2004, 03:11 AM
..........Way cool Doc! Nice work. Did you bore the clamp holes in your fixture with a boring head. I have to make one of these for my ownself :-).

"11" Logan, actually. Model 950 I believe? Used to be a "production" turret lathe, "

When I saw the photo with the compound and the ways I thought "Logan" to myself. That's what I have, a Logan/Powermatic Model 1111011-L00H, made in 1981. It was used to turn plastic and had the crossbed dual toolpost and a bed mounted turret.

Great work and nice sharp clear photo's. Is this place and inspiration or what?


Doc Nickel
05-24-2004, 07:49 AM
No, I don't have a boring head for either the mill nor one large enough for the lathe. I did the large holes with the plates in the 4-jaw, stacked together.

Forrest says "I done good"? I'll take that as a compliment. http://bbs.homeshopmachinist.net//biggrin.gif I wonder if I can put that on a resume`...?

Tomorrow, I turn a new cutter, and see if I can have the same success with a fine-pitch double lead internal thread that's also kind of a pain...


Paul Gauthier
05-24-2004, 10:11 AM
Damn Doc thats brilliant. I gotta make one.

Paul G.

05-24-2004, 10:17 AM

Nice job.

As other have said this is "thread milling" with a slight modification of the technique we use on CNC mills.

If you do some web searches of manufacturers of thread mill cutters you'll find a chart giving the minimum inside diameter thread versus cutter diameter without causing unacceptable flank error and other problems.

For the double lead thread, you'll need the smallest diameter cutter you're comfortable running since the pitch will be double and more likely to have flank issues.

Maybe someday you'll want to spring for a ready made cutter. The smallest I have is from Micro100 Company, a TM-250, meaning thread mill with a .250" diameter. Solid carbide, very sharp and fragile, but does a nice job. The carbide should work well in the high speed die grinder. Moon Cutter Company makes HSS versions which aren't quite so brittle.

Can I assume you're doing conventional milling as opposed to climb milling? We have better luck with climb milling in the CNC's. If you aren't climb milling you may want to think about trying it. Start at the back of the thread and feed out. Normally climb milling is not done in manual machines, in this case the cutting forces are so low and with the mass of the chuck and gear train it's unlikely to grab and self feed.

G.A. Ewen
05-24-2004, 10:48 AM
Exellent technique! Thanks for sharing it Doc.

Doc Nickel
05-24-2004, 04:15 PM
For internal threading, it's conventional milling, for external threading it's climb milling. The die-grinder is not reversible, so to change that, I'd have to swap sides and turn the chuck the other way.

When I did experiment with an external thread, the finish was very poor- the cuts were highly faceted, notchy. I suspect the air-motor bearings aren't as rigid as they probably should be, and the climb milling let it chatter. Internal threading was far smoother.

I did look up ready-made cutters in MSC, but there was nothing in that shank size or with a small enough cutterhead. I'm sure they're available, but hey, it took me less than an hour to make this one. http://bbs.homeshopmachinist.net//biggrin.gif

The pitch of the double-lead should be even less of a problem for the helix angle; the bore to be threaded is larger, and it'll be a 16 pitch (32 tpi) rather than a 14 as the first one.


Spin Doctor
05-24-2004, 04:35 PM
Why not just run the lathe in reverse and cut the threads on the back side of the hole?

And to avoid the problems related to offsetting the compound to the right jus feed straight into the work. good sharp tooling and it should work fine. This way you can run the tool into the bore with a stop set on the ways and have no problems with overshooting on the way out.

[This message has been edited by Spin Doctor (edited 05-24-2004).]

Spin Doctor
05-24-2004, 04:39 PM
Nice idea though

J Tiers
05-24-2004, 04:45 PM
<font face="Verdana, Arial" size="2">Originally posted by Doc Nickel:

When I did experiment with an external thread, the finish was very poor- the cuts were highly faceted, notchy. I suspect the air-motor bearings aren't as rigid as they probably should be, and the climb milling let it chatter. Internal threading was far smoother.

Don't forget that internal threads "wrap around" the cutter. The approach and departure angles are relatively shallow.

The smaller the ID, the better off you are for that, although you may have to be more careful about thread angle.

The external threads curve away from the cutter, and thus have a much smaller arc of contact. The approach and departure angles are much steeper.

And, the smaller the OD of the part, the worse the faceting should be based on approach angle etc.

For external, I would expect you would have to increase cutter speed, and/or slow the spindle down. Or you could just have more cutting sections, per the commercial thread mills. That should knock off the facets by each row cutting in random orientation vs the prior facets.

05-24-2004, 05:14 PM
One advantage of thread milling like this that hasn't been mentioned is the ability to cut very coarse threads on less rigid machines as long as the machine's gear train supports that pitch. For instance, cutting an 8 pitch or coarser in steel on a small South Bend or equivalent can be difficult.

Several times I've used my CNC mill to cut a 2 pitch thread because my CNC lathe won't handle a cut like that when it gets down to the finishing passes, too much load on the cutter. A fairly light duty mill handles it just fine.

Incidently, if you ever run into a know-it-all carbide insert salesperson, ask him why internal and external thread milling inserts have different part numbers, but to the naked eye they appear to be exactly the same insert.

Forrest Addy
05-24-2004, 06:24 PM
Sorry, Doc. I didn't mean to sound condescending. If I saw instantly from the clarity of your presentation and the photographs that anyone could make a similar setup for thread milling on an engine lathe I should have said it in so many words instead of drooling out "You done good".

Doc Nickel
05-24-2004, 07:17 PM
Nothing to apologize for Forrest. I did take it as a compliment! I am (comparatively to most in here) still just a 'punk kid', and when someone with an order of magnitude more skill and experience than I have says "I done good", yer durn right I'm gonna take that as a compliment. http://bbs.homeshopmachinist.net//biggrin.gif

JT: You're right about the approach angle, though I still wonder if the climb/conventional has more to do with it, since the finish was almost a 'chatter', a rigidity thing. I'll definitely be doing more experimenting.

As for cutter speed, since it's an air-motor, I found it's basically all-or-nothing. Anything less than wide open and it wouldn't have enough torque to make a full-depth pass. Fortunately it was aluminum, I gave it a healthy dollop of WD-40, and I could vary the "feed rate" by how fast I manually turned the chuck, so I just turned it on full blast (earmuffs are a must!)

Spin: I can't thread normally (IE, not a powered cutter) in reverse since the Logan has a threaded spindle. I'm sure I can turn it backward manually with this threadcutter, but I haven't tried it yet.


Doc Nickel
05-25-2004, 07:19 AM
Update: I made another cutter, this time with two rows 0.030" apart. This let me do a 32 tpi double-lead internal thread, which is usually a real pain in the clavicle, in a single pass.

I ran 25 parts in the time it would have taken me to set up and run three, maybe four, by conventional threading.

Needless to say, I'm quite happy with this setup. http://bbs.homeshopmachinist.net//biggrin.gif


05-25-2004, 08:42 AM
Wow! There are a lot of lessons in those photos...thanks.

05-25-2004, 08:49 AM
Doc Nickel

Please contact me off-post at cfoster@villagepress.com regarding the toolpost


John Stevenson
05-25-2004, 09:05 AM
I'm impressed, very impressed.

There is an attachment for external thread milling in the Lathe Accesoroies book by Jack Radford, words and music but it can't do internal.

It would be interesting to see what the results were using a convention carbide thread milling cutter on a steel job.

I must admit I have looked at The Radford one quite a few times with an eye to being able to do single pass threading.
I had thought about using a steel disk as a cutter with the vertical mounted threading inserts fitted as opposed to the laydown version.
This way cutter speed isn't so much an issue.

John S.

05-25-2004, 09:38 PM
Excellent!I have thought of that in the past,but never had the occasion to try it,now I know it works!

You know ,i have looked and looked for 1/4" carbide burrs in the 60* profile and not found any,they do make them in HSS,but they don't last in steel.

Nice job,and I'll bet that setup would make excellent threads in wood.

Doc Nickel
05-26-2004, 07:13 AM
Cfoster- Message sent.

Here's the double-lead cutter:


Again, turned from 3/8" O1 and given a quick harden with a torch, though not was well done, I was afraid of burning off the tooth points. The two teeth are 0.030" apart to give a 32 TPI double-lead thread when turned at a 16 pitch.

And the finished bore (a little blurry):


The lead-in was a bit rough on some, I should have had a bit more chamfer to the boring tool when machining the steps. But they work, the parts fit, and each one (I ran 25) took a small fraction of the time they used to take with manual threading.


06-02-2004, 10:06 AM
Sorry to drag this post up so late. I've been on vacation. Way to go Doc!

This post is very interesting to me. I do this exact thing in wood. I have a high speed electroc motor (1" diam) mounted in a boring bar holder in my QC tool post holder.

I modify a lathe tool to do this. It is a PITA. I would prefer a tool like Doc made.

Weird and Dr mention commercially available cutters of this sort.

I would very much like to find a commercial made cutter like the one Doc made with a 1/4" or a 3/16" shank for very small (3/8)ID thread in hardwood. HSS or carbide makes no difference to me.

Anyone help? Many thanks as always.

06-02-2004, 11:47 AM
For commercial threadmilling cutters in small diameters go here:


I have the TM 250, which is a little scarey because of the necked down area. Every time I use it I'm sure it'll break.

02-04-2006, 12:51 PM
What works best to make the cutter from oil hardering or water hardering drill rod? Gary P. Hansen

02-04-2006, 01:21 PM
O-6 tool steel is the easiest to work with. I turned up this cutter, still haven't tried it yet. O-6 has a 125% machinability rating and turns almost like aluminum.


02-04-2006, 01:27 PM
Run with what you have. Oil will work as a quench for air, water or oil hardening steels, not the reverse.

The deciding factor is the hardness you draw it back to.

02-23-2006, 10:17 PM
Bumping back to the top. Gary P. Hansen

Doc Nickel
02-24-2006, 03:07 PM
Funny you bring this back up after all this time. I just built this small inserted-carbide cutter to use in my air motor, for threading some stainless parts internally.


It worked like a charm, but the larger diameter and the fact the tool mount isn't angled slightly to accomodate the angle of the threads, gave me some less-than-perfect threadforms.

I ended up cutting undersize and then running a commercial tap through it. Wasn't perfect, and in stainless was a pain in the tailbone, but it got the job done.

I need to redesign the cutter to better support the inserts though...


02-24-2006, 10:54 PM
Maybe an insert made for cutting threads might be helpfull. Hard to tell from the photo but those 60 deg insert look they were for general turning. I believe there are special ones made just for cutting threads. Gary P. Hansen