Thread Milling (in Metal) on the Shapeoko (3)

This is something I have wanted to try for about a year, and it finally made it to the top of the To Do List.

The price of 1/4 shank Carbide Thread Mills is crazy expensive so I decided to use my Tool Maker experience and make one from an old worn 1/4-20 tap. The goal is to remove all the teeth except ONE! It really isn’t that difficult, since you have about 12 teeth (about) to practice with. Meaning if you make a mistake, grind off the mistake, and go to the next tooth. Once you have a single tooth on one of the 3-4 flutes, now it’s time to grind all the other teeth off slightly below the minor diameter.

Now the hard part. If the thread you are cutting is a 20TPI, you don’t need to do anything, but since I was cutting a slightly smaller, I needed to grind the helical angle on the top side of the tooth so that it wouldn’t rub. Some Dykem, some good magnification glasses and steady hand is what it takes (and practice)


She may not be pretty, but great for a trial.

PS Dykem on the tool so I could look for rubbing (Insufficient clearance)

Next, I used Fusion 360 to (a) design a tool that had the OP and length of my new (handmade) tool and wrote the program and posted it with my personal Post Processor

I used 5 passes to get to depth, but since the tool is HSS there was some deflection on the bottom and it took another 2 more runs of the program to remove the spring.

Speed: 10,000 rpm
Feed 11 in/min
Thread depth (0.055")
Actual Thread depth (Cut) 0.062
Lube: WD40 (of course)

The thread data is 12mm - 1.25mm x 19mm

I don’t have anyway to measure the internal pitch, but the top is a few thousands larger then and bottom, but overal I am VERY pleased with this first attempt.


@RichCournoyer So excited to see this post. Thread milling is also pretty high on my list. Although I’ll probably save for a new endmill since making my own exceeds my confidence level. Very, very impressed with your success!.


Very nice job. Any issues with tool balance?

1 Like

Oddly no. I tried to keep the offset mass as small as possible.

This might be a silly question, why would you want to machine a thread? Surely this would take longer than just tapping by hand other than a cool to do?


Great question.

Short answer: I don’t own a 12mm-1.25mm Tap (Yes I could buy one)

Long answer. As an engineer and a designer (with a home machine shop) I like to design items that use bolted joints, and (a) making sure that threads are perfectly perpendicular is difficult to do in a small shop like mine. I do have a hand tapper (see photo), but it has its limitations (3/8"). Secondly (b) are you familiar with tap sizes (More often called Class: GH1 - GH7)? Sometimes I want my bolted joints to have an interference fit, and having to but different classes of taps for all the sizes I use would be cost prohibitive. Lastly © driving a large tap (e.g. 1.0 inch) is very difficult, whereas machining a 1.0-inch thread is pretty easy on the Shapeoko. (Plus the short answer)


Rich -

Interesting hack to create a thread mill. I’m wondering how you chose that specific location of the tool, and did you just hand grind? I’ve not priced thread mills vs. taps, but I presume they’re less expensive.

One of these years I’m gonna fire up Fusion… Thanks for the post and pushing project limits.


I’m looking forward to trying this as well! Thanks.
Now if I’m understanding correctly from others I’ve seen, If the threads were actually 20tpi, you could have left a whole row of cutter teeth on?
I know yours was modified for metric, just asking if I’m seeing/understanding it right.
Another good reason to save broken taps :slight_smile:

I’m not sure I understand (how you chose that specific location of the tool).

Since I do not own a cylindrical cutter grinder, yes it was all ground by hand (actually that is how I was trained back in the late 70’s, learn to hand grind before you machine grind).

I chose a 1/4-20 because the 20 tpi makes for a large tooth, so it has a wider range for future thread cutting (in theory is should be able to cut from 48tpi to 20tpi. Now having said that, I also had to remove the helix to that single tooth, which is very tedious. But working with a tap gives you MANY teeth to practice with. Meaning do NOT remove the extra teeth until you have successfully ground a perfect single tooth. So in answering why did I choose that location? It is where the perfect tooth was.

I am still trying to locate a reasonably priced thread mill, and will probably work with a Chinese exporter and have some made up and try to sell them to other bold Shapeoko users (I figure they should cost around $15 (max) compared to $40 for US made tools. The difference in quality is negligible for a hobby machine.

I hope I answered your question (and more).


Correct. I was planning on buying some carbide taps and giving that a try in the future.

I see the benefit of one tooth doing more than one pitch, tho. Cool stuff.

Thread milling is… interesting.

Unlike single pointing on a lathe, or using a tap, where the cutting edges enter the material once and trace the full thread helix (at progressively greater depths), the cutting edge enters and exits the thread many (many thousands in general) times as it is rotating rapidly while the tool traces the helix. This means that the relief and clearances will not match without the extra work that RichCournoyer did, since the tool is ground at the factory with the pitch angle as part of the relief and clearance. Without the modification, there will be drag.

To leave multiple cutting edges, you would need to modify every ‘tooth’. Commercial thread mills come with this already done, whether they are ‘single form’ cutters (one circumferential set of teeth, all at the same axial position) or multiform (sets of teeth properly spaced for a given pitch)

THere is a lot to thread milling. I never thought of doing it this way. May take a stab at it, as I also find the price of off-the-shelf tools to be prohibitive for my own projects.


You answered my question (which tooth you chose), thanks.

I understand the basics behind thread tools and the ability to cut a range of thread densities. This is yet another realm I want to venture into with Shapeoko, so I’m hoping your tool creation efforts bear fruit. $40+ is not horribly expensive, but if you and C3D have an offering I’m all over it.


I understand you. Thanks.
I hadn’t thought of each tooth angle being ground away. Rubbing.

Very impressive! Had been thinking about this. Have an idea for some wood bolts and nuts incorporated in to a project. Will have to give this a go when I finish all my other projects. Thanks for sharing this.

I bought some a while back while waiting for my Shapeoko (still haven’t used them yet) but about six from the top of the list should begin 1/4" or 1/8" shanks.

eBay thread mills (corrected)

Edit reason - Wrong bookmark


That link isn’t much better, sorry.

How much were the thread mills and a picture of them would be great!

US $33.95

Yeah, I’m not spending $34 for a tool that should cost $8. (ok, maybe $12). Nobody thread mills in China, which is why they are almost 100% made in the US, and cost 1/2 an arm and part of a leg. I need to get a drawing to a couple of Chinese cutter grinder companies…(I’ve been saying that for a year)

1 Like

Just for the sake of my own enlightenment, how do they thread in China?