Metric Fine Threads

Hello everyone

I'm currently working on a pen made from stainless steel utilising a shake mechanism I got from a German supplier, the shake mechanism has an obscure thread on it M7.5x0.5.

I bought a tap for this and it’s worked fine but I’m now trying to machine an external thread for the top of the pen body and I can’t find any information for the max and min diameter for the external threads so I can cut these on the lathe.

I’ve got a copy of machinery handbook, but can find any information on this particular thread, I’ve even tried subtracting the pitch from the M7.5, but it’s really slack…

Can anyone help?

Cheers

Martin

Edited By Martin Currie on 24/08/2023 18:05:21

Base it on any common 0.5mm pitch metric thread such as M3 and simply add 4.5mm to the diameters

If you do a bit of research you will find all the formulae for thread dimensions. It is not as simple as deducting the pitch from the diameter as root and crown radii are involved. Even after calculating and having the right radius tool. You will need to machine it until it fits, this is where thread gauges come in but the expense is outside of our remit.

Martin

Plenty of info here on M fine threads, not in the exact size you need but will give you some idea.

**LINK**

Emgee

From Emgee's chart it should become obvious that any 0.5mm pitch thread has a minor diameter that is a constant amount less than the OD

M4 x 0.5 has OD of 4.0mm and minor dia of 3.387

M5 x 0.5 has OD of 5.0mm and minor dia of 4.387

M5.5 x 0.5 has OD of 5.5mm and minor dia of 4.887.

All are 0.613mm less than nominal

So for your M7.5 x 0.5 you want an OD of 7.5 and a minor dia of 6.887 (7.5 - 0.613)

As I said something like M3 x 0.5 has a Minor dia of 2.387 so if you added 4.5 to that you would get the 6.887

Edited By JasonB on 24/08/2023 18:54:16

To amplify Jason's point, for _any_ thread series (ISO metric, UN, Whitworth, BSCy, PG)* where a particular pitch is used on more than one diameter (so, really anything except BA), the depth of thread is only related to pitch and form (geometry).

In particular, it is independent of diameter. You can cut 1mm pitch on 6mm diameter or on 50mm diameter. The amount you plunge in is the same.

The only place diameter has an influence is when calculating helix angle, which determines the clearance angles required on the cutting tool (the M6 x 1.0 will have a much steeper helix to M50 x 1.0) .

* ISO metric and UN use identical forms, so really this is a list of four possiblities, not five.

Meytric threads make life easy.

Thye Tapping size will be Nominal - pitch.

Thus M6 x 1 is drilled 5 mm.

I cut some internal 5 x 0.5 threads using a 4.5 mm drill. For externals, I used a Die, but if screwcutting would have gradually increased the infeed to the 0.3067 shown in my Zeus charts, for a full depth thread.

The 6 x 1 thread has a depth of 0.6134, but has a flat of 0.125, so the hole shopuld really be 5.232,.but the 5mm drill used by many of us produces a useable thread for most purposes.

Unified threads are truncated so applying the same sort of calculation, based on the pitch, will work.

Whitworth form threads (BSW, BSF, BSB, BEC, ME ) being n55 degree make the calulation a little mor difficult, mand nthe threads bshould be round topped rather than flat

For most purposes, Zeus Charts, or Model Engineer's handbook will provide the theoretically precise dimensions, and often the nearest drill for Tapping..

Howard

I buy the partial form outside threading inserts in the pitch I want. Then cut the outside of the threaded about 0.1 to 0.15 larger in diameter. I then cut the thread until the outside is a little smaller diameter than the nominal of the thread designation. So on a 7.5 X 0.5 pitch thread will make it down to 7.48mm to 7.46mm on diameter.

How does that work Ick?

All the partial form inserts I have seen tend to cover a range of pitches eg 0.5 to 1.5

If I wanted to cut say a 0.75mm pitch I would have to by a full form 0.75mm pitch insert as I can't by 0.75mm partial form

It doesn't.

The partial profile inserts are not 'topping' inserts.

Every major insert manufacturer spends a lot of time and money producing literature describing their products. The literature stresses that for partial profile inserts, the stock diameter is critical.

See bottom of page 10.

https://usercontent.azureedge.net/Content/UserContent/Documents/034353.pdf

I call them partial inserts, as the full form ones that I was used to, looked more like the Sandvik insert style.

What I am using is called now the full form insert, and will radius or put the thread form on the crest of the thread.

The V tools , I call them a generic insert, and will have a radius that only matches that of the finest pitch it is suited for. Like the 0.5 to 1.5 , the root radius really is getting too sharp for my liking for a M10 X 1.5 pitch for example.

There are ground inserts and pressed form inserts. For the finer pitches, I have only seen the ground inserts. The pressed form inserts like those from Mitsubishi, has a great geometry for breaking the chip.

For finer pitched threads and the odd ones, 0.6 , 0.4mm or 0.35 as examples, I have not seen the pitch specific inserts. For these I use thread gauge wires, but recently got myself a thread mic with a set of anvils for the range of threads I am ever likely to come across. It covers from 0.3 to 3.5mm pitches, but is only in the 60 deg form. With Whitworth I resort back to the thread wires and white grease.

My thread inserts go from 0.5 through to 3mm pitch, and I do have a few Whitworth ones and a few UN pitch inserts . I went this way just from the easy way to make External threads.

I also make truncated thread forms as well, where a partial depth of the thread is created, like a M10 x 1.5 that has a root diameter of 9.1mm and the nut has an inner diameter of 9.15 to 9.2.

Like been said, there are tables and lots of information about thread forms and root radius etc all on the net or in Zeus books etc.