Internal thread calculations

[Adam HarrisParticipant @adamharris13683]

When making a nut, how do I calculate the internal diameter of threaded nut needed to fit a metric threaded bolt with known Major diameter and pitch. I assume because the nut will have a lower height thread than the bolt, it is not a good idea to start boring to the Minor diameter of the bolt, but maybe what percentage increase on the Minor diameter is the place to start boring before thread cutting? My measurements are not standard  – the male (“bolt”) thread pitch is 32 x 2.0mm, with the actual external Major diameter 31.92mm. Is there a nifty calculator somewhere? Any help much appreciated as always!

[Adam HarrisParticipant @adamharris13683]

In my case of non-standard measurements, I do not know the Minor diameter but is there a formula for that too?

[EmgeeParticipant @emgee]

Hi Adam

Screenshot shows the info you need, link to the site is shown also.

https://www.ring-plug-thread-gages.com/PDChart/Metric-Fine-thread-data-30-64.html

Emgee

 

[JasonBModerator @jasonb]

Even if it is a non standard diameter the pitch is likely to be the same as another thread so just use a chart to see how much smaller the hole needs to be than the nominal dia and then apply to your particular thread.

M16 x 2 is a common standard metric coarse pitch and easily found charts for that give minor diameter of hole  as 13.835 so that is 2.165 less than nominal so apply that to any 2.0mm pitch, from Emgee’s chart above you can see that it works for M33 x 2

[DC31kParticipant @dc31k]

As above, it is the thread pitch and thread form that determine the _difference_ from nominal diameter. These figures are independent of actual diameter.

What does depend on diameter is the thread helix angle, which comes into play when considering clearance required on the cutting tool.

A good figure to print out is the diagram of the ISO metric thread form from Wikipedia. It shows the tip and root truncation numbers, which simply interchange depending on whether the thread is internal or external.

Unified threads have identical form, so the diagram covers most things you would need – the addition of a similar diagram for Whitworth form threads would probably get you up to 99.5% coverage.

[FulmenParticipant @fulmen]

For metric and unified it’s really simple, ID is nominal OD minus pitch (rounded up to the nearest 0,1mm).

[Fulmen]

On Fulmen Said:

For metric and unified it’s really simple…

The answer you give is normal practice for a tapping drill size, when you wish to tap a thread. It is based on a ‘good enough for most purposes’ percentage of thread engagement.

However, if you are screwcutting the thread, you need to be more careful in your calculations as there is a relationship between the ID of the blank part and the infeed depth of your screwcutting tool.

[Adam HarrisParticipant @adamharris13683]

Thank you Emgee that chart and website is just perfect!

[Adam HarrisParticipant @adamharris13683]

That is great Jason  – many thanks

[noel shelleyParticipant @noelshelley55608]

There are countless books that give this info. Zeus book, metalworkers Data book, The model engineers handbook Etc. Standard threads easy, non standard require a little maths but still simple. Noel.

[Adam HarrisParticipant @adamharris13683]

Thanks DC. So to clarify , in my example of 32 x 2mm pitch, if I manage in theory to bore out nut to exactly the theoretical Minor Diameter of female of 29.835mm (as per chart) and then start cutting the thread with a single point cutter to a perpendicular depth of 3/4 H, I should end up with a perfect mesh that would be an undesirably tight fit? In order to achieve the best case of both a comfortable spin-on fit and minimal wobble, is there an accepted industry practice of increasing the theoretical minimum diameter boring by some small fixed amount for a given pitch? For example , I note that Rego-Fix produce ER 25 nuts to the standard 32 x 1.5 pitch with an internal diameter of threaded part of about 30.55mm as opposed to the theoretical diameter of 30.376 mm. Should I also bore out nut to about 29.835 + (the correct increment for 2.0 pitch rather than the 1.5 pitch of ER25) before cutting thread? I realise the norm is for repeated trial fits throughout the cutting process but I just want to be clear about the best practice bore to start with when cutting a female inner thread.

[Adam HarrisParticipant @adamharris13683]

Talking about screw cutting the thread not tapping

[Adam Harris]

On Adam Harris Said:

So to clarify…

I feel bad about saying this, but it is not quite so simple.

First, the tip radius of your screwcutting tool will influence the infeed depth you need to cut the thread.

Let us assume you are using a full form thread-cutting insert (sometimes called a ‘topping’ insert). In that case, you can start with stock at the thread’s minor diameter and plunge to the depth given in the manufacturer’s literature (you could check the numbers, but I think they should be very close to the 5H/8 given in the Wikipedia graphic). The geometry of the insert assures the root and crest of the thread are correct.

If you use any other cutting tool, (e.g. hand ground HSS), you have to: (1) make some assessment of the infeed depth. If, for instance, it had a totally sharp point on it, you would need to feed in more than the 5H/8 (probably 3H/4) so the sharp point ends up in the right place. (2) increase the minor diameter as the cutting tool will not do anything to the internal thread tip.

Second, the diagrams show an idealised thread. The actual dimensions you use depend on the class of fit you want to achieve. That is the 5g/6H kind of thing in the ISO limits and fits document. If you do not know the class of the external thread, it would be quite difficult to make any judgement on the necessary class of internal thread.

If you are cutting something like an ER collet thread, maybe RegoFix has written down somewhere what class of fit is used in their products. If they have, that would probably be a good place to aim for.

You can play with some numbers in this:

ThreaDoctor: Advanced thread Calculator

The difficulty with all of this is that it is completely academic unless you have the means to measure what you are making (i.e. M30 x 2 go/no-go gauge of a defined class).

[DC31k]

On DC31k Said:

However, if you are screwcutting the thread, you need to be more careful in your calculations as there is a relationship between the ID of the blank part and the infeed depth of your screwcutting tool.

True, but I have never been able to cut proper fitting threads that way. The only way I know of is to measure the finished threads somehow. This can be as simple as fitting them to the mating part or a test piece, using thread wires (tricky on internal threads) or by measuring the OD/ID using full profile inserts.

[Adam HarrisParticipant @adamharris13683]

Thanks. The Machining Doctor looks another very useful site. However I notice the terminology is confusingly different from the ring-plug-thread-gages site in respect of the internal bore measured on a threaded nut. I thought this bore  was called the Minor Diameter (of the female/nut thread), as per the ring-plug-etc chart, with a value of 29.835 mm but in Machining Doctor “Minor Diameter” of the nut thread has a completely different value of 1.083mm (which is obviously in fact thread form height), and it is a “Pitch Diameter” that has the value of 29.835mm but this is a completely different measurement from the Pitch Line (mid peak-to-root) which is certainly not the bore diameter taken between opposing peaks.

Going back to basics using the Wiki ISO metric thread form diagram, it seems obvious that the nut bore should be the bolt external diameter (Major Diameter) less [the radial overlap (5/8 x H) times 2 since we want the diameter difference], and since H = (SqRt3 divided by 2)x P, nut bore should be 32-(5/8×1.73×2) = 32-2.16 = 29.84

[Adam HarrisParticipant @adamharris13683]

In terms of depth of cut , feed etc, that is very interesting but not wholly relevant to me given my assumption that the actual process of cutting will be ended when the trial and error of fit is acceptable by feel. I would still like to know the best bore to start with that gives me the best chance of a spin-on fit with minimal wobble

[Adam HarrisParticipant @adamharris13683]

As I say,  I imagine the exact theoretical bore of 29.835 or 29.84 of the threaded nut will be too tight to allow spin-on performance

[FulmenParticipant @fulmen]

Exactly, some clearance is needed. And the max/min diameters has little to no impact on fit or strength, so keeping it simple makes sense.

[Adam HarrisParticipant @adamharris13683]

Yes , after all this pondering it does seem that ” ID is nominal OD minus pitch (rounded up to the nearest 0,1mm)” is the way to go! Thanks

[JasonBModerator @jasonb]

The rule of thumb of nominal minus pitch is usually used for threading with taps and gives a reduced percentage engagement and reduces the risk of tap breakage.

If you are making your hole larger remember to allow for that on your depth of cut and associated with that is the tip radius of your tool as published data is based on a fully formed correctly sized radius

[jaCK HobsonParticipant @jackhobson50760]

I’m still not sure what to do. And why do I have most trouble with Brass?!

[JasonB]

On JasonB Said:

gives a reduced percentage engagement

No, not really. It should be smack in the middle of the 6H tolerances which are roughly ±0,1P.

 

[JasonBModerator @jasonb]

Certainly can on the smaller pitches where 0.1mm could be 25% of the the engagement. Plus/minus 0.1P is different to plus/minus 0.1mm or rounding up to nearest 0.1mm.

But the main thing to be aware of is that changing your hole size will affect other sizes that you may read on charts,etc and should be taken into account.

[FulmenParticipant @fulmen]

True, true. The rounding is only valid for normal sizes, but the rest should be valid for even the smallest threads.

[Tony Pratt 1Participant @tonypratt1]

From our old favourite Zeus book, M16 x 2mm pitch hole has a tapping drill size of 14mm i.e. 2mm less. I would suggest the OP bores the hole to 30mm, i.e. 2mm less.

Tony

[Author]

Posts