What's new
What's new

Nomenclature Metric Thread Tolerances Calculation

Human

New member
Greetings, experts!

I'd be eternally grateful if one of you could teach me how to CAD a thread, "the easy way", preferably.
I've already done the profile as per attached visual. This all works great and reliable however tolerances are missing.
My question; how do we go about computing/calculating those tol based on the ISO nomenclature formulas?

I understand there are several online calculators computing major/minor/etc, but I'd like to have those formulas added as expressions to the the existing nomenclature base profile formula. Not sure if this makes sense... happy to clarify the question if I'm asking the wrong way.

Thanks

Profile-Calculation.jpg
 

sfriedberg

Active member
TLDR: Get the specific tolerances from the standard. Don't try to compute them.

I can't tell if you want to know how to draft a threaded component on a blueprint (or CAD system), or cut one on a lathe.

If you are designing (drafting), and if you are not doing some God-forsaken special thread, then state the simple nomenclature on the drawing and refer to the standard for the tolerances. Generally, the nomenclature will specify class of fit, rather than explicit +- on diameters, and the tolerances will be different for the male and female threads. And you have no need to reverse engineer the thinking that went into the standard. Just reference the standard.

If you are machining, and if your customer did not hand you some God-forsaken special thread, then open up your copy of the standard (or the relevant data which is available in tens of printed handbooks and uncounted hundreds of websites) and take the tolerances directly from the standard's tables. You have no need to reverse engineer the thinking that went into the standard.

Finally, one thing that really confuses a lot of people when they first encounter it, the ANSI and ISO thread specs rely heavily on profile tolerance. You will not find anything about tolerance on flank angles, for example, because any flanks that fit within the profile tolerance are acceptable.
 

Human

New member
Thanks, sfriedberg.

The end goal is indeed to have threads machined on a lathe. At this stage I'm looking for a methodology to have sketches automated by expressions for when I need to add a thread profile to a geometry (drag & drop, ideally). I'm really only looking at the mathematical formula to add to the base ISO nomenclature profile standard (as seen on the OP's visual) for both positive & negative tolerances.

All I'm trying to achieve in this early stage of learning the great science of threads & tolerances (new to me, btw).

See attached visual to visualize what I'm doing and where I'm at with this. How do I add e.g. the 6g and 6H tolerance to let's say the Dedendum calc? Is this a simple matter of looking up the h&H tol in the standard publication and adding/subtracting it?

M10x1-50-Nomenclature.jpg
 

JST

Moderator
Do you actually need to 3D model the actual thread?

All I have ever done for that is to call out the thread size and class, and the length of it. Has never been a problem.

Unless you are doing some sort of 3D printing, I am not seeing why the thread itself needs to be exact in CAD. It will probably make the model a lot bigger file-wise, slower to display, etc, and it doesn't seem as if there is an advantage.

Maybe you can explain why you need to have it exact in the model. And what CAD you are using.

If the CAD is some integrated system such as Boeing uses, then I can see it, maybe, since theirs also integrates into 3D simulation assembly and service training. But then you would not be asking.
 

Human

New member
All fair points, JST.

Was actually hoping that nobody ask because the answer is quite embarrassing; I've always been spoiled and used the CAD commands and their built-in lookup thread tables. Aimed the CAM toolpaths on crests & roots and just like magic, that always worked kinda great (for my own prototypes and gizmo purposes anyway). Probably luck more than anything else.

Truth be told I need to learn all about M threads & tol from scratch. And so soon could be a good time to begin from the start (i.e. drawing basic profiles) and move on to automating tol, so to be able to reliably call threads + tol on geometry. Theoretically anyway. Let's hope this brings practical advantages over let's say cad standard sizes lookup tables.
 

sfriedberg

Active member
How do I add e.g. the 6g and 6H tolerance to let's say the Dedendum calc? Is this a simple matter of looking up the h&H tol in the standard publication and adding/subtracting it?
If I understand your question correctly, the answer is "you don't do that." The hole/shaft fit clearances/interferences do not apply to internal/external thread sizing. That role is played by thread class of fit. The ANSI UN thread standard calls out only three classes of fit, not the 20 or so combinations you get in the hole/shaft fit standard. I imagine ISO M threads are similar.

Let's hope this brings practical advantages over let's say cad standard sizes lookup tables.
Probably exactly the reverse. If you start putting explicit tolerances (other than "class of fit") on a thread callout, the shop is either going to ignore them (bad shop) or look up the standard tolerances and try to figure out what part of your specification is non-standard (good shop). On the other hand, if you just use the standard nomenclature (including "class of fit"), the shop can use its standard tooling, gaging, and processes (including quoting!).

[Added in edit] Assuming we are talking about making threaded parts, and not making thread gages, there is at least one thing I neglected to discuss. If you need to cut a threaded hole oversize, for example to allow for plating or shrinkage in heat treat, then you can get oversized taps in various increments above the nominal size. However, size tolerances on these holes still should be determined by the nominal thread size and class of fit. For all practical purposes, the oversize taps just increase the nominal diameters by a fixed amount (not proportionally).

If you can, stay out of the space of God-forsaken special threads, and especially annoying God-forsaken special threads which are almost a standard thread.
 

Human

New member
Kind of you for taking to time, sfriedberg. Slowly starting to get a feel of how it's done professionally (effectively?), thanks.

However still very much confused with "drawing" a 2D M thread w/ tolerance variables from scratch. It would be so helpful to have an example of let's say a M10X1.50 6g screw and its mating M10X1.50 6H bolt so I can reverse engineer the formulas. Strangely enough I've spend an hour looking on the www yesterday for a 2D example of a 'commercial/general purpose' ISO 965 standard just so I can validate my understanding against the standard, and just couldn't find anything anywhere. Not even a dxf or a 3d step file. Starting to believe I'm the only one who cares...

Regarding 'practical advantages' I had in mind insert/tool profiles selection, design validation, and of course linear strains & stresses analysis of different thread profiles/tol/geometries.

The hole/shaft fit clearances/interferences do not apply to internal/external thread sizing.
According to this table the tol is added or removed from the basic thread profile's H, dD, etc. See Important Calculations.
ISO Metric Thread Tolerance Tables | Accu(R)


If you can, stay out of the space of God-forsaken special threads, and especially annoying God-forsaken special threads which are almost a standard thread.

Ideal and perfect world's my hope too however chances this truly exist is slim. Take oxidation thicknesses varying by several anodizing methods/requirements for instance. Not complaining about the CAD lookup tables, they are fast and great for most cases as you've stated however those are pretty generic and often doesn't offer a great deal of customization, let alone true 2D/3D profiles representations.
 

Mechanola

Active member
Dear Human

Unless a non-standard tolerance is needed you don’t put any tolerance on paper, just note M 11 for example. Please hit the space key after the M.

There are no positive and negative tolerances. What you mean are deviations, in French écarts.
 

sfriedberg

Active member
According to this table the tol is added or removed from the basic thread profile's H, dD, etc. See Important Calculations.
ISO Metric Thread Tolerance Tables | Accu(R)
Yeah, I just learned how the ANSI and ISO standards differ. I had assumed (incorrectly) that the ISO standards were similar to the ANSI standards in this regard.

However, please be careful with those tables. An allowance (or deliberate deviation from nominal) is not the same thing as a tolerance (allowed, but unintentional deviation). That webpage has tables of both allowances (for the equivalent of ANSI class of fit) and tolerances. Without consulting 965, I am not sure if the tolerances are symmetric and bidirectional. The formulas given on the webpage only apply the tolerances in one direction (separately for internal and external), to obtain the extreme dimension, but the standard may specify dimensional limits of +- tol, rather than -0+tol.
 

Human

New member
However, please be careful with those tables.

Finally someone who acknowledge to the insanity of M Threads ;) I swear those tables & figures differs between publications, to handbooks, to Int'l standards, tech doc, from public domains, its literally all over the place. Flat root profiles, rounded, min/max, rads... I've never seen anything quite like it, and probably the reason it is impossible to find a 'standard defined' 2D drawing anywhere - nobody knows how to define reliable and consistent M threads...

Conclusion; aim the CAM toolpath on the crest and root, or take a few pass with the manual lathe, see if the little nut fits, and call it a thread?!
 

Human

New member
Dear Human

Unless a non-standard tolerance is needed you don’t put any tolerance on paper, just note M 11 for example. Please hit the space key after the M.

There are no positive and negative tolerances. What you mean are deviations, in French écarts.

Deviations. I stand corrected. To my limited knowledge an unmarked M11x1.5 is a basic/nominal profile on drawing, or a 100% binding unusable thread mating reference rather.
Normally PMI as e.g. M11x1.50 4/6/8(e,f,g,h) for external and uppercase for internal M11x1.50 4/5/6/7/8(H,G).

Hence the importance of being able to 1) understand and draw a basic profile and 2) mathematically add tolerance matting to the base profile dimensions as per mechanical engineer's spec. And that's what I'm trying to achieve/understand, not trying to cut a thread.

Anyone can draw a 2D of a generic ISO965 M10X1.50 external & M10X1.50 internal base profiles and add 6g & 6H respectively w/ dim relations?
 

gregormarwick

Active member
Finally someone who acknowledge to the insanity of M Threads ;) I swear those tables & figures differs between publications, to handbooks, to Int'l standards, tech doc, from public domains, its literally all over the place. Flat root profiles, rounded, min/max, rads... I've never seen anything quite like it, and probably the reason it is impossible to find a 'standard defined' 2D drawing anywhere - nobody knows how to define reliable and consistent M threads...

Conclusion; aim the CAM toolpath on the crest and root, or take a few pass with the manual lathe, see if the little nut fits, and call it a thread?!

So get an actual copy of ISO 965 / DIN13 and take the data from the source. It is an extremely comprehensive standard and NOTHING is left to guess. You are muddying the waters by including ASME/ANSI in the mix, and taking data from random online sources of completely unknown derivation.

What you want to do is absolutely possible, but it's a bit like recreating the wheel IMO unless you have some purpose for actually accurately modelled threads? If you want it to put some sizes on your prints then I'd have to ask why? Are you having problems with unreliable vendors? Is it for internal manufacture and you don't want your own guys wasting time looking up standards? Accurate models for simulation?
 

Mechanola

Active member
You are not off the track but also not fully on. The metric threads evolved over quite some time in Europe where political (or chauvinistic) factors have played a role. Just note that the metrication came from France where rationalism was a royal matter. The people of the other countries didn’t like to undergo a French dictate.

Then German rationalism, which is a bit less stringent, said that only a selection of all possible sizes should be used, the others set back in tables numbered II, III, and so on. Even-number diameters were also given preference, M 2 through M 60. It was bad to call out M 7 or M 13. The M 1,5 was removed from all standards, who knows why.

I often have to do with set screws M 2,3. Although perfectly feasible and calculated after the basic formulae as you know them by now they are so strange in this country that I suspected an American origin. And so it is, the prototype of the device was designed in Chicago, the thread was 3/32". One of the Swiss engineers must have changed the specification from the 2,38125 mm that correspond to 3/32 in. In other places of the same device I find bores of 1,27 to 1,28 mm diameter, on obvious 0.05".

Again, the metric specification should read M 24. Period. Only non-regular threads are designated with addenda such as M 20 × 1. That’s a fine thread IV. The core diameter of the female thread is clearly defined by the standards and the nominal diameter of the male one as well. The triangle serves just as the calculation base.

You really shouldn’t overthink this. Get yourself the standards in force and learn to write metric measures with space and comma. Switch the computer off more often.
 

Human

New member
If you want it to put some sizes on your prints then I'd have to ask why?

The ultimate end goal for now is to understand how to 2D draw a M thread. 1) basic profile (done) 2) add standard defined deviations/tols via dimensions (automated expressions in my case) - work in progress. So to gain understanding and an accurate representation (in CAD) of the true geometry I am dealing with.

For instance; here goes a true representation of a ISO965 M10X1.50 6g and the mating M10.1.50 6H. How would I go about machining this non-sense with a so called full-profile ISO 60deg insert with a tip radius of 0.22mm, or should I say how much deeper I need to dive that insert in that material to have it fully machined, or ruined.

Your Q: Why? I need validation, dims, compute on screen, a reliable method, linear analysis geometry, something/anything to ref about...

M10-X1-50-ISO6g6-H.jpg
 

Human

New member
You really shouldn’t overthink this. Get yourself the standards in force and learn to write metric measures with space and comma. Switch the computer off more often.

Have a feeling those dev/tol standards we're established back when machine-tools were incapable to thread or keep up within tolerance lol
We're dealing with micron accuracy nowadays, so, what is the size of a M 11 the engineer wants, I'll pull it off within 30microns on any material.
Get my drift? Not amusing those eternal min/max eiEI confusions...

Thanks for that background info btw, quite fascinating :cheers:
 

EPAIII

Active member
At one time I also thought a lot about thread dimensions and tolerances. After looking at the drawings in Machinery's Handbook and the tables showing the dimensions and the allowable tolerances for the various classes of fit I found myself very confused.

It was only after I thought about how screws, bolts, and nuts are MASS PRODUCED that the above drawings and tables started to make sense. We, poor machinists have very little say in how these drawings and tables were drawn up. It is the manufacturers that make the threads by the hundreds of millions, by the billions who have the real input here. You need to think about how an exterior thread is ROLLED between two dies with the thread form on them. About how those dies will WEAR. About where they start when new, before that wear occurs. About how they are adjusted as they wear. You need to think about things like that. And how many threads can be produced before the dies must be adjusted. How many can be produced before the dies must be replaced.

Those are the considerations that are the primary reasons for the thread drawings and the tables and the tolerances.

When you see a dimension as a fraction of the pitch that is NOT a typical number. It is a maximum or a minimum number that represents the point where one of those dies is worn past the point of producing a thread that is in tolerance. Thus, your drawing shows a crest on the exterior thread as P/8 and the size of the valley in the interior thread as the same P/8 dimension. BUT those numbers almost never occur in the life cycle of a pair of dies or of a tap for making the nut. Those numbers are where the two threads, external and internal, will MEET lacking any clearance. Then clearance is added to one or both to allow them to not interfere. And that is still the end of life of the dies and taps. So even more is added or subtracted when making the dies and taps so that there is some room for them to wear while still guaranteeing that there will be the amount of clearance required by the class of fit being made.

And I only mentioned one pair of numbers. But the same applies to all of the numbers involved in making the threads. The wear on the dies and taps may be greatest at the tops of their teeth, but they will wear at other parts as well and different amounts of allowances must be made to ensure that all parts of the thread form will be in tolerance through out the life of the dies and taps.

A good example of how this actually works is if you notice the P/4 dimensions for the valleys between threads. If you examine any number of commercially available screws and nuts, you will find that you almost NEVER see any that approach that number. In fact, they ones that I have examined under magnification almost always have this dimension a lot closer to P/8. And I must conclude that P/8 is the real nominal number that these manufacturers always shoot for. And they retire their dies and taps long before they are producing anything remotely close to the P/4 number. YET, P/4 is the number that you always see. It is the absolute limit of permissible wear, not a nominal or average dimension.

When I reached this conclusion, this revaluation I finally understood the real purpose of the published drawings and tables. This is when I knew that it was completely useless to try to model threads in any CAD system with any exactitude.

If you need a 3D CAD model of a thread for 3D printing I will suggest two things. First, most 3D modeling programs will have threads built in. JUST USE THEM and make a test print. Adjust as needed. If you absolutely must do the modeling yourself, then do this:

1. Make the OD of an external thread a bit smaller than the nominal screw diameter. This is what the published tables show anyway.
2. Make the pitch diameter a bit small on external threads and a bit large on internal ones. Again, the published tables can help here.
3. Make the flat at the top and the fill in the valley P/8. Either can be either flat or a radius, but keep the final form INSIDE of that P/8 straight line.

Threads that are 3D printed with those rules will probably fit each other and also purchased fasteners. If you must have a percentage number for the smaller and larger numbers, use 2% or a minimum of 0.001" / 0.025mm.
 

Human

New member
Thanks, EPAIII. Absolutely fascinating read, ideas, opinions, knowledge, views, e v e r y t h i n g. Glad I've joined this experts community at last, although I doubt I'll be able to contribute an equivalent amount of knowledge. I'll do my best though...

Reading through your thoughts, I think you are right. Certainly makes sense about those endless accuracy hunting from a machinist/CAD designer perspective. Could I unknowingly be developing my very own in-house standard with this CAD idea then? Not far off to be honest, have the mating sketches, all what's left doing is automating dims vars(expressions) and converting this into reuse profiles for anything-M-thread.

Paid off already. Managed to get the correct dims to match that full profile ER-16 ISO R.22 insert. I probably would have scraped 5 parts before figuring out I've used the wrong min/max major/minors/pitch radi etc, so kinda glad I've taken this challenge.

Mthread.jpg
 

Conrad Hoffman

Active member
Nobody gets it, but I get it. I'm never content with tables and usually want the original derivations for spreadsheets and such. Now, you have to be careful, because many times they've tweaked the numbers and the formulas won't give exact (official) results. I don't remember if this is the case with metric threads or not. There are also rules about transgressing MMC you have to be aware of. I've studied this for years and am still fuzzy on some aspects. Anyway, I have a spreadsheet you might be able to pull some formulas out of. PM me and I'll send a copy. BTW, you can't imagine how complicated threads really are until you read Vogel.
 

Human

New member
Nobody gets it, but I get it.

Hi Conrad, yeah, that would be me only 72hrs ago.

The lazy-cut-corner attitude toward the science of threads change dramatically when your parts comes back from the anodizer and the beautiful precision doesn't works anymore, locks half-way, or you need to have your delrin parts placed in the freezer overnight to be able to assemble a prototype before next morning (thermal expansion coefficients missed-out). Both occurrence fairly complex parts. And so, enough, need a fail-proof method that works.

Too kind on offering years of experience, Conrad. Only a fool would refuse this level of generosity and so I'll take the offer. Let me know if I can do anything to compensate your efforts in any way. I'll update on progress made and achievements based on your work using this discussion-thread.

PM sent.
 








 
Top