Calculated Thread Depths for Metric fine threads

[Paul Alciatore]

Where do you get the P/4 and P/2 widths for the flats? At P/2, the flat would be at the pitch diameter. And at P/4 it would be half way there from the other end. You would be left with only 1/4 of the full thread. The basic metric thread form calls for 5/8 of the full thread form.

My Machinery Handbook shows the width of the flat at the crest of an external thread is P/8 and P/4 at the root. And these are nominal values. Some variation is allowed. An internal thread could have a smaller flat at the major diameter and a larger one on the minor diameter to allow clearance for the fit.

I have seen many metric threads and I doubt that ANY of them had that full P/4 flat in the roots. All of them were probably a lot closer to P/8 or even P/10. Perhaps things are different in some other countries, I don't know. But, for real world metric threads in the US, that P/4 has got to be considered more of a maximum size instead of a nominal one as the drawing in the spec would imply. This is further shown with an additional drawing that shows a minimum radius (not flat but radius) at the root of 0.125P (1/8P). That is a radius of an arc that is tangent to the two flanks and the bottom of that arc would be below even a 1/8P flat. I would think of that P/4 flat as the absolute limit of wear on the tool that is producing the thread and most factories apparently do replace that tool a long time before that limit is reached.

The Major Diameter - Pitch formula I used earlier provides a bore or minor diameter for the internal threads that is one Pitch smaller than the major diameter. If you calculate the diameter of the P/4 root flat of an external thread, it is 1.083 Pitches less than the major diameter. This is 0.0083 Pitches smaller than the rule of thumb formula provides. This is a small amount for most threads and a tap drill will probably drill a bit over-sized anyway so the actual hole will be closer to the theoretical position of the P/4 flat of the external thread that will be inserted into the tapped hole. Add that to the fact that few, if any at all, actual external threads have a full P/4 flat at the root and you will see that the rule of thumb works for providing root clearance for practically all real world threads.

My point is that you can not count on the exact P/8 or P/4 flats being exact values. They are nominal or maximum values. So when you cut an internal thread, you must take all possibilities into account. This is why they make thread gauges. A shop made gauge would be a good idea for situations like this.

All of these fine points of the thread form are why I said it is not as simple as just touch off and cut to a specified depth; without knowing ALL the dimensions involved, including those of the cutting tool you are using.

The width of the flats of the internal and external threads is precisely described. For an external thread the flat for the minor diameter is P/4 and the flat for the major diameter is P/2. This is inverted for internal threads. Everything is derived from the pitch. Note too the asymmetry in the flat widths. This is because the thread is not cut symmetric about the pitch diameter. This defines the form of the cutters needed to cut internal and external threads. A sharp vee cutter is not used nor defined in the standard. That hasn't stopped anyone from doing so.

The height of the thread is defined as the distance between the points when the thread is drawn and the specification requires H = cos(30) * P and is yet another dimension derived from pitch. The points are imaginary and are located outside the actual thread. The thread depth is precisely described in the standards and is Dmaj - Dmin. Dmaj is given in the designation of the part eg, M8x1.25 defines Dmaj as 8mm. Dmin = Dmaj - 2 * 5/8 * H = depth of thread.

So we have the major diameter and the pitch as starting points. We quickly calculate H and Dmin and we're ready to cut. Except the thread cutting tool is a form tool and we have to address that. There's one more problem to solve and that is the clearance at the thread root. Some clearance is required outside the dimensions of the thread. This clearance area is not part of the thread itself. From reading above we see that for an external thread the thread width at Dmin is P/4. Using a sample M8x1.25 thread the minor diameter flat will be 1.25/4 == 0.313mm. So we grind our perfect 60؛ cutter to a fine point then grind the tip off until it is 0.313mm in width. Except that leaves nothing for the clearance. So we use our optical comparator to locate the P/4 line on the cutter tip and grind a slight radius that fits the P/4 line.

Nothing left but to cut the thread.

Edit: Forgot to add this - including the clearance, the depth of cut will be 0.614 * P which means you can ignore everything else in this thread if you use threading inserts.

[dp]

http://upload.wikimedia.org/wikipedi...Dimensions.svg

Fat fingered P/2 - should be P/8. P/2 is the tooth width at the pitch diameter.

[madman]

DOH typo error thread was 12 mm x 1.25 (NOT .125) would the dimensions change for this change? Thanx and I apologize) Mike

[dp]

The formulae that use constants and pitch (Metric thread depth is 0.614 x pitch, cos(30) * P, etc.) won't be affected but you do have to recalculate with the correct pitch. And don't forget the results will be in what ever units you use for pitch so if your dials are not in those units the additional conversion to your dial units is needed.

[Paul Alciatore]

In a word, YES, they would change.

Time is short now. I will attempt to run through it again later.

Are you sure this time?

DOH typo error thread was 12 mm x 1.25 (NOT .125) would the dimensions change for this change? Thanx and I apologize) Mike

[Forrest Addy]

Sorry, I haven't read most of the previous posts, but what I have to say here is pure gold: if you have to bore an accurate internal thread, first acquire/make an accurate gage.

Internal threads can't be directly measured. They have to be gaged; preferably with calibrated Go and No-Go gages. However a home brew Go gage wll serve for most practical purposes. Make it right and check its pitch diameter over wires. If official wires are not handy (what machinist's tool box doesn't have a set of Pee Dee thread wires in the center right small drawer in their Gerstner chest) use the nearest size drill shanks (drills are tapered; mike 'em where they contact the thread) and do the math to solve for M.

Once you have a practical gage, boring a good internal thread is easy.

Cutting good threads from pure calculation is like shooting crows in a coal mine; success will be accidental. You need either measurement or gaging to make your fits and tolerances

[Carld]

removed post

[Carld]

I agree with Forrest, you will have to make a male thread to the diameter and pitch you want and use it for a test part to make the internal thread. I have never found a measuring tool to measure an internal thread. Making an internal thread without a mating male test part is like taking a shot in the dark with a blindfold on and expecting to hit a target.

To make the male thread you will have to use measuring wires or measuring triangles for it to be accurate.

[elf]

How hard would it be to make or find some thread wires the correct size? https://www.youtube.com/watch?v=QGBRwXwxnuU

[oldtiffie]

First of all the"3-wires" can be any diameter so long as they are all quite accurately the same diameter and all will engage the thread on its "flat faces".

The diameter sought does not need to be the Pitch diameter but within the pitch diameters at the limits of the sizes as specified in Machinery's Hand Book.

Here are the workings for a 1/2"- 13 - UNC - 2A male thread.

http://i200.photobucket.com/albums/a...wirecomps1.jpg

Here are the 3-wire sets:

http://i200.photobucket.com/albums/a...ds/3-wire2.jpg

http://i200.photobucket.com/albums/a...ds/3-wire3.jpg

And here are the thread details and limits:

http://i200.photobucket.com/albums/a...n_P72-73_1.jpg

[oldtiffie]

There are tolerance limits on: OD of a bolt (male); the pitch cylinder required as well as the point radius on the threading/screwing tool.

So in that lot there is no one set "in" feed on the screwing tool that will give everyone /anyone the pitch cylinder diameter.

Check Machinery's Hand Book.

The maths required for using the "3-wire" method will stop some people cold if they do not have the maths for it.

The logical answer is to use a good thread micrometer where the pitch cylinder diameters can be read off directly without any maths and without the frustration of keeping control of the three wires - and Using machinery's hand Book for the sizes required.

https://www.google.com.au/search?q=t...2&ved=0CCUQsAQ

https://www.google.com.au/?gws_rd=ss...ead+micrometer

[oldtiffie]

Mathematically it s quite feasible to measure thread pitch diameters with "wires" three wasy:

using three wires;

using two wires; and

using one wire.

I will cover it at my leisure at some time in the future.

It should be said in this context that the "3-wires" are only used on ISO and UNC/UNF ("Vee") threads that have a helix angle not exceeding 5 degrees.

(Check Machinery's Hand Book).

[PixMan]

The OP is a classic example of why we all want to see your location in your profile. You need to make a simple, standard, relatively small internal thread. I have several styles of M8 taps and would loan one to you if I knew you were close to me.

But I have no f'n idea.

BTW, an M8x1.25 is not a fine thread, it's the standard pitch (coarse.)

[Paul Alciatore]

OK, the calculation again, with the correct thread pitch.

Based on M12 x 1.25 and Sharp Vee tool:

Bore Size = Diameter - Pitch.

12mm - 1.25mm = 10.75mm

That's an easier drill to find. If you have access to inch size drills, that translates to 0.423". That's almost exactly 27/64" (27/64" = 0.422"). Again, you can go with a smaller hole than this. Anything between 10.6 and 10.8 mm will probably be OK. I don't know what drills are available where you are so I will go with 10.75mm or the 27/64". Since it is important to start at a known ID, I would suggest drilling a bit smaller and boring it out to exactly 10.75mm.

With a 10.75mm bore, you will need to move your SHARP VEE tool out far enough IN A RADIAL DIRECTION to bring the flat of the thread (which does not exist on that sharp vee tool) to the 12mm nominal OD size of the thread. Thus the tip of that sharp vee tool will be at a greater diameter than 12 mm. The metric standard thread has a 1/8 h flat on the tip of the threads where h is the height of a sharp vee thread. (same paragraph as before)

Height of a sharp, 1.25mm pitch thread, h = 1.25mm x cosine(30) = 1.083mm.

And 1/8 of that is 0.135mm.

So we are going to need to move the tip of our sharp vee tool out to a diameter of

12mm + (2 x 0.135mm) = 12.271mm

We are starting (touching off) at 10.75mm and going to 12.271mm

12.271mm - 10.75mm = 1.521mm

But that is on the diameter and we are moving on the radius so we need only half that amount:

1.521mm / 2 = 0.761mm (0.030")

You can use that if you are moving out using the cross slide.

If you are using the compound set to 29.5 degrees then that amount would be increased to

0.761mm / cos(30) = 0.879mm or 0.034".

That would be a theoretical thread size. Since you have no way of testing it, I would recommend that you cut just a bit further to ensure a fit. Perhaps another 0.025 or 0.050mm or one or two thousandths more.

Again,I would greatly appreciate it if someone else here would check my math on this.

Also, as I and others have stated above, it would be best to have a gauge to check these internal threads. Even a shop made gauge is of great value here. Cut the gauge a thousandth or two larger than the maximum size allow for a male thread, then cut the internal thread using that gauge for proper fit.

[boslab]

Sewing needles make good thread wires for small sizes, they are quite accurate too
Mark