Results 1 to 20 of 35

04092013, 06:38 PM #1
Internal UN thread engagement percentage confusion
According to MH that i have in possession thread % for Unified threads should be calculated as follows:
Hole_Size=Basic Major Diameter(1.08253 × Per_Cent_Full_Thread)/Number of Threads per Inch
But many other sources give 1.299 number instead of 1.08253.
Also hole sizes calculated using above formula look a lot bigger than they should be.
IE: a 1/420 UNC tap hole with 75% thread engagement comes out 0.209" instead of 0.201" like in any other tap drill chart....
Indecently MH also gives Hole_Size=Basic Major Diameter(1.08253 × Per_Cent_Full_Thread) x pitch for metric taps as well.
Is my copy of MH27 faulty or everybody else is wrong?
here is a page out of that Machinery's Handbook 27


04092013, 08:14 PM #2The constant 1.08253 in the above equation represents 5H/8 where H is the height of a sharp Vthread.
Last edited by sfriedberg; 04092013 at 08:20 PM. Reason: Completely rewritten

04092013, 08:58 PM #3
That is the question i am asking.
Regardless of other sources
All of the tap charts give #7 drill for 1/420 UNC tap at 75% thread engagement.
But if you calculate hole size using MH formula you get 0.209"!
At the same time the chart in attachment above shows hole size to be 0.201 !!!!
I am totally lost.
1.299 constant is not even in MH

04092013, 11:59 PM #4
Scratching my head here, I think the MH formula should be not be saying "basic major diameter", but rather "major diameter of thread form" which is smaller than the basic major diameter. I took a look in Moltrecht, and he gives the 1.08523 formula for American Unified thread form and the 1.29904 formula for American National thread form, but I can't put my hands on any reference that suggests these thread forms differed substantially and think both of them are wrong.
The 1.29904 constant is 1.5*sin(60), while the 1.08523 constant is 1.25*sin(60).
I'm going to ignore allowances and tolerances and just talk about geometry.
UN and metric threads are truncated by H/8 at the major and H/4 at the minor diameters of the nominal sharp Vthread. So a 100% engagement involves 5/8 H of actual thread height. Because you have engagement on opposite sides of the thread cylinder, total 100% engagement is twice that, or 5/4 H or 1.25 H. A tiny bit of trig tells you that H is sin(60)/TPI for 60 degree thread forms. So 100% engagement is 1.08523/TPI on diameter.
So if MH has the "right" constant, why don't the tap drill sizes come out correctly? Well, the answer is that the 100% engagment doesn't begin at the basic major diameter, but at a lesser diameter. Namely, at the H/8 truncation of the nominal sharp Vthread at its major diameter. Because you have that truncation on opposite sides of the thread, that lesser diameter is BasicMajor  H/4, or BasicMajor  0.21651/TPI. The hole size would be BasicMajor  0.2165/TPI  1.08523*percentage/TPI.
When I plug in 20TPI and 75%, I get .1986 which errs in the opposite direction and is bit under a #8 drill.
Also, 1/4 sin(60) [thread major diameter correction] + 5/4 sin(60) [thread engagement correction] is 3/2 sin (60) or 1.5 sin(60). So that's how the MH formula and the other sources are related. However, I think it's an error to add the two constants that way. The percentage engagement should only apply to the 1.08523. The 0.21651 is not affected by engagement. So I think both formulas are incorrect.
Hole diameter = basic major diameter  1.08523 * percentage / TPI
Hole diameter = basic major diameter  1.29904 * percentage / TPI
So, every tap chart in existence is wrong.

04102013, 01:08 PM #5
So nobody?
Where is that Danish thread ninja when his expertise is needed?
I guess I will just use 1.299 constant as it seems like everybody else is doing the same.
And MH? Screw the MH!


04102013, 04:55 PM #6
When in doubt don't ask, draw it out!
Was told this on asking a similar sort of question when I was, maybe, 20. Good advice as I was able to figure out that the two conflicting sources were talking about different things, coming from different places and both ending up in the kitty litter. CAD makes the drawing bit much easier so no excuses.
Never assume the charts, tables or statements from higher authority are correct. Major errors can go uncorrected for years. There is just so much stuff there. Proof reading is hard enough and reverification from first principles just doesn't happen. If it looks odd it probably is odd. But there may be a reason for the oddness.
Clive

04112013, 05:46 AM #7
Hello Eldar,
I got a bit curious, so I did a bit of sniffing around and saw a site that listed formulae for tap drill sizes, and it shows using 1.08523 for UN and using 1.29904 for American National. I looked in both Van Keurens Handbook and a Seventh Edition american Machinists Handbook, which both refer to American National, and the tap drill sizes published in both agree with the 1.29904 constant to within a tenth or two.
In looking at the page from MH that you posted, the chart at the top states American National, but the formula below states Unified. Perhaps that is why the hole size differs from the chart when using the formula. (1/8P vs 1/4P root difference on the male thread)

04112013, 08:52 AM #8
In my 24th MH for this table 4 it states that the 1.08253 is for American Unified thread form and the 1.29904 is for American National thread form. A cut & paste: "The American National Standard Series (NSeries) was last defined in ANSI/ASME B1.1:1935 and has been obsolete since 1949. In ANSI/ASME B1.1:1949 when the American National Standard Series (NSeries) was made obsolete the NSeries screw thread data was moved to the Nonmandatory Appendix. When the standard was revised again as: ANSI/ASME B1.1:1960 the American National Standard Series was intended to be forgotten and was removed completely from the standard. ANSI/ASME B1.1 has since been revised in 1974; 1982, 1989 and 2003."

04112013, 01:06 PM #9
So we all are tapping holes using a standard that became obsolete in 1949??

James H Clark liked this post


05302013, 03:06 AM #10
Slightly stale thread, but I want to follow up and correct something I wrote earlier.
It was surprisingly difficult to find a trustworthy source for the details of the US Standard (aka Sellers) thread form of the late 1860's to late 1940's. But as Glen Wegman stated, the Sellers thread form was truncated H/8 at both major and minor diameters. The Unified thread form (1949 and onward) is truncated H/8 at the major and H/4 at the minor diameter. So the Unified thread form requires a larger tap drill diameter than the Sellers, and yes, virtually every published tap drill chart for inchbased threads is almost 60 years out of date.
So if MH has the "right" constant, why don't the tap drill sizes come out correctly? Well, the answer is that the 100% engagment doesn't begin at the basic major diameter, but at a lesser diameter.
Therefore the tap drill diameter for UN threads is
BasicMajor  1.08523*percentage/TPI
BasicMajor  1.29904*percentage/TPI
ISO M threads have the same form as UN threads. Obviously they don't use TPI, but the same factor applies.
Clive603 was spot on:
Proof reading is hard enough and reverification from first principles just doesn't happen.

05302013, 07:01 PM #11
To fill in a bit more:
The Single Depth (what sfriedberg refers to as "H") of a 60 degree Sharp V threadform  which has been obsolete since the mid 1800s, but has goodplacetostart geometry  is Cosine 30 degree x Flank Length. Since the Flank Length of a 60 degree Sharp V threadform is exactly equal to the Pitch, Cosine 30 degree x Flank Length can be restated as Cosine 30 degree x Pitch.
The Sellers / Franklin Institute / U S Standard / American National threadform, having a 60 degree FlanktoFlank angle like the 60 degree Sharp V threadform, AND 1/8 x Pitch flats at both the Major and Minor Diameters, has the same Single Depth as the 60 degree Sharp V when expressed as a function of Flank Length, Single Depth = Cosine 30 degree x Flank Length. But the flats reduce the Flank Length from 1 x Pitch to (1  1/8  1/8) x Pitch = 3/4 x Pitch. Expressed as a function of Pitch, the Single Depth of a Sellers threadform is Cosine 30 degree x 3/4 x Pitch.
The Unified (and ISO Metric) threadforms, in their most basic form, have 60 degree FlanktoFlank angles, a 1/4 x Pitch flat at the Minor Diameter, and a 1/8 x Pitch flat at the Major Diameter. The Single Depth as a function of Flank Length remains Cosine 30 degree x Flank Length, and, just as with the Sellers threadform, the flats shorten the Flank Length as a function of the Pitch. So for both the Unified and ISO Metric threadforms, the Single Depth = (1  1/4  1/8) x Pitch = 5/8 x Pitch, and the Single Depth expressed as a function of Pitch = Cosine 30 degree x 5/8 x Pitch.
Of course, the Single Depth of the screwthread is only one half of the difference between the Major Diameter and Minor Diameter. As you might suspect, we often call the difference between the Major Diameter and Minor Diameter the Double Depth of the screwthread. As you might also suspect, the Double Depth of a screwthread is simply twice its Single Depth, and the calculations as a function of Pitch are these:
For the Sellers threadform, the Double Depth = 2 x Cosine 30 degree x 3/4 x Pitch = 1.299038+ x Pitch
For the Unified and ISO Metric threadforms, the Double Depth = 2 x Cosine 30 degree x 5/8 x Pitch = 1.082531+ x Pitch.
And that's where the textbook "magic numbers" come from. Why the textbooks present these values as constants, without explaining their derivations, mystifies me.
John

Jared liked this post

05312013, 12:38 AM #12
The second thread formula on this link might help
http://www.fms.dk/1.09.pdf
Gordon
I would suggest that anyone working regularly with "American" threads buy ASME B1.1. I'm assuming that info in MHs is taken from standard sources.

4GSR liked this post

05312013, 03:24 PM #13
Gordon 
Now I'm curious. I don't recall ever seeing a standard or specification for the Unified threadform with radii at both the Major and Minor Diameters, whether internal or external.
The basic Unified threadform has flats (which, despite the name "flat", are really supposed to be helical sectors of cylinders) at both the Major and Minor Diameters, and there are two wellknown variant forms of the Unified that require a radius in place of the Minor Diameter flat of the external (only) thread. The Unified R variant has a standard Minor Diameter, and a 0.14434 x Pitch radius in lieu of the 1/4 x Pitch flat; the Unified J variant has an enlarged Minor Diameter, with a 0.15011 to 0.18042 x Pitch radius that, has  at its points of tangency to the thread flanks  a chordal length of 5/16 x Pitch.
The Unified R external thread readily engages a standard (flatted at both Major and Minor Diameters) Unified internal thread, meaning that there is no need for a Unified R internal thread specification. On the other hand, the Unified J male thread doesn't necessarily engage a standard Unified internal thread, and there is a specification for a Unified J internal thread. The Unified J internal thread has a 1/8 x Pitch flat at its Major Diameter paired with a 5/16 x Pitch flat at its Minor Diameter.
There is an interesting subtlety associated with the Unified J threadform. The Single Depth of the screwthread is different for the external and internal threads. The external thread's Minor Diameter radius obviously needs to clear the internal thread's flat, so the external thread is "deeper" or "taller" than the internal thread. Quantitatively, the basic Single Depth of the external Unified J threadform is Cosine 30 degree x 2/3 x Pitch , and the basic Single Depth of the external Unified J threadform is Cosine 30 degree x 9/16 x Pitch.
This leads to an interesting bit of trivia that comes into play when needing to cuttap an internal screwthread of the Sellers, Unified, and Unified J threadforms. Assuming that the Major Diameter and Pitch match, the SAME Sellers (aka U S Standard or American National) tap is used  and explains why most "inchsizes" taps in the US are still marked NC or NF rather than UNC or UNF.
If the internal thread is to be a Sellers threadform, the absolute minimum diameter of the hole to be tapped is Major Diameter  2 x Cosine 30 degree x 3/4 x Pitch.
If the internal thread is to be a standard Unified threadform, the absolute minimum diameter of the hole to be tapped is Major Diameter  2 x Cosine 30 Degree x 5/8 x Pitch.
If the internal thread is to be a Unified J threadform, the absolute minimum diameter of the hole to be tapped is Major Diameter  2 x Cosine 30 Degree x 9/16 x Pitch.
By "absolute minimum diameter" in the above paragraphs, I mean "one hundred percent depth of thread, any smaller and the screw probably won't fit, provided you don't plug the hole with a broken tap first"; here in Practical Land the holes need to be a bit larger. And that leads to another interesting bit of trivia: The old US NBS Standard H28 set the maximum permissible depthofthread of internal threads for US Government service at 83 percent, and the basic Single Depth of a Unified threadform of a given Pitch is 83 percent of the Single Depth of a Sellers threadform of the same Pitch. In practice, that means a maximumpermissible Sellers internal thread will, if just barely, accept a maximumpermissible Unified external thread of the same Major Diameter and Pitch.
John

06012013, 07:12 AM #14
.
you make things too complicated
1/420 thread
1000/20= 50 thats 0.050 from 0.250 so 0.200 tap drill, adjust slightly depending on material and depth
.
drill bits drill over size. how much depends on a lot of things. i have seen a CNC put a 1.500" drill through and hole 0.050" oversize. sure properly sharpened and use a pilot drill hole will be much closer. point is 99.99% of the time the tap drilled hole is oversize. use a reamer if you are worried about it.

06012013, 08:54 AM #15
John, too much detail I'll keep my reply as simple as I can.
First flat contra radius: http://www.fms.dk/1.05.pdf
A radius gives a stronger thread and avoids possible sharp corner shearing.
The American UN thread form (named ISO Inch by ISO) has the identical theoretical profile as the metric thread. The difference is in the radii.
A MJ thread has a larger root radius than standard and is often used with high stress bolts to again, minimize shearing.
There will be flats on the top of external threads depending on the turned diameter just as there will often be flats on the internal thread depending on the diameter bored. There should ALWAY be radii on the root of external threads (d1) and on the "OD" of internal threads (D).
Gordon
I hope I don't give too many a heart attack in here but i always prefer what is in standards as opposed to Machinist Handbooks. The people that write Machinist Handbooks take what they feel is important from standards and at other times just give "advice". I'm no better than most in that I tend to keep something like a MH even if some of the information gets outdated.
I've never understood that less than a full thread profile seems to be acceptable to some. Many NoGo thread plug gauges here are made so that they also check for a too large bore diameter.

06012013, 02:29 PM #16
Hello Gordon,
In your drawing, you appear to be showing a .10825P radius on the crest of a UN thread. That is what is being questioned.

06022013, 12:42 AM #17
If a thread is cut with a full form insert removing all the material then it will have a radius. The radius shown is the correct radius for that particular thread pitch. A single point threading tool will result in a flat. Of the two then a radius looks and feels better.
Even threads like ACME and Tr have tiny radii as sharp edges should be avoided when possible.
I don't know if I can explain it better.
Gordon

06022013, 12:27 PM #18
The radius is an allowable option, but not the standard.
Your drawing appears to present it as the standard for UN.
You do not show the Metric thread form with the same radius crests!

06022013, 10:55 PM #19
Doh, the thread got resurrected and I missed all of the action!
So. If I make software that shows thread % for a number of drills and I use a standard that's been obsolete for the last 60 years nobody will really care that its wrong?
Just because everybody else is doing the same thing?

06032013, 05:41 AM #20
H28 states:
“Percent of threads listed in tables is the ratio in percent of the actual height of the thread to the value of 0.75H; this value is the basic thread height of the obsolete American National Thread Profile. Since the basic height of the Unified Thread Profile is 0.65H, the maximum percent thread permissible is 83.3%. Due to allowances for drills to cut oversize or due to lack of availability of drills within specified minor diameter limits, tap drills listed in tables II.A.1 and II.A.2 may show greater than 83.3% threads. This indicates that the drill size is smaller than the minimum thread minor diameter and additional machining of the hole may be necessary in order to permit economical tapping.”
The charts do go on to list a number of drill sizes for each thread size and list the theoretical percent thread for each drill size along with the possible hole size error for the drill.
Sounds to me like if you need a specific thread height percent, you need to be doing some calculations rather than just relying on the published tap drill charts! The charts will obviously work for general purpose though.
Bookmarks