How to specify a Unified screwthread in an otherwise-metric documument?

John Garner · Jul 19, 2017

Good Afternoon, All --

Is there a generally-preferred way to specify a Unified screwthread in an otherwise-metric document?

Going way back three decades or so, I received two documents – one French, the other Swiss – that called-out a 5/8-11 UN thread as “MS 15.88 x 2.31” . . . which was oddball enough that it’s clear in my memory still. More recently, I have seen “.2500 - 28 UNJF” on a metric drawing I've been asked to review, and although I think that citation better than the pseudo-MS citation, its reliance on the “UN” to communicate the unit transition to inches doesn’t seem adequate.

My own inclination would be to say something along the lines of “1/4 inch x 28 thread per inch, J-form Unified screwthread”.

If there is a generally-preferred way of making such a citation, I’d like to know what it is; if there isn’t, I’d like to know your thoughts on the question.

Thanks,

John

litlerob1 · Jul 19, 2017

I think what is easiest to interpret, without room for argument. I think what you recommend would do just fine for me personally.

R

Forrest Addy · Jul 19, 2017

This little problem is easily solved with a little research.

The official call-out for 60 degree Unified screw threads is: nominal size (inches) - threads per inch (space) UN (denotes Unified) (no space) class of fit (generally 2a - external threads, or 2b for internal threads. There is also a Class 4 (obsolete) and a Class 5 (for interference thread studs in tapped holes.)

Generally speaking Class 1 is a looser class for freely assembled utility grade threaded fasteners and Class 3 for application requiring high confidence, precision fit, etc..the Metric world has their equivalents.

The correct call-out for your first example is: 5/8 - 11 UN 2b.

ASME b1.1 (2003) specifies the form of Imperial screw thread call-outs and I14.5 specifies when and where to employ them.

The transition from the Metric world the the Imperial isn't difficult but those used to working in one but unfamiliar with the other are bound to include little slip-ups in their work. These are easily resolved with a little research and maybe a phone call or email.

All things are possible with people of good will.

guest · Jul 19, 2017

Call out the thread you want. If you want a 1/4-28 UNF 2B, call it that.

Other than the depth of threads, I don't want or need any more information than that. And you don't have to tell me what size drill to use either.

I hate it when people call out UN threads in metric. Like the country bumpkin who saw his first giraffe in the zoo- "There ain't no sich animal"

John Garner · Jul 19, 2017

Forrest and jancolic --

This particular citation -- on someone else's drawing -- is intended to specify a commercially-procured nutplate, so the depth of thread is wholly moot and its class is substantially moot.

And, jancolic, because you specifically mention your distaste for drill-size callouts on drawings, I'm going to ask you a serious question: Do you think specifying drill size is unnecessary when drilling and tapping a J-form thread -- either UNJ or MJ, doesn't matter -- is required?

FWIW, I think specifying drill size (or even better, Maximum and Minimum Minor Diameter limits) is worthwhile when calling-out a J-form thread.

John

alextnnr · Jul 19, 2017

Just please don't tap English threads in a standard metric bolt hole pattern... I have used equipment that had iron castings with standard metric bolt patterns that had been bored and tapped with a larger English sizes which meant it was incompatible with all off the shelf tooling.

guest · Jul 19, 2017

John Garner said:
...And, jancolic, because you specifically mention your distaste for drill-size callouts on drawings, I'm going to ask you a serious question: Do you think specifying drill size is unnecessary when drilling and tapping a J-form thread -- either UNJ or MJ, doesn't matter -- is required?

FWIW, I think specifying drill size (or even better, Maximum and Minimum Minor Diameter limits) is worthwhile when calling-out a J-form thread.

John

Yes, specifying drill size or major/minor diameters is not necessary. If you want a J thread form, call out a 1/4-28 UNJF 3B and I will make the hole. I will make sure the minor dia. is correct, and I will gage it with the correct gage. That's my job.

The more you call out, the more time I have to spend checking you- and the greater potential for dispute. I can read a thread chart, and a thread is either in spec or it isn't. Putting a bunch of extraneous information on the drawing is just a pet peeve of mine.

Also, when you say .2500-28 UNJF that also annoys me. That's a 4 decimal callout for a fractional dimension. If you have an aversion to fractions, use .25.

The drawing should tell me everything I need to know to make the part, and nothing else. 1/4-28 UNJF 3B is a perfect description of that hole.

It's not that I'm a dick- though maybe I am. The drawing is there to tell me what you want. Making the part is my responsibility. When you start telling me how to make the part, you share the responsibility of making it right, and I don't think you should want that.

There are times when controlled operations are appropriate- specific coolants on exotics, roughing allowances for heat treat, etc., In those cases I follow the planning to the letter. If the part comes out bad (say it warps out of spec in heat treat), it's not my fault if I followed the planning and documented it- YOU were the one who determined .100 was enough roughing allowance...

robert123 · Jul 19, 2017

How do you know it is a metric drawing? Does the drawing say "All dimensions in mm unless otherwise specified" or something else? Do whatever will make the drawing not contradict itself. I think I might use 1/4"-28 UNJF 3A to clarify that it is in inches instead of millimeters. Even better is to provide the spec for the thread so there can be no confusion: 1/4"-28 UNJF 3A per ASME B1.1.

robert123 · Jul 19, 2017

guest said:
Yes, specifying drill size or major/minor diameters is not necessary. If you want a J thread form, call out a 1/4-28 UNJF 3B and I will make the hole. I will make sure the minor dia. is correct, and I will gage it with the correct gage. That's my job.

The more you call out, the more time I have to spend checking you- and the greater potential for dispute. I can read a thread chart, and a thread is either in spec or it isn't. Putting a bunch of extraneous information on the drawing is just a pet peeve of mine.

Also, when you say .2500-28 UNJF that also annoys me. That's a 4 decimal callout for a fractional dimension. If you have an aversion to fractions, use .25.

The drawing should tell me everything I need to know to make the part, and nothing else. 1/4-28 UNJF 3B is a perfect description of that hole.

It's not that I'm a dick- though maybe I am. The drawing is there to tell me what you want. Making the part is my responsibility. When you start telling me how to make the part, you share the responsibility of making it right, and I don't think you should want that.

There are times when controlled operations are appropriate- specific coolants on exotics, roughing allowances for heat treat, etc., In those cases I follow the planning to the letter. If the part comes out bad (say it warps out of spec in heat treat), it's not my fault if I followed the planning and documented it- YOU were the one who determined .100 was enough roughing allowance...

I agree it is unnecessary to provide duplicate information. If you want to make it easier so I don't have to look up the thread details (though I probably will anyway), include the info but mark the dimensions as reference. Of course, if you are modifying the thread to be non-standard, then do include the dimensions that vary from spec.

6PTsocket · Jul 20, 2017

guest said:
Call out the thread you want. If you want a 1/4-28 UNF 2B, call it that.

Other than the depth of threads, I don't want or need any more information than that. And you don't have to tell me what size drill to use either.

I hate it when people call out UN threads in metric. Like the country bumpkin who saw his first giraffe in the zoo- "There ain't no sich animal"

I agree. I had to adapt to metric and have no problem with M4-.7 and would look at it with confusion if it were converted to unified thread. I see they translate ratchet drive sizes to metric. It seems that after years of complaining about the metric system, we have become the more flexible, working between the two. I have come to appreciate the metric system and we should have switched a long time ago but it is slowly taking over everywhere, from plywood to soda bottles.

Sent from my SM-G900V using Tapatalk

Punkinhead · Jul 20, 2017

guest said:
And you don't have to tell me what size drill to use either.

We may not need to tell you, but there are a lot of machinists out there that apparently need to be told. Wish it weren't so, but that's reality. In fact, there was a thread here awhile back on this very topic and one of the board members was arguing that he didn't need to be told the tap drill size for metric threads because he had a complicated formula involving multiplication that would give him a close enough number. After being burned a few times by guys like him, I put the tap drill size on the drawing.

michiganbuck · Jul 20, 2017

Ot Jancollic: [I hate it when people call out UN threads in metric.]
like calling a metric in inch.. just more chance to calculate an error ..

Bobw · Jul 20, 2017

Punkinhead said:
We may not need to tell you, but there are a lot of machinists out there that apparently need to be told. Wish it weren't so, but that's reality. In fact, there was a thread here awhile back on this very topic and one of the board members was arguing that he didn't need to be told the tap drill size for metric threads because he had a complicated formula involving multiplication that would give him a close enough number. After being burned a few times by guys like him, I put the tap drill size on the drawing.

Functional and "in-spec" are 2 TOTALLY different things when it comes to threads..

I much prefer it when the hole size is provided on the drawing.. Then I don't have to look it up..

Especially when its an oddball type thread... Helicoil (STI) threads, give me the hole size,
I don't want to look it up..... J threads same thing...

Another thing with the oddball threads.. I've seen where if the machinist doesn't know
what all the letters are after a thread call out, they just ignore it.

1/4-28 UNJ... I don't know what the "J" stands for, must have been a typo, but I DO know
what a 1/4-28 is, so I'll just go with that.. If the hole size is on the print, even
the most dense machinist that has no clue what the J means will make the thread properly.

10-32 STI. What the hell does STI mean? I don't know, but I know what a 10-32 is, so
we'll just go with that.. If you call out the hole size (which I believe is .201 ±.003)
they'll realize they have a problem and need a new tap when the 10-32 tap falls through
the hole.

And calling out an imperial thread in MM's is just retarded... How do you reference
that back to a spec? Calling it an MS (assuming Metric Special) doesn't seem to
be a very intelligent thing to do when its a STANDARD thread..

tnmgcarbide · Jul 20, 2017

i think it is imperative to indicate the rogue dimensions in the title block . i was a draftsman long before i
became a machinist , so maybe i am critical of engineers' poorly executed prints . CAD is great , but also
leads to laziness .......especially when it comes to title block tolerances +/- ( .x , .xx , .xxx , 1/x ) , and
bilateral tolerances that are left to apply to things that must fit together ( 1" shaft,1" sleeve, +/-.005)with a .001 press fit ............

anyway, it's not the end of the world ...just make notes of the specific inch or SI thread limits and how much thread
is needed( 50, 75 , whatever % ) but again , nobody wants to drill / bore/ ream a tapdrill hole to .0001 , just
because autocad was set to .xxxx for the drawing.

anyway PUT IT iN THE TITLE BLOCK NOTES FIRST>

be nice to your machinist.

about inch/metric conversion......... let the machinist figure it out .

if the threads are spec'd in a different form.... and i have to helically-threadmill it ,G76 it , or G84 rigid tap, in order to keep things constant and not write a different fucking program,YES! i will convert .

extropic · Jul 20, 2017

John Garner said:
Good Afternoon, All --

Is there a generally-preferred way to specify a Unified screwthread in an otherwise-metric document?

Going way back three decades or so, I received two documents – one French, the other Swiss – that called-out a 5/8-11 UN thread as “MS 15.88 x 2.31” . . . which was oddball enough that it’s clear in my memory still. More recently, I have seen “.2500 - 28 UNJF” on a metric drawing I've been asked to review, and although I think that citation better than the pseudo-MS citation, its reliance on the “UN” to communicate the unit transition to inches doesn’t seem adequate.

My own inclination would be to say something along the lines of “1/4 inch x 28 thread per inch, J-form Unified screwthread”.

If there is a generally-preferred way of making such a citation, I’d like to know what it is; if there isn’t, I’d like to know your thoughts on the question.

Thanks,

John

Does your "document" specify a controlling Standard, such as ANSI Y14.5?

If it does specify a Standard, as all technical documents should (personal opinion), look up the Standard and follow it.

If the preparers of the "document" don't, or won't specify a controlling Standard, it's my practice to do as Y14.5 specifies anyway.

You seem to be located in the USA. ANSI Y14.5-(appropriate year) "Standard establishes uniform practices for stating and interpreting dimensioning, tolerancing, and related requirements."

If the intent is to describe the characteristics of a purchased part, my preference is to describe in the Parts List by using the manufacturers nomenclature. If I felt compelled to describe the thread on the face of a drawing, I would show it as REFERENCE information and describe the thread as per the manufacturers nomenclature. After all, the "document" that you are working on is NOT controlling the thread. The nut plate manufacturer's practice/documentation (what ever that may be) is controlling the thread.

Sarcasm redacted.

John Garner · Jul 21, 2017

I thank all of you who have commented, I appreciate your time and effort.

Just for the record, the drawing isn't mine, and I don't have the whole drawing. I was asked to review and comment on the one sheet. I wholly agree with those of you who commented on the absurdity of the four-place decimal Major Diameter callout, which matches the absurdities of the 101.6 millimeter spacing of screw holes and their +/- 0.254 millimeter spacing tolerance.

IanX · Jul 21, 2017

5/16"-18 I have as stop screws on a little turret. 5-16-18 says "Again he prayed, and the heavens gave rain, and the earth produced its crops". The fraction slash and the quotation mark used to denote Inch (Pouce, Zoll) followed by the thread count seems adequate for most work.

Dinosaur Engineer · Jul 21, 2017

It's quite common to call out UNC/UNF (or BSW) threads on metric standard drgs. UNC threads are used when a stronger coarse thread form is required. UNC threads are still used by some Auto makers for cast iron engine block threads and even German manufactures use BSW form pipe threads. Aircraft fittings still use American std threads on metric drgs. All engineers I've met understand what 5/8" - 11 UNC 2b means.

Lambert · Jul 22, 2017

I grew up in metricland and occasionally see some imperial threads called out.

Just put the minumum amount of info needed on the drawing to get the the thread you need in your product.
Don`t clutter the drawing with all kinds of info when all you care about is a certain thread in a specified place.

Size of thread, type of thread and optionally toleranceclass... that`s all !

gregormarwick · Jul 22, 2017

I work with parts everyday that are fully metric from conception to manufacture, ones that are inch from start to end, and ones that have been converted at every step in the middle. Unless the drawing is complete garbage, threads are called out according to the standard they belong to, regardless of drafting standard or units used.

1/4-28UNJF is what I would expect to see on your drawing.

How to specify a Unified screwthread in an otherwise-metric documument?

Titanium

Diamond

Diamond

guest

Guest

Titanium

Plastic

guest

Guest

Stainless

Stainless

Aluminum

Cast Iron

Diamond

Diamond

Diamond

Stainless

Titanium

Aluminum

Aluminum

Hot Rolled

Diamond

Similar threads