UNEF Thead form

You should have a flat equal to 1/8 the pitch at the major diameter of the thread. The thread crests should be truncated to about 1/4 pitch at the minor diameter. There are good illustrations in MH, several pages before the tables in my 22nd edition.

Also note, that's a 2B thread -- 2A is the external spec.

OK, I need to put the 1/8 flat on the major diameter and then the minor diameter should fall into place.

Got it. Thanks for your help.

No. Here is the thread data from my software:

0.875"-20 T H R E A D D A T A

0.8750 D Basic diameter (in)

0.0500 P Pitch (in) 0.029 Ideal measuring wire size (in) 0.029 W First practical measuring wire size (in) 0.0437 Subtract from first wire measurement for actual pitch diameter (in) 0.032 W Second practical measuring wire size (in) 0.0527 Subtract from second wire measurement for actual pitch diameter (in) NOTE: interpolated fundamental deviation INTERP: 1.2700 on [1.0000,1.5000] onto [0.0260,0.0320] --> 0.0292 0.0012 EI Fundamental deviation (allowance), internal thread (in)

-0.0012 es Fundamental deviation (allowance), external thread (in) INTERP: 1.2700 on [1.0000,1.5000] onto [0.1600,0.1900] --> 0.1762 NOTE: ext thread pitch dia tolerance above max pitch in table INTERP: 1.2700 on [0.0000,1.0000] onto [0.0000,0.1180] --> 0.1499

0.0069 TD2 Internal thread pitch diameter tolerance (in) 0.0059 Td2 External thread pitch diameter tolerance (in) INTERP: 1.2700 on [1.0000,1.5000] onto [0.1800,0.2360] --> 0.2102 INTERP: 1.2700 on [1.0000,1.5000] onto [0.2360,0.3000] --> 0.2706 0.0083 Td External thread major diameter tolerance (in) 0.0107 TD1 Internal thread minor diameter tolerance (in)

EXTERNAL:

0.8738 dmax Major dia, max (in) 0.8656 dmin Major dia, min (in) 0.8197 d1max Minor dia, max (in) 0.8047 d1min Minor dia, min (in) 0.8414 d2max Pitch dia, max (in) 0.8355 d2min Pitch dia, min (in)

INTERNAL:

0.8903 Dmax Major dia, max (in) 0.8762 Dmin Major dia, min (in) 0.8327 D1max Minor dia, max (in) 0.8220 D1min Minor dia, min (in) 0.8506 D2max Pitch dia, max (in) 0.8437 D2min Pitch dia, min (in)

EXTERNAL THREAD PRACTICAL DATA:

0.8656-0.8738 MAJOR DIAMETER RANGE 0.8792-0.8851 PITCH DIAMETER MEASUREMENT RANGE ON 0.0290 WIRES 0.033-0.039 SHARP-TOOL MINIMUM INFEED (decrease by tool tip blunting)

INTERNAL THREAD PRACTICAL DATA:

0.823-0.833 BORE 0.033 SHARP-TOOL MINIMUM OUTFEED (decrease by tool tip blunting)

Ned got me pointed in the right direction and the problem is solved. Is your software available for download?

Which just begs the question: what are the major and minor diameters?

The ideal thread form has no direct application in practical thread cutting. It's kind of like saying holes should be round. It doesn't tell you how out-of-round your real holes can be, or how much over- or under- sized they can be. It is the latter allowances that determine how to drill or bore a real hole.

To cut real standard threads, you must stay within allowances that are rather randomly related to the ideal forms in both sign and magnitude, and which do not necessarily even include the ideal dimensions.

While the tables in Machinery's Handbook are correct, they only tell you the range of allowed results, and not the practical tool shapes and cuts that yield those results.

It's a miserable 300+ lines of GAWK code. You want that?

Not quite. It seems you're confusing allowances and tolerances. Allowances are applied to the basic (ideal theoretical) thread form to insure that male and female threads will mate under real world conditions. In other words, the allowances introduce clearance between an assembled screw and nut. The various thread classes are the result of applying specific allowances to the basic thread dimensions.

The tolerances are the acceptable deviations from the dimensions that define a specific thread and class.

Also make sure that the pitch diameter falls in spec.

I'll look at that.

Another question, if I'm making a set of drawings for a machine shop to fabricate, do I have to draw the whole form with all the dimensions or can I just spec

7/8-20 UNEF 2B on the drawing?

While you will need three hands to use it, invest in a three wire thread gage set. [Don't loose the instruction/cheat sheet that comes with it.] Hint: use a wad of modeling clay to hold the three wires in position as you measure the pitch diameter of the thread.

Most any mill supply should have in stock. For an example see hand side about 1/3 down -- thread measuring wire sets.

Unka' George [George McDuffee]

------------------------------------------- He that will not apply new remedies, must expect new evils: for Time is the greatest innovator: and if Time, of course, alter things to the worse, and wisdom and counsel shall not alter them to the better, what shall be the end?

Francis Bacon (1561-1626), English philosopher, essayist, statesman. Essays, "Of Innovations" (1597-1625).

That's the complete and proper callout for a standard UN thread, there's no need to graphically dimension the thread. You can specify thread depth either in the callout or by dimensioning the appropriate drawing view. Barring any ambiguity, I prefer putting it all in the callout.

Here's what my templates for thru and blind holes look like. (DP) stands in for the ANSI depth symbol, the one that looks like a down arrow with a cap.

7/8-20 UNEF-2B THRU

7/8-20 UNEF-2B (DP) 1.25 MIN TAP DRILL (DP) 2.00 MAX

No. Design sizes (what one actually attempts to fabricate) are derived from the "basic" size (the geometric ideals) with allowance applied. The design limits are then subordinately derived by application of tolerances to the design sizes. Thus my point that the basic sizes are of no direct guidance as to practical machining steps; one must apply arbitrary dimensions (allowances) that have no underlying "ideal".

This is why the ISO standard calls allowances by the term "fundamental deviations" in their more rational terminology. Numbers like EI, ES, ei, and es are "fundamental" in that they are arbitrary starting points that have no relation to the ideal thread forms, yet they determine the limits of practical dimensions.

The common UN threads are a surprisingly complex subject. Consider that MH takes five pages just to define the terms. Unless you respect them all, you're just kidding yourself that your results are anything but accidentally within standard.

Cf the wire sizes and micrometer ranges in my thread data listing.

From your drawing it looks like a blind hole. I the mating part screws in all the way to the bottom, there should be an internal groove turned before threading. Make the groove just bigger than the major diameter and considering the thin wall give it a small corner radius. The width of the groove should be at least two pitches.

That's what I said.

I don't doubt that's what you meant, but not what you said, specifically, "To cut real standard threads, you must stay within allowances..." The allowances are single values, not ranges that "you must stay within." That's a better description of tolerances.

Which was my point. It may seem like quibbling, but your use would likely confuse the concept of allowances vs. tolerances for someone who hasn't read those pages carefully.

*I* would like it. I live in unix, and gawk is always within reach -- without even having to install cygwin on a Windows system.

As long as the overall size of the e-mail is not over 30K it should be fine. If all of the 300 lines are 80 characters long, we only reach 24K, so we are fine.

Thanks, DoN.

------------- General convention is to simply spec as 7/8-20 UNEF 2B, possibly with spec id [eg . ANSI B1.1] This avoids double dimensioning. More recent convention is to schematically represent the threads on the print using hidden/phantom lines. Be sure to discuss with your supplier to make sure everything is clear such as length of full threads and revise the print as required per the discussion. Also be sure to verify they have recently calibrated go/no-gages and are not checking with an off the shelf nut or screw.

See

Unka' George [George McDuffee]

------------------------------------------- He that will not apply new remedies, must expect new evils: for Time is the greatest innovator: and if Time, of course, alter things to the worse, and wisdom and counsel shall not alter them to the better, what shall be the end?

Francis Bacon (1561-1626), English philosopher, essayist, statesman. Essays, "Of Innovations" (1597-1625).

Yes, an allowance proper is a single value, not a range. But it is a single value within which you must stay, an upper or lower limit or worst or best fit, the tolerance being the specification for how much within. The allowance informally is what I've called that shaded area in MH 16 p

1762 fig 6, because that is where the thread surface is "allowed to be". But I suppose the term "limits" would be more appropriate, although this is not a term in the standards.

Confusing things is a specialty of mine. I've read those pages carefully and am still somewhat confused. But at least now my parts don't come back with "won't fit" complaints.

See: