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.
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?
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
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
On Thu, 23 Oct 2008 10:00:47 -0700, Jim Stewart
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.
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).
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.
On Thu, 23 Oct 2008 00:08:32 -0500, Richard J Kinch
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.
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.
On Thu, 23 Oct 2008 16:01:10 -0500, Richard J Kinch
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.
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.
On Fri, 24 Oct 2008 01:28:41 -0500, Richard J Kinch
"Limits" makes sense to me.
I certainly don't claim to understand the whole subject either. For
instance, the thread tables aren't sufficient to completely specify a
good thread. It seems at least one more toleranced dimension is
required. I suspect the key is the illustration in my MH that shows
the proportions of internal and external thread at maximum material
condition, but I've never had a good enough reason to take the time to
work through it.
Quite so. That's why I wrote the software, partly to make sure I
understood the specification properly, and partly to yield practical
machining specs, as opposed to abstract geometry that are all the standards
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)
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)
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:
0.033 SHARP-TOOL MINIMUM OUTFEED (decrease by tool tip blunting)
*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.
Email: < firstname.lastname@example.org> | Voice (all times): (703) 938-4564
(too) near Washington D.C. | http://www.d-and-d.com/dnichols/DoN.html
Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here.
All logos and trade names are the property of their respective owners.