I need a reality check. I constructed this
7/8-20 UNEF Class 2A thread from the data I
found in the Machinery's Handbook. I can't
believe that the minor diameter lops so much
off of the lower part of the form. Is this
right?

http://www.grumpyoldgeek.com/images/UNEF_thread.jpg

On Wed, 22 Oct 2008 15:07:32 -0700, Jim Stewart
wrote:

I need a reality check. I constructed this
7/8-20 UNEF Class 2A thread from the data I
found in the Machinery's Handbook. I can't
believe that the minor diameter lops so much
off of the lower part of the form. Is this
right?

http://www.grumpyoldgeek.com/images/UNEF_thread.jpg

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.

--
Ned Simmons

Ned Simmons wrote:
On Wed, 22 Oct 2008 15:07:32 -0700, Jim Stewart
wrote:

I need a reality check. I constructed this
7/8-20 UNEF Class 2A thread from the data I
found in the Machinery's Handbook. I can't
believe that the minor diameter lops so much
off of the lower part of the form. Is this
right?

http://www.grumpyoldgeek.com/images/UNEF_thread.jpg

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.

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

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

Got it. Thanks for your help.

Jim Stewart writes:

Is this right?

No. Here is the thread data from my softwa

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)

Richard J Kinch wrote:
Jim Stewart writes:

Is this right?

No. Here is the thread data from my softwa

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




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 Simmons writes:

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.

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.

Jim Stewart writes:

Is your software available for download?

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

On Thu, 23 Oct 2008 00:08:32 -0500, Richard J Kinch
wrote:


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.

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.

--
Ned Simmons

On Wed, 22 Oct 2008 16:21:58 -0700, Jim Stewart
wrote:


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


Also make sure that the pitch diameter falls in spec.

--
Ned Simmons

Ned Simmons wrote:
On Wed, 22 Oct 2008 16:21:58 -0700, Jim Stewart
wrote:

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


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?

On Wed, 22 Oct 2008 15:07:32 -0700, Jim Stewart
wrote:

I need a reality check. I constructed this
7/8-20 UNEF Class 2A thread from the data I
found in the Machinery's Handbook. I can't
believe that the minor diameter lops so much
off of the lower part of the form. Is this
right?

http://www.grumpyoldgeek.com/images/UNEF_thread.jpg
==========
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.

http://www.vankeuren.com/tmo.aspx

Most any mill supply should have in stock. For an example see
http://www.use-enco.com/CGI/INPDFF?P...MITEM=619-3127
left 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).

On Thu, 23 Oct 2008 10:00:47 -0700, Jim Stewart
wrote:


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
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

--
Ned Simmons

Ned Simmons writes:

It seems you're confusing allowances and tolerances.

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.

Jim Stewart writes:

Also make sure that the pitch diameter falls in spec.

I'll look at that.

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

"Jim Stewart" wrote in message
.. .
I need a reality check. I constructed this
7/8-20 UNEF Class 2A thread from the data I
found in the Machinery's Handbook. I can't
believe that the minor diameter lops so much
off of the lower part of the form. Is this
right?

http://www.grumpyoldgeek.com/images/UNEF_thread.jpg

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.

On Thu, 23 Oct 2008 16:01:10 -0500, Richard J Kinch
wrote:

Ned Simmons writes:

It seems you're confusing allowances and tolerances.

No. Design sizes (what one actually attempts to fabricate) are derived
from the "basic" size (the geometric ideals) with allowance applied.

That's what I said.

The
design limits are then subordinately derived by application of tolerances
to the design sizes.

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.


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.

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.

--
Ned Simmons

On 2008-10-23, Richard J Kinch wrote:
Jim Stewart writes:

Is your software available for download?

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

*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.

--
Email: | Voice (all times): (703) 938-4564
(too) near Washington D.C. | http://www.d-and-d.com/dnichols/DoN.html
--- Black Holes are where God is dividing by zero ---

On Thu, 23 Oct 2008 10:00:47 -0700, Jim Stewart
wrote:

snip
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?
snip
-------------
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
http://www.draftingzone.com/standards/standard5/
http://www.tpub.com/content/draftsma...s/14040_51.htm
http://www.gewinde-normen.de/en/specifications.html
http://www.gewinde-normen.de/en/unif...ne-thread.html

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).

Ned Simmons writes:

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.

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.

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.

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.

DoN. Nichols writes:

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

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

See:

http://www.truetex.com/thread.awk

On 2008-10-24, Richard J Kinch wrote:
DoN. Nichols writes:

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

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

See:

http://www.truetex.com/thread.awk

Thanks! Got it and it works fine. An impressive bit of awk
programming.

Thanks again,
DoN.

--
Email: | Voice (all times): (703) 938-4564
(too) near Washington D.C. | http://www.d-and-d.com/dnichols/DoN.html
--- Black Holes are where God is dividing by zero ---

On Fri, 24 Oct 2008 01:28:41 -0500, Richard J Kinch
wrote:

Ned Simmons writes:

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.

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.

"Limits" makes sense to me.


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.

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.

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.

--
Ned Simmons

Ned Simmons writes:

For
instance, the thread tables aren't sufficient to completely specify a
good thread. It seems at least one more toleranced dimension is
required.

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
give.