Machinist

[Lawrence London <lfljvenaura@gmail.com>]

http://www.practicalmachinist.com/vb/general/manual-lathe-threading-question-261962/


chappyman
chappyman is offline Plastic

Join Date
    Mar 2012
Location
    South Florida
Posts
    4   

Default Manual lathe threading question...

    Hello there.. I've recently purchased a 10x22 lathe, and I've been
making small projects and tuning things up on it for a while. I'm
feeling fairly confident in my ability at basic operation of it,
however I really lack any formal training aside from machine shop I
and II at the local community college 20 years ago, and I'm a little
confused when it comes to threading. The way I've always understood
threading on a lathe, I can internally and externally thread any pitch
I want (within the lathes capability) on any size shaft or internal
diameter (within the lathes capability). Im having trouble figuring
the thread depths however, and its really irritating me. Id be
grateful to anyone who could teach me a thing or two about this
subject.
    According to my 1968 eighteenth edition Machinery's Handbook,
under American Standard Unified Thread Form Data chart, the depth of
external thread for 20 tpi is .03067", and the depth of internal
thread is .02706". Now, to me this seems to say that there is .00361"
of clearance between the od. of the shaft threads and the od. of the
internal thread. So, in theory anyhow, assuming my internal threads
are cut properly to .02706, can I just turn the shaft to this diameter
before cutting the external threads using this little formula?

    Dia. hole + .02706" - .00361" = correct shaft dia.

    Example: turning 20tpi in a hole of .750"
    .75+.02706-.00361= .77345 shaft dia.

    Does this make sense?

    Like

Quick reply to this message Reply   Reply With Quote Reply With Quote
 Multi-Quote This Message
03-09-2013, 03:01 PM #2
Putch's Avatar
Putch
Putch is offline Cast Iron

Join Date
    Nov 2011
Location
    Butler, PA
Posts
    456 

Default

    Are you trying to make a custom thread size? Why not just stick
with a standard thread and go by the numbers in the book, then as you
get good at cutting normal threads, you will learn what you need to.
Cut the internal thread first, then cut your external thread to match
it. That way you can use your internal thread as a gage to figure out
when to stop cutting your external thread. You can flip your threading
bar upside down, cutting in reverse - starting in the back thread
relief and cutting away from the spindle and out of the hole so you
don't have to worry about crashing into a wall in the back of the
bore. Just make sure you're cutting ON CENTER! Going by the numbers is
good, but you'll probably find you always have to cut a little deeper
than your numbers say to, due to small inaccuracies in alignment,
cutter angle, tool wear and so on. Oh, and cutting threads at 29 1/2
degrees offset from the face of the part allows the tool to cut only
with the leading edge of the cutter, instead of with both sides of the
tool which causes twice the cutting force to be exerted on the tool,
part, and machine, giving you less than desired results. Good luck!

    Like

Quick reply to this message Reply   Reply With Quote Reply With Quote
 Multi-Quote This Message
03-09-2013, 03:16 PM #3
thermite
thermite is offline Diamond

Join Date
    Sep 2011
Location
    Mid-Atlantic USA, South China
Posts
    5,653       

Default

    Quote Originally Posted by chappyman View Post
    Hello there.. I've recently purchased a 10x22 lathe, and I've been
making small projects and tuning things up on it for a while. I'm
feeling fairly confident in my ability at basic operation of it,
however I really lack any formal training aside from machine shop I
and II at the local community college 20 years ago, and I'm a little
confused when it comes to threading. The way I've always understood
threading on a lathe, I can internally and externally thread any pitch
I want (within the lathes capability) on any size shaft or internal
diameter (within the lathes capability). Im having trouble figuring
the thread depths however, and its really irritating me. Id be
grateful to anyone who could teach me a thing or two about this
subject.
    According to my 1968 eighteenth edition Machinery's Handbook,
under American Standard Unified Thread Form Data chart, the depth of
external thread for 20 tpi is .03067", and the depth of internal
thread is .02706". Now, to me this seems to say that there is .00361"
of clearance between the od. of the shaft threads and the od. of the
internal thread. So, in theory anyhow, assuming my internal threads
are cut properly to .02706, can I just turn the shaft to this diameter
before cutting the external threads using this little formula?

    Dia. hole + .02706" - .00361" = correct shaft dia.

    Example: turning 20tpi in a hole of .750"
    .75+.02706-.00361= .77345 shaft dia.

    Does this make sense?
    Do a search on 'thread wires', specialized mics, and thread
measurement in general and discover it is as much of a PITA to measure
them as to make them.

    Take Putch's advice as to just making it FIT.

    Grab a few hardware-store nuts and bolts 1/4" through 3/4" and
practice making mating male and female parts to fit each. Keep in mind
these are 'sloppy' fits, but you'll soon get the hang of what works
and does not work at a cheap-enough investment before risking anything
harder to replace.

    Bill

    Like

Quick reply to this message Reply   Reply With Quote Reply With Quote
 Multi-Quote This Message
03-09-2013, 03:31 PM #4
chappyman
chappyman is offline Plastic

Join Date
    Mar 2012
Location
    South Florida
Posts
    4   

Default

    I don't have problems with the standard sizes, its the "custom"
sizes. I need to thread inside of thin walled pipe and shafts.

    Like

Quick reply to this message Reply   Reply With Quote Reply With Quote
 Multi-Quote This Message
03-09-2013, 04:06 PM #5
thermite
thermite is offline Diamond

Join Date
    Sep 2011
Location
    Mid-Atlantic USA, South China
Posts
    5,653       

Default

    Quote Originally Posted by chappyman View Post
    I don't have problems with the standard sizes, its the "custom"
sizes. I need to thread inside of thin walled pipe and shafts.
    Eh .. well if you really mean it that way, then is it the
measurement calculation or the measurement 'method' or device that is
the nut to crack?

    Bill

    Like

Quick reply to this message Reply   Reply With Quote Reply With Quote
 Multi-Quote This Message
03-09-2013, 04:07 PM #6
manualmachinist
manualmachinist is offline Aluminum

Join Date
    Oct 2012
Location
    Washington, USA
Posts
    131 

Default

    Here is a simple formula from the Henry Ford book that works for
almost any internal thread.

    1.0825 divided by the TPI subtracted from the Thread’s OD provides
the size to bore the hole before threading.
    Thread the internal to fit the gage that you have made to the
pitch diameter for the thread, using thread measuring wires or a pitch
micrometer.

    Like

Quick reply to this message Reply   Reply With Quote Reply With Quote
 Multi-Quote This Message
03-09-2013, 04:19 PM #7
chappyman
chappyman is offline Plastic

Join Date
    Mar 2012
Location
    South Florida
Posts
    4   

Default

    The calculation.

    Like

Quick reply to this message Reply   Reply With Quote Reply With Quote
 Multi-Quote This Message
03-09-2013, 04:20 PM #8
thermite
thermite is offline Diamond

Join Date
    Sep 2011
Location
    Mid-Atlantic USA, South China
Posts
    5,653       

Default

    Quote Originally Posted by manualmachinist View Post
    Thread the internal to fit the gage that you have made to the
pitch diameter for the thread
    +1

    Making a custom TAP (or die..) is a PITA. Making a custom GAGE is
easier. Needn't have cutting edges, relief, nor even necessarily be
hardened.

    Bill

    Like

Quick reply to this message Reply   Reply With Quote Reply With Quote
 Multi-Quote This Message
03-09-2013, 04:20 PM #9
chappyman
chappyman is offline Plastic

Join Date
    Mar 2012
Location
    South Florida
Posts
    4   

Default

    Thanks very much, and I'll give that a try..

    Like

Quick reply to this message Reply   Reply With Quote Reply With Quote
 Multi-Quote This Message
03-09-2013, 04:27 PM #10
thermite
thermite is offline Diamond

Join Date
    Sep 2011
Location
    Mid-Atlantic USA, South China
Posts
    5,653       

Default

    Quote Originally Posted by chappyman View Post
    Thanks very much, and I'll give that a try..
    Tad bit of taper ELSE step-cuts undersized on the leading end doesn't 
hurt.

    Otherwise it is a long and tedious process of too-tight, too-tight
..... Oh shit, too loose now! . 'coz it doesn't want to even START...



    Bill

    Like

stephen thomas and 1HobbyMachinist like this.
Quick reply to this message Reply   Reply With Quote Reply With Quote
 Multi-Quote This Message
03-09-2013, 04:50 PM #11
Sean the Dog
Sean the Dog is offline Aluminum

Join Date
    May 2011
Location
    Nova Scotia
Posts
    175 

Default

    You are right about being able to cut almost any pitch on any
diameter, within reason. Lathe capability is not the only limiting
factor however; the amount of material available also matters greatly.
Cutting 8 tpi on a 1/8 OD shaft will result in some chips and no
shaft. Cutting 40 tpi on an 8.0 in shaft looks like a roughing cut.

    The numbers you gave as an example (actual numbers to be used?) do
seem workable, although I do see three problems with what you are
trying to do.

    #1 - The clearance you specify is based on a single depth of
thread; that is, the depth on one side. In reality, because the thread
is cut around - on both sides - of the shaft, your clearance would be
twice what you think. ex: 0.00722, not 0.00361

    #2 - Your numbers seem to be based on perfect v-shaped threads. In
reality, such threads don't exist. Allowances have to be made for tool
tip wear, and for the fact that no cutting tool is perfect. This is
why ranges are given in other charts (including in Machinery's
Handbook) for all aspects of thread dimensions. Looking at another
chart and doing some math will give you numbers you need. Sort of.

    #3 - Working with an established minor diameter in a nut makes
things much more difficult because you will not have an actual nominal
outside diameter to apply calculated numbers towards. (This will make
sense in a minute.)

    Here is what I would do, for what it's worth:

    I looked in the Handbook 26th Edition and found a 20 tpi thread
whose nut's ID was close to your 0.750. 3/4-20 UNEF was the best, at
0.696 to 0.707. Only class 2 threads are listed; you could calculate
numbers based on class 3 specs if wanted, but you will have to look at
a different thread.

    NUT: difference between nominal OD and ID= 0.054 to 0.043,
therefore OD based on 0.750 ID would be 0.804 to 0.793 (Being inside a
nut, there is no way to measure this, but it will let you know if your
pipe's OD is big enough.)

    SCREW: OD should be 0.0013 to 0.0094 smaller than nominal OD size.
We don't have an actual nominal OD, so guesstimate OD sizes here would
be anywhere between 0.8027 to 0.7836. That's an awful lot of range.

    I hope you are making both threads, because there is no easy way
to standardize this with someone else's work. I would make the
external thread first, just because it's easier to see what you are
doing.

    I would cut the external thread OD to a little below 0.800, using
0.800 that as a sort of nominal. Cut the thread to what appears to be
a good depth. If plunge cutting, use 0.0307 but use 0.0375 if
infeeding with the compound (0.75/p). If you have a way to measure the
thread PD, it can be calculated based on the new OD.

    Then, cut the inside thread to fit.

    Good luck with this. Let us know how it turns out.

    Like

Quick reply to this message Reply   Reply With Quote Reply With Quote
 Multi-Quote This Message
03-10-2013, 12:28 AM #12
Mike C.
Mike C. is offline Diamond

Join Date
    Nov 2004
Location
    Birmingham, AL
Posts
    9,747       

Default

    On custom work, inside or outside, at our hydraulic shop, I will
not even attempt to cut a thread unless I have the mating part in hand
for test fit. On custom work, most of it is made to fit, as the guys
above wisely advise. If you make your part exactly to spec and the
mating piece is not to spec and doesn't fit, you catch hell, no matter
how perfect your work. I have a formula I use to get me in the
ballpark, but it VERY rarely works out exactly on the money. I usually
stop a little before the spec fit and start test fitting from there.

    Like

Quick reply to this message Reply   Reply With Quote Reply With Quote
 Multi-Quote This Message
03-10-2013, 12:51 AM #13
Gordon Long's Avatar
Gordon Long
Gordon Long is offline Cast Iron

Join Date
    Oct 2006
Location
    San Leandro, California
Posts
    475 

Default

    Sean did a good job of explaining his approach.
    One ballpark method you may want to check is to add the pitch of
the thread to the inside diameter of the pipe you are threading. That
would give you your nominal thread diameter.
    This is like calculating a tap drill diameter. Tap drill size is
basically OD minus pitch. Take for example a 3/8-16, 3/8 minus 1/16 =
5/16 which is what most tap drill charts will give you.
    With that number, touch your thread boring tool to the ID of the
pipe and then the amount you feed your tool will be the nominal OD
minus the pipe ID. Like Mike C. advises, start checking your fit
before you hit your final target. I would only get scientific about
the exact dimensions if I didn't have the mating part on hand.
    The other thing to remember about the Unified National thread form
is like Sean explained, that the male thread doesn't have a sharp
point. I usually just cut the OD to about .005" smaller than the
nominal OD for the average range of diameters I use. I think the
actual width flat = 1/8 times the pitch of the thread.

    Like

Quick reply to this message Reply   Reply With Quote Reply With Quote
 Multi-Quote This Message
03-10-2013, 02:09 PM #14
stephen thomas
stephen thomas is offline Diamond

Join Date
    Jun 2001
Location
    downhill from Twain\'s study outside Elmira, NY
Posts
    5,824       

Default

    Thermite's note about fitting is spot on. For whatever reason,
(tool "jump" at the start on looser/small lathes?) a male thread can
be a little bigger and a female a little smaller at the starting end
unless you consciously reduce it a little. On the male it can be as
simple as a healthy chamfer _after_ thread cutting. Female, multiple
passes on the first thread, plus chamfer. Or very short, very slight
step in the bore. Not saying "do anything real obvious, just, be
aware, and compensate a little.

    I would almost always make the male thread first. It just works
out easier. Even if you don't have to fit a given size, it is easier
to make it "perfect" including check over small drill shanks (if you
don't have wires or thread mics) that the threads are parallel. Then
make the female to fit.

    smt