Threding

[J. Tranter]

I understand how to to single point a thread on a lathe. But how do you know how deep to go for (I know you have to take several passes) a certain pitch?
John T.

 

[mklotz]

Download my DOT (Depth of Thread) program and it will tell you all.

Here's a sample output:

DEPTH OF THREAD CALCULATIONS

Threads angle [60 deg] ?
Threads per inch [20] ?
Compound rest angle [29 deg] ?

thread angle = 60.00 deg
threads per inch = 20.0 (pitch = 0.05000 in/thread)
{compound feed at compound angle = 29.0 deg}

(A) dot sharp crest - sharp root = 0.04330 in {0.04951 in}
(B) dot flat crest - flat root = 0.02706 in {0.03094 in}
(C) dot sharp crest - flat root = 0.03248 in {0.03713 in}
(D) dot flat crest - sharp root = 0.03789 in {0.04332 in}
(E) double dot sharp crest - sharp root = 0.08660 in

For American National (60 deg) thread form, subtract 0.0325 in from
major diameter (assumes p/8 flat on crest) to obtain pitch diameter

use any line on threading dial

 

[rake60]

John

At the risk of over simplifying it, I'd suggest you have a look at this link.
Thread Cutting Guide

The V Tool single depth number will be real close to the perfect fit
advancing the tool straight into the cut. For larger diameter threading
you need to consider the compound setting method.
If it doesn't fit take a spring cut.
If it still doesn't fit take cuts of .002" at a time until it does.
No Black Magic there...

As Marv said you can use any number on the thread dial for any even number
pitch if it is a American National 60 deg thread, as long as you engage the
half nut on the SAME number every time.
If the thread is an odd number the documentation that came with your lathe
will show what thread dial number you need to use.

Rick

 

[Mcgyver]

With the compound at 29.5, for a 60 degree V thread, advance the compound in .750/tpi. Fit of course depends on the OD you start with, that formula assumes the OD is the correct amount under the nominal size. What i usually do is test something on when I'm getting close or chase it with a die. The proper way to do this, and how you should proceed for higher class work is to use a thread mic or thread measuring wires

 

[rake60]

Single point threading seems to be a scary thing for many new beginners.
I'll admit it was for me in a job shop environment at first!
After years of experience I lost all that to, "Make It FIT!"

Just think about it for a second.
How tough is it to cut a shallow "V" groove in a piece of stock?
How challenging is it to feed a tool at a faster than average rate
along that piece of stock, starting each cut at the same reading
on a slow spinning dial?

Combine those two simple processes and you end up with a thread.

At work I've cut 2" pitch buttress threads 1.032" deep.
At home I've cut 56 pitch V threads .013" deep.
The only difference between them is the number of cuts to produce the
finished threads.

At work every thread I cut is measured over wires or triangles.
My name is on that "In Process Inspection" report that will be attached
to that part until it reaches the end user. If it doesn't fit there's hell to pay!
At home it's a much less stressful level.
Just make it fit!

It can be as simple or as complicated as you wish to make it.
Either way, if end result fits the mating part, it's a success.

Rick

 

[mklotz]

Using the threading dial often seems a bit of a mystery for newcomers. Some time ago, I wrote a brief treatise on this subject for the members of our club. This seems like a good place to pass it along...



USING THE THREADING DIAL

Some folks are confused by which marks to use on the threading dial on their
(assumed Imperial) lathe. Of course, you're always safe restarting on the
same dial mark on which you started but that means you'll spend a lot of time
'waiting for your number to come up'.

It's pretty easy to think through. Most dials have four numbered marks
labeled, unsurprisingly, 1-4. Between these marks are smaller, unnumbered
marks.

[Aside: A consequence of the four numbered mark dial is the fact that the
gear that meshes with the feed screw will have a number of teeth which is four
times the tpi of the feed screw, i.e., an 8 tpi lead screw will have a 32
tooth gear on its thread dial. This is worth knowing if you intend to build a
threading dial for a lathe that lacks one. Since there's no load on this
gear, a perfect match to the helix angle of the lead screw is not needed. Any
old gear with the right number of teeth can be pressed into service.]

The numbered marks almost always correspond to a carriage movement of one
inch. (However, you should confirm this by actual measurement on your lathe.)
By deduction, the unnumbered lines must then correspond to a carriage movement
of one-half inch.

Now, suppose I'm cutting an even-numbered thread (e.g., 32 tpi). If I move the
carriage by one-half inch, the tool will reenter the thread perfectly. If I
move the carriage one inch, the tool will also reenter. Therefore, I can
reengage the half-nuts on ANY line on the threading dial.

If I'm cutting an odd-numbered thread (e.g., 13 tpi), the tool will not reenter
the thread if I move one-half inch - I have to move one inch. Therefore, I
must reengage the half-nuts on ANY NUMBERED LINE on the dial. (If I started
the thread on an unnumbered line, I would then reengage on unnumbered lines but
that is generally too difficult to remember in the 'heat' of thread cutting and
should be avoided.)

If I'm cutting a half-fractional thread (e.g., 11-1/2 tpi), the tool will only
reenter the thread every two inches. Therefore I must reengage the half-nuts
on ONLY THE ODD NUMBERS ON THE DIAL (1 and 3) or on the even numbers (2 and
4). It's a good idea to decide on one of these options and always stick with
it. I always start the thread on 1 and then use either 1 or 3 to reengage.

Rarely, a lathe can cut a 1/4 thread (e.g., 1-1/4 tpi). This thread will only
repeat every four inches so, in cutting such a thread, one would reengage the
half-nuts on the same mark one used to start the thread.

 

[mklotz]

If you're cutting threads, you really need to have a so-called 'fishtail' (center) gauge.

http://www.use-enco.com/CGI/INSRIT?PMAKA=890-1357&PMPXNO=3377754&PARTPG=INLMK3

On that gauge are some thread depth numbers. The trick is knowing what to do with those numbers. Some time back, I investigated this subject and wrote up my discoveries for our club...


Some time ago I wrote a treatise on the fishtail gauge (see below the =====
line) where I puzzled about the utility of the "double depth of sharp thread"
numbers on every one of these gauges I've seen. I concluded that, since the
tool is advanced using the (angled) compound, these numbers weren't terribly
useful and wondered why they were there. The numbers do not take into account
the effect of the angled compound so they seemed useless.

Since then I've come across some new information that may provide a solution to
my puzzlement. I'd like to pass that along since it will be of use to those of
us who screwcut threads.

In his book, "The Model Engineer's Workshop Manual", the author, George H.
Thomas, describes a simple and intriguing method for cutting a thread.

1. Using the cross-slide, bring the tool up to touch the work and zero the
cross-slide dial. Also zero the compound dial.

2. Move the carriage to the right to clear the end of the workpiece and feed
the cross-slide in by "the thread depth". Depending on how your cross-slide is
calibrated (diameter reduction or actual movement), this is either the number
on the fishtail gauge or half the number on the gauge. Rezero the cross-slide
dial.

3. Back off the *compound* sufficiently such that, the carriage can be moved to
the left with the tool opposite the work again.

4. Feed the *compound* forward until the tool tip just touches the work piece.

From this point you can begin cutting the thread. Keep feeding in on the
compound until the dial reads zero again, at which point you'll be at proper
thread depth. The cross-slide can still be used to withdraw the tool at the
end of the cut. It is reset to its zero for the next cut.

There are several advantages to this technique. Note that at no point do we
need to concern ourselves with the angle of the compound. Whether you set the
compound to 29, 29.5 or 30 degrees doesn't matter. This technique
automatically compensates for the angle used. Secondly, there is no finish
value to remember for the compound - you go to zero and that's it. And
finally, all the information you need to do this is right there in your hand
on the fishtail gauge that you used to set the tool perpendicular to the work
piece.

Now you (and I) know why those numbers are on the gauge!

==============================================================================

Re our recent May meeting discussion of threading, and specifically, the depth
of thread...

Like most folks who thread on the lathe, I have a fishtail gauge (also called a
center gauge) which I use to ensure that the thread cutting tool is
perpendicular to the work.

On said gauge (and most others that I've seen) is a set of numbers labeled
"double depth of sharp thread". Specifically, the numbers on mine are those
given in columns A (tpi) and B (double depth of sharp thread) in the chart
below. I've always guessed that these numbers were somehow useful in deciding
how much to feed in when cutting a thread but I never took the time to sort out
how to use them. (For me, it's always been easier to draw a picture of the
thread and derive the depth I need using mathematics.)

A couple of questions at the meeting made me decide to puzzle out, once and for
all, what those numbers really are and how to make use of them.

Mathematically, the height of a thread, measured perpendicular to the thread
axis from sharp root to sharp crest is given by the following equation.

h = .5*pitch/tan(30)

where:

h = height of thread
pitch = 1/tpi

The little program I wrote prints out two times 'h' in column C in the table
below. As you can see, 2*h agrees perfectly with the numbers printed on the
fishtail gauge.

So the numbers on the gauge are indeed as described - the "double depth of
sharp thread".

So now the question becomes, "Why are those numbers on the fishtail gauge?"
Those numbers aren't particularly useful when cutting the thread. Most of the
time the question is, "How much do I need to feed in the compound when it is
set to angle 'ca' (compound angle)?" Mathematically, the answer to that
question is:

cin = h/cos(ca)

where:

cin = compound infeed

I've printed out cin for ca=30 deg in column D. For this case, we have:

cin = .5*pitch/[tan(30)*cos(30)] = .5*pitch/sin(30) = .5*pitch/.5 = pitch

and you'll note that the numbers in column D are exactly equal to the pitch of
the thread with tpi as given in column A.

So, the bottom line here is that I still don't know why those numbers are
there. Perhaps an old school machinist can explain how to use them but I
don't see any immediate value to them. (I can't imagine a machinist
multiplying the number in column B by .5/cos(ca) to get the compound feed
depth he needs.) If you didn't angle the compound at all when cutting threads
(i.e., feed straight in with the cross feed) and your crossfeed was calibrated
in diameter reduction (a .001 feed reduces diameter by .001), then the numbers
in column B would be your infeed to cut that thread. But what competent
machinist wouldn't angle the compound?

I don't know the answer but I do know this...I'm going to continue to ignore
the numbers on my fishtail gauge and base my calculations on what I understand.

A B C D

4 0.433 0.433 0.250
5 0.346 0.346 0.200
6 0.289 0.289 0.167
7 0.247 0.247 0.143
8 0.217 0.217 0.125
9 0.192 0.192 0.111
10 0.173 0.173 0.100
11 0.157 0.157 0.091
12 0.144 0.144 0.083
14 0.124 0.124 0.071
16 0.108 0.108 0.062
18 0.096 0.096 0.056
20 0.087 0.087 0.050
22 0.079 0.079 0.045
24 0.072 0.072 0.042
26 0.067 0.067 0.038

 

[rake60]

Marv your information is as always very detailed and perfectly correct,
but it would scare a first time beginner to death...

For model scale threading I have never used the compound method.
A tool ground from a HSS bit with proper clearance will cut a clean
thread at straight in full tool pressure if the SFM speed is correct.
My own home ground threading tool is nothing special.
It's was simply hand ground to fit the fish tail gage.

I cut threads at a relatively high speeds. If you thread at very slow
speeds the tool pressure of a straight in cut definitely does become a
concern even on a shallow depth thread.

Threading is very much like driving. The driver of the car in the
lane next you may think your a total idiot, but if it feels right to
YOU it's right!

I believe I've posted this video before, but here it is again...
It's cutting a 10-32 thread in brass at 300 RPM.
In brass you do NOT need to run that fast to get a clean thread,
it's just my twisted mind at the controls.
It consists of 4 cuts and 1 spring cut straight in to reach the
depth of .019" The nut I used as a size piece fit with very little
slop on the first try.
[ame]http://www.youtube.com/watch?v=pAwy6CUnzJ8[/ame]

A 10-32 thread is a great size to practice with.
It's major diameter is .190" MAX / .184" MIN so a piece of
3/16" brass rod fits the application perfectly.
Being an even number pitch any number on the thread dial
will work just fine.

OK so a 10-32 is so small, why not just use a die?
You can train a monkey to turn a die...
Single point cutting that thread is a satisfaction that monkey
will never know!

I worked for a Foreman for a few years who offered the same
answer to every question you'd ask him.
It was, "JUST CUT THE

THING!"

Threading is one process where that is the absolute best way
to learn.


Rick

 

[lathe nut]

Fellows, to a guy like me threading is something that I want to master, I have wanted to make some projects and was turned off when I saw threading, that die business is not of much use, it is having the satisfaction that I did it, can only learn from some one that is good at it and does it right the first time that can teach someone that wants to learn, I have been a salesman in the Oil Field for 30 years, that was the hardest job that I had ever done, many days I would go back in the office and ask the boss to put me back in the field, he would sit me down and help me with the art of selling, now it is easy but when we put a new saleman on I help train them, the are scared and ask questions, about the product, what If I cannot answer the customer, customer complaints, over coming not getting the sale, being responsible for keeping the business, I think that we if moving forward will never become complacent always learning every seeking knowledge, I hope some day to be able to say that it is so simple to thread, I am doing some each time I can get in the shop, so for I do find that it is easier to do fine threads, thanks for all the help, I need it, take care, Cando

 

[J. Tranter]

It consists of 4 cuts and 1 spring cut straight in to reach the
depth of .019"

I've single point threaded before and I know how to do it. But how do you know how deep to go before the thread is done?

Rick how did you know to go to a depth of .019 on that thread?Or how do I know how deep to go on say an 1.5 8 thread?

 

[Bogstandard]

Cando,

I think all the ones 'in the know' on here realise that if threading with a single point tool is mastered, it opens a whole new world. You are not limited to what you can buy.

You can turn threads to any shape and size you want.

There is no easy way to explain it. You can have all the theory on how to do, pictures and vids showing what to do next.

The only real way to learn and get over the fear, is to get on the lathe and try for yourself. Hopefully with someone at your shoulder pointing the way, but if not, learn the basics by yourself.

Set aside an hour or so 'playtime'. Mount up a bit of brass rod in the lathe (brass is a lot more forgiving than most other metals when trying new techniques), not thin stuff, give youself a bit of meat to play with, say around 1/2" or above. If you haven't got a threading tool, grind one up yourself, doesn't have to be perfect 60deg angle at this stage, just make sure you have got the clearances and rakes correct.

Put your lathe on the slowest speed it will run at, and just play for an hour, trying to cut threads. Take it very steady at first, get bolder as you progress.

Once you can see what you are trying to achieve, and how the lathe does its work when levers are moved, then you can go and learn about topslide offsets, speeds and feeds, grinding the correct angles, how to set your lathe up to get different pitches etc.

If you make it too much like going back to school, you will just lose interest in doing it.

Play first, lessons later.

Not enough people 'play' with their machinery. They expect to dive in and get it perfect straight away, and usually end up disappointed.

I still 'play' with my machines when I want to learn a new technique, and I've been 'playing' with them for more years than I care to remember.

Just enjoy it.

John

 

[lathe nut]

Bogstandard, You are right, practice, I have been doing a lot of that here lately, I put something in the chuck, and make an attempt, I can now cut with easy in the 95 RPM, I have a new 14X40 HF lathe, that is a lot better than the wore out others that I have, that helps, I can cut the fine threads easier than the course, found that I was possible feeding in to much when cutting the course threads, so when the bit bits in the work and damages it, take it out try again and if happens again, cool of time try it the next day, going to get there, thanks for the encouragement, lathe nut

 

[Bernd]

Play first, lessons later.

Not enough people 'play' with their machinery. They expect to dive in and get it perfect straight away, and usually end up disappointed.

I still 'play' with my machines when I want to learn a new technique, and I've been 'playing' with them for more years than I care to remember.

Just enjoy it.

John

Bogs,

Truer words were never spoken. That's how I learned a lot. And it doesn't only apply to machine tools.

Bernd

 

[Mcgyver]

I've single point threaded before and I know how to do it. But how do you know how deep to go before the thread is done?

Rick how did you know to go to a depth of .019 on that thread?Or how do I know how deep to go on say an 1.5 8 thread?

JT, I wrote how in my earlier post. with the right flat stoned on the front of the tool and the compound at 30, advance the compound .750/tpi. for a 8tpi thread, thats .09375. with the tool touching the work, you want to advance the compound in .09375 (over many passes of course!) You should get some text and a copy machinery's handbook - its hard to completely get the theory (which is important to be able to do the practical) without the content and I'd be typing until dinner and still not get it all.

In practice, since we don't want to stone on different width flats for every thread we have to cut, use the .750/tpi as a guide and as you get close, test with its mating part OR use thread measuring wires to measure the thread pitch with a micrometer

 

[mklotz]

Marv your information is as always very detailed and perfectly correct,
but it would scare a first time beginner to death...

Rick

Yes, Rick, sometimes my answers to a simple question can be akin to drinking from a firehose. Nevertheless, I think it's important that we try to answer newcomer questions as completely as possible. They should know the details involved even if they don't adhere to all of them from the start. Experimentation is always good for the newcomer but it's important for him to understand where that experimentation should lead him.

The OP's original question was how deep to feed the tool. My answer to that question was about as simple as it gets - a program that will give him the number he requires for any pitch. You then mentioned the thread dial and I thought it was worth expanding on how it is used for each type of pitch (even, odd, 1/2).

But, more important, there's a technique he can use where he needs nothing more than the fishtail gauge numbers and that is outlined in my third post.

It may take a bit more concentration to read these longer treatments of the subject but I try to make them directly useful to the newcomer. Remember, I'm a self-taught amateur myself so I'm writing from the viewpoint of someone who had to do the experimentation to learn this myself.

A further concern is the folks who may read this thread in the future. My hope is that they will benefit from seeing a complete treatment of the subject in one place.

 

[rake60]

Points well taken Marv.

J. Tranter, I cut threads to the published Double Depths.

Perhaps a little insight into my own threading experience is in order.
My very first job was at a production machine shop known locally as
"The Screw Factory" They didn't manufacture screws, but every part
made there involved a thread.
Work there was on a production scale. Die Heads and Adjustable
Tapping Heads do not require much craftsmanship.

My first REAL single point threading was on a vertical boring mill.
The machine was manufactured by the TOS company in Czechoslovakia
in 1974 and looked exactly like this one that is currently listed as an auction item.

A vertical boring mill is nothing more than a very large lathe stood up
on end. The table of that machine is 5 feet in diameter and with the saddle
up to the limit you can fit a 54" tall part under the head.
As you can see there is no compound on a vertical boring mill.
Threading means straight in cuts.
To cut a clean, chatter free, deep thread you had to use a different
method of relieving the tool pressure and avoiding a full tool cut.
A 60 deg thread is actually two 30 deg tapers that create a 60 deg included
angle. One job that was a repeat offender involved a 8 pitch thread on a 12" diameter,
at the top of a 4 foot high part. It had to be perfect! The locknut that would go that
thread would be used to set the preload of the tapered roller bearing in the final
assembly.
For an 8 pitch thread the published Double Depth charts give a number of .1624"
Why a "Double Depth" ? I have NO idea! But divide that by 2 and the depth per
side is .0812. To me as a machinist that means .082"
So you work it in .005 at a time but when it gets to .050 deep it starts to chatter.
Time to get out the calculator. The Tangent of 30 deg is .57735" multiply that by
the .031" you still need to reach that depth and you get an answer of .01789"
Shift the entire saddle up .018" Now the tool is only cutting heavy on one edge.
On the final cut at the .082 depth the tool will just scrape the original leading edge
of the first attempt at taking the thread to depth completing the full thread.

Do that often enough and you learn just how deep you can go on a thread before
becomes a complicated ordeal.

Play with it! Get some 3/16" stock and practice a 10-32 thread.
Try the straight in method, then set your compound to an approx 30 deg and try
that. Compare the results. The method that works best for you is the best way!

Rick