I hope somebody has the patience to read through this :-) I am trying to
include all the details because I don't know what I am doing wrong.


I recently tried to cut a 3/8-40 thread on a piece of 1018 HRS. First
pass was smooth. With later passes the surface seemed to get rough,

then before reaching final depth small sections of the thread tore out...
so I tried again:

I ground a new 60 degree HSS threading tool with 12 deg. relief on both
sides and 10 degrees side and back rake, and stoned the top and sides

smooth. It is mounted directly in a turret type tool post, (i.e. the tool
bit is horizontal, not sloped upward as in a rocker type tool holder).

I turned a 0.500 diameter section on a short bar. It is held in a three
jaw chuck, (no tailstock support).

I set up the threading tool on center height and perpendicular to the
surface.

I set up the QC gearbox for 40 TPI, spindle for slowest speed (about 40
RPM), compound slide at 30 deg.

First pass was just barely grazing the surface to ensure that there were
no surprises (i.e. mistakes in my setup), zeroed the collars.

I started by feeding in the compound 0.002", reducing progressively to
0.0005" for the last pass.

I measured the OD occasionally. It increased by 0.001" after about three
passes, i.e. it appears that a "burr" is being raised - is this

normal? I didn't expect it. I touched up the OD with a file before
proceeding.

I seem to be reaching the final thread form before I have cut as much as
I thought I needed from the Machinery's handbook, (0.01534" deep,
0.0177" on the compound at 30 degrees).

Finally on one pass I got a rather rough appearance to the thread at the
right hand end, although the rest of the thread still appears to be

smooth.

In case it's relevant I am doing this on a 10" Atlas lathe.

1) What can I do to reduce/eliminate the "burring"

2) Any ideas why I ge the rough thread, especially at the right end?

Rob

"Rob McDonald" wrote in message
...
I hope somebody has the patience to read through this :-) I am trying to
include all the details because I don't know what I am doing wrong.


I recently tried to cut a 3/8-40 thread on a piece of 1018 HRS. First
pass was smooth. With later passes the surface seemed to get rough,



1018 HRS, that is your problem!
Greg

Rob McDonald writes:

I hope somebody has the patience to read through this :-) I am trying to
include all the details because I don't know what I am doing wrong.


I recently tried to cut a 3/8-40 thread on a piece of 1018 HRS. First
pass was smooth. With later passes the surface seemed to get rough,

then before reaching final depth small sections of the thread tore out...

I had a similar problem turning threads on similar material- I gave up
on trying to get a smooth finish on the lathe, and switched to
"burnishing" on a wire wheel. Probably rank heresy but it did clean
up the burr pretty well. I was doing 1/4-20, that 40tpi might not
burnish so well...

Gregm

I agree. 1018 hrs is terrible to thread. But there are a few things to try.
You state that you turn a section to .500 dia.
I assume you meant to say that you turned a section to .375 for a length of
..500. If so, try going a little smaller. The book says you can go to a
minimum of .3691. Unless this is a very important part, I would go to about
..365 dia.. This will give you a flat on top of your thread which should
help with the burr. Also use a small triangular file to just kiss the burr.
With the lathe running, hold the file so that it is about 45 degrees to one
side of the thread and let it ride down the thread. Then hold it on the
other side and let it ride to the left again. Do this several times. Then,
make one more pass with the threading tool set at the final dimension that
you used before you used the file. This should clean up any burr you
created with the file.
You did not mention cutting oil. I like the old fashion sulfur oil. Good
luck

"Greg O" wrote in message
...

"Rob McDonald" wrote in message
...
I hope somebody has the patience to read through this :-) I am trying to
include all the details because I don't know what I am doing wrong.


I recently tried to cut a 3/8-40 thread on a piece of 1018 HRS. First
pass was smooth. With later passes the surface seemed to get rough,



1018 HRS, that is your problem!
Greg

"Greg O" wrote in
:


"Rob McDonald" wrote in message
...
I hope somebody has the patience to read through this :-) I am trying to
include all the details because I don't know what I am doing wrong.


I recently tried to cut a 3/8-40 thread on a piece of 1018 HRS. First
pass was smooth. With later passes the surface seemed to get rough,



1018 HRS, that is your problem!
Greg



Can you expand upon that? What do you suggest?

Rob

--

Also make sure the tool height is on center line.


"Chief McGee" wrote in message
news:duesc.19880$JC5.1768108@attbi_s54...
I agree. 1018 hrs is terrible to thread. But there are a few things to
try.
You state that you turn a section to .500 dia.
I assume you meant to say that you turned a section to .375 for a length
of
.500. If so, try going a little smaller. The book says you can go to a
minimum of .3691. Unless this is a very important part, I would go to
about
.365 dia.. This will give you a flat on top of your thread which should
help with the burr. Also use a small triangular file to just kiss the
burr.
With the lathe running, hold the file so that it is about 45 degrees to
one
side of the thread and let it ride down the thread. Then hold it on the
other side and let it ride to the left again. Do this several times.
Then,
make one more pass with the threading tool set at the final dimension that
you used before you used the file. This should clean up any burr you
created with the file.
You did not mention cutting oil. I like the old fashion sulfur oil. Good
luck

"Greg O" wrote in message
...

"Rob McDonald" wrote in message
...
I hope somebody has the patience to read through this :-) I am trying
to
include all the details because I don't know what I am doing wrong.


I recently tried to cut a 3/8-40 thread on a piece of 1018 HRS. First
pass was smooth. With later passes the surface seemed to get rough,



1018 HRS, that is your problem!
Greg

In article ,
Rob McDonald wrote:
I hope somebody has the patience to read through this :-) I am trying to
include all the details because I don't know what I am doing wrong.


I recently tried to cut a 3/8-40 thread on a piece of 1018 HRS. First
pass was smooth. With later passes the surface seemed to get rough,

1018 may not be the best choice -- and depending on where you
got it, it could be *very* bad. Home Depot "steel" is rather poor for
machining in any case. Very gummy, which could contribute to your
problems. And if it is of poor consistency, tearouts are more likely.
(See also the cutting oil comments later.)

then before reaching final depth small sections of the thread tore out...
so I tried again:

I don't see you mentioning *any* lubricant while cutting the
threads. I use lubricant even when threading 12L14 (about the nicest
threading steel that I have worked). I usually use one of three
lubricants, depending on the degree of difficult expected:

1) The high-sulfur pipe threading oil sold by almost everyone,
including Home Depot, packaged by Rigid (among others).

2) Molly-Dee (light oil with molybdenum disulfide).

3) Sul-Flo -- *very* high sulfur cutting oil -- best applied with
an acid brush. It has so much flowers of sulfur in it that it
looks more like mustard. It stinks when cutting, but you
produce beautiful threads.

Note that I usually use carbide insert lay-down threading tools,
typically TiN coated for the larger sizes.

I ground a new 60 degree HSS threading tool with 12 deg. relief on both
sides and 10 degrees side and back rake, and stoned the top and sides

O.K. Though ideally, there should be more relief on the
left-hand side than on the right-hand side to accommodate the helix
angle of the thread.

smooth. It is mounted directly in a turret type tool post, (i.e. the tool
bit is horizontal, not sloped upward as in a rocker type tool holder).

O.K.

I turned a 0.500 diameter section on a short bar. It is held in a three
jaw chuck, (no tailstock support).

0.500" for a 3/8-40 thread? Or is this just a test pass with a
larger diameter before going to the final diameter?

I set up the threading tool on center height and perpendicular to the
surface.

Good.

I set up the QC gearbox for 40 TPI, spindle for slowest speed (about 40
RPM), compound slide at 30 deg.

Hmm ... there are debates about the angle, but the ideal
according to some is 29-1/2 degrees -- so it does a light cut on the
right-hand flank with each pass, along with the heavy cut on the
left-hand flank.

O.K. Did you turn a runout groove at final thread depth, so you
don't have to wind the cross-slide out very quickly (and at precisely
the same point each time)?

First pass was just barely grazing the surface to ensure that there were
no surprises (i.e. mistakes in my setup), zeroed the collars.

O.K.

I started by feeding in the compound 0.002", reducing progressively to
0.0005" for the last pass.

Hmm ... for 16 TPI, I start out with 0.010" per pass, and reduce
to perhaps 0.002" for the last pass or two. I also make two or three
repeats at the final depth.

I measured the OD occasionally. It increased by 0.001" after about three
passes, i.e. it appears that a "burr" is being raised - is this
normal? I didn't expect it. I touched up the OD with a file before
proceeding.

I touch up the OD with a file after *finishing* the thread. No
point until then.

I seem to be reaching the final thread form before I have cut as much as
I thought I needed from the Machinery's handbook, (0.01534" deep,
0.0177" on the compound at 30 degrees).

Hmm ... my threads program suggest the following for 40 TPI:

================================================== ====================
izalco:dnichols 23:27 threads -i 40

For a thread of: 40.0000 TPI
the pitch is: 0.0250"/thread

| Thread Style
Format | Sharp-V | Trunc | Formed
================================================== ===================
Single depth: | 0.0217" | 0.0189" | 0.0135"
Double depth: | 0.0433" | 0.0379" | 0.0271"
29.5 deg. angle feed: | 0.0249" | 0.0218" | 0.0155"


Note: Sharp-V is top and bottom sharp. (Not often the best choice.)
"Trunc" is top truncated only.
"Formed" is both top and bottom truncated or rounded.

Select whichever suits your needs and available tooling.
================================================== ====================

The pitch calculation is for convenience in using a small CNC lathe
which I have. "Single depth" vs "double depth" is because some lathes
have handwheels calculated in diameter removed, instead of radius. My
program calculates for 29.5 degrees, not 30 degrees, as that is the
angle which I use. You seem to be getting shallower cuts than my
program suggests for a pointed tool and truncated crests.

However, one other thing comes to mind -- how tight are the gibs
on your lathe? If they are too lose, the compound or the carriage will
rock to one side under cutting loads, thus possibly tearing out the
thread, even in the presence of adequate lubricant.

Lock the carriage, and press sideways on the toolpost. See how
much it rocks. If it is any preceptable amount, you need to tighten the
gibs to prevent this. While it is possible to set the point of the tool
over the center of the ways, to minimize the sideways thrust, as you
crank the compound, you will exit that sweet spot.

The forces can also cause the tip of the tool to dip, placing it
below the centerline of the lathe.

Finally on one pass I got a rather rough appearance to the thread at the
right hand end, although the rest of the thread still appears to be

smooth.

O.K. How long is "short" compared to the diameter of the
workpiece? If there is more than 4 times the diameter sticking out of
the chuck, you will have deflection -- to an amount dependent on the
cutting forces involved.

I would support the end with a live center, if it allowed me to
get in close enough to do the threading -- otherwise, with a hardened
half-center and proper lubrication. (The half-center is ground on one
side, so the tool can get closer to the center of the end of the
workpiece.

An alternative is a follower rest. It provides brass wear
points behind and above the workpiece, and travels with the carriage, so
it supports directly behind the cut. The positions of the wear points
counters the two most likely directions of deflection. It is
absolutely necessary when threading a long shaft, as even a tailstock
center won't support it in the middle.

Next -- what shape are the jaws in? A common wear pattern on
chuck jaws is to wear at the tips (where short workpieces are clamped)
more than at the back. So -- when you clamp something using the full
length of the jaw faces, that workpiece will be tightly clamped only at
the back, and can deflect somewhat at the front. Check the workpiece
for deflection with force to see whether this is happening. A solution,
if it is *just* the faces of the jaws, is to set them up under load, and
run a toolpost grinder (or even a toolpost mounted Dremel with a
grindstone) in a little at a time, until you get the full length of the
jaw faces cleaned up.

However, if the jaws have been tightened too much at the tip, too
often, you will have wear in the ways in the chuck, and in the jaws. If
this is the case, it *might* be possible to make new jaws with tighter
way grooves, but it would be quite difficult -- especially for someone
who is at your current stage of machining indicated by your question.
So -- a replacement (new) chuck would probably be the best bet. Bison
seems to make high quality chucks for reasonable prices. (They are from
Poland.) I have a nice 6-1/4" one on my 12x24" Clausing. I suggest
getting one with two-piece jaws, so you can replace the top jaws if they
ever become worn, or so you can fit "soft" jaws and bore to hold a
special project. I don't need that too often, but it is really nice to
have when I do need it.

In case it's relevant I am doing this on a 10" Atlas lathe.

Another set of thoughts?

1) What kind of spindle bearings? Earlier ones have bronze
bearings which are adjusted by removing shims and tightening,
and then reaming to the proper size for the spindle.

Newer ones have ball (or roller) bearings, and until they die,
all that is needed is to keep them well lubricated.

2) What is the condition of the bed near the chuck? A worn bed
will allow the whole carriage to rock as it approaches the chuck
(usually the most worn area), and this could be the cause of
your problem -- or at least one cause. In particular, with the
square bed which the Atlas line used, you could also have wear
in the width of the bed, so the carriage can move forward and
back with force near the chuck (the most worn area).

Do you get taper when turning close to the chuck?

Larger at the free end is likely deflection of the workpiece
(either bending or worn/sprung chuck jaws).

Larger closer to the chuck is more likely to be bed wear.

1) What can I do to reduce/eliminate the "burring"

File when you are done. This is normal -- especially with soft
gummy steels like you are using. Get some 12L14 to see what heaven is
like. Even with 12L14, I file after cutting to clean up the crests.

Use a proper threading lubricant. (*Not* motor oil -- one of
the ones which I mentioned above will do -- though Sul-Flo is quite
difficult to get in small quantities. A club member who *really* wanted
some bought a minimum quantity, and then sold it by the gallon to other
club members to share the costs. :-)

2) Any ideas why I ge the rough thread, especially at the right end?

At the very end suggests deflection of the workpiece, though it
could be play in the gibs of the cross-slide or the compound. Or a
combination of them all.

So -- you now have a checklist of possible causes. Someone else
may well think of something which I forgot to mention, so look at
whatever other followups appear, too.

Good Luck,
DoN.

P.S. Now that I have spent this time typing, I suspect that at least
*one* other followup will have shown up. There were none when I
started typing.
--
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 ---

"Rob McDonald" wrote in message
...


1018 HRS, that is your problem!
Greg



Can you expand upon that? What do you suggest?

Rob

The lower carbon steels all cut and thread poorly. Higher carbon, to a
point, will cut cleaner, too high and it gets hard on tooling. Most CRS cuts
better than HRS. Best yet is leaded steel. The stuff cuts and threads like
butter, compared to plain 1018 HRS. Then again, choice of material depends
on the application.
Greg

I was going to put a couple cents in, but just follow what Don said. He
covered my 2 cents and the rest of the buck.

Good info, Don.

michael

Other replies had much good info, but:


I set up the QC gearbox for 40 TPI, spindle for slowest speed (about 40
RPM), compound slide at 30 deg.

You might want to try threading at the highest speed you dare run at.
Since this is a very fine thread, you can probably do the threading
at several hundred RPM, at least.


I measured the OD occasionally. It increased by 0.001" after about three
passes, i.e. it appears that a "burr" is being raised - is this
normal? I didn't expect it. I touched up the OD with a file before
proceeding.

Definitely, the burr is normal.


I touch up the OD with a file after *finishing* the thread. No
point until then.


I seem to be reaching the final thread form before I have cut as much as
I thought I needed from the Machinery's handbook, (0.01534" deep,
0.0177" on the compound at 30 degrees).

Tool deflection or workpiece deflection is very common in threading
operations. So, I'd expect it to take more infeed to get down to
final thread diameter. How do you measure it, with wires or triangles?
Without these special tools, measiring the true thread diameter is
almost impossible.


2) Any ideas why I ge the rough thread, especially at the right end?


At the very end suggests deflection of the workpiece, though it
could be play in the gibs of the cross-slide or the compound. Or a
combination of them all.


Right! Does it make a crunching or snapping sound when threading at
that end? If so, you may need either a tailstock center or a follow
rest to support the workpiece and keep it from climbing up over the
threading tool. Long, thin workpieces will try to do this, and you can
actually see the part jumping up and down as the threading tool takes
bites out of it. Even without the tearing, you'll never get a proper
thread when the work is flexing like that.


Jon

Greg Menke wrote in
:


Rob McDonald writes:

... I recently tried to cut a 3/8-40 thread ...

I had a similar problem turning threads on similar material- I gave up
on trying to get a smooth finish on the lathe, and switched to
"burnishing" on a wire wheel. Probably rank heresy but it did clean
up the burr pretty well. I was doing 1/4-20, that 40tpi might not
burnish so well...

Gregm

Thanks Greg,

This one needs to be close fitting and smooth running so that wouldn't do
here. Besides, this is a point of honor now :-) I want to figure out what I
am doing wrong and make a good thread.

Rob

(DoN. Nichols) wrote in
:

In article ,
Rob McDonald wrote:

... I recently tried to cut a 3/8-40 thread ...

1018 may not be the best choice -- and depending on where you
got it, it could be *very* bad.

I got it from a local steel supplier (Elma Steel) it could have come from
anywhere.

I don't see you mentioning *any* lubricant

I used a cutting lubricant I had on and, but I doubt it's as good as any
of the ones you mentioned. It is time to invest in some good cutting and
threading lubricants.

I ground a new 60 degree HSS threading tool with 12 deg. relief on
both sides and 10 degrees side and back rake, and stoned the top and
sides

O.K. Though ideally, there should be more relief on the
left-hand side than on the right-hand side to accommodate the helix
angle of the thread.

Good point, I hadn't thought of allowing for the helix angle.

I turned a 0.500 diameter section on a short bar. It is held in a
three jaw chuck, (no tailstock support).

0.500" for a 3/8-40 thread? Or is this just a test pass with a
larger diameter before going to the final diameter?

Test piece after the initial failure.

Hmm ... there are debates about the angle, but the ideal
according to some is 29-1/2 degrees -- so it does a light cut on the
right-hand flank with each pass, along with the heavy cut on the
left-hand flank.

OK

O.K. Did you turn a runout groove at final thread depth, so you
don't have to wind the cross-slide out very quickly (and at precisely
the same point each time)?

Yes.

I started by feeding in the compound 0.002", reducing progressively to
0.0005" for the last pass.

Hmm ... for 16 TPI, I start out with 0.010" per pass, and reduce
to perhaps 0.002" for the last pass or two. I also make two or three
repeats at the final depth.

Knowing that I had trouble already, and that my Atlas lathe is not very
rigid I wanted to minimize deflection/vibration.

I seem to be reaching the final thread form before I have cut as much
as I thought I needed from the Machinery's handbook, (0.01534" deep,
0.0177" on the compound at 30 degrees).

Hmm ... my threads program suggest the following for 40 TPI:

This value: Formed Single depth: 0.0135" corresponds to the value for an
internal thread in the handbook. I am using the value specifed for an
external thread.

However, one other thing comes to mind -- how tight are the gibs
on your lathe? If they are too loose, the compound or the carriage
will rock to one side under cutting loads, thus possibly tearing out
the thread, even in the presence of adequate lubricant.

The gibs are tight, so I don't think this is the problem (but I'm going
to double check them anyway).

The forces can also cause the tip of the tool to dip, placing it
below the centerline of the lathe.

The turret tool holder is quite rigid, and the tool is clamped very short
to minimize this.

O.K. How long is "short" compared to the diameter of the
workpiece? If there is more than 4 times the diameter sticking out of
the chuck, you will have deflection -- to an amount dependent on the
cutting forces involved.

Nowhere near 4X. Test piece is 1" diameter protruding 1-1/2" from the
chuck, the last 1" is turned down to 1/2" diameter with a groove at the
shoulder - this simulates the configuration I would be machining on the
real part.

I would support the end with a live center,

I'll try that. The fact that the problem is worst at the end of a
cantilevered workpiece makes me think "deflection."

An alternative is a follower rest.

That is on my wish list :-)

Next -- what shape are the jaws in? A common wear pattern on
chuck jaws is to wear at the tips (where short workpieces are clamped)
more than at the back. So -- when you clamp something using the full
length of the jaw faces, that workpiece will be tightly clamped only
at the back, and can deflect somewhat at the front. Check the
workpiece for deflection with force to see whether this is happening.
A solution, if it is *just* the faces of the jaws, is to set them up
under load, and run a toolpost grinder (or even a toolpost mounted
Dremel with a grindstone) in a little at a time, until you get the
full length of the jaw faces cleaned up.

This is a definite possibility. The jaws are in lousy shape and I have
been considering grinding them as you suggest.

However, if the jaws have been tightened too much at the tip, too
often, you will have wear in the ways in the chuck, and in the jaws.

I'll look into this, I don't remember them being loose this way but it is
an old chuck. If so would definitely replace rather than repair.

..I suggest getting one with two-piece jaws,...

Thanks for the suggestion.

In case it's relevant I am doing this on a 10" Atlas lathe.

Another set of thoughts?

1) What kind of spindle bearings?

It is a babbit bearing headstock. I must admit I have had concerns here,
since it is an older lathe which is known to have spent part of it's life
in a low production environment. I lack the skills to confidently
determine it's condition.

2) What is the condition of the bed near the chuck? A worn bed
will allow the whole carriage to rock as it approaches the chuck
(usually the most worn area), and this could be the cause of
your problem -- or at least one cause. In particular, with the
square bed which the Atlas line used, you could also have wear
in the width of the bed, so the carriage can move forward and
back with force near the chuck (the most worn area).

I will look into this.

Do you get taper when turning close to the chuck?

Larger at the free end is likely deflection of the workpiece
(either bending or worn/sprung chuck jaws).

Yes, this is what I get, possibly related to the battered chuck.

1) What can I do to reduce/eliminate the "burring"

File when you are done. This is normal -- especially with soft
gummy steels like you are using. Get some 12L14 to see what heaven is
like. Even with 12L14, I file after cutting to clean up the crests.

That was my first choice, but the local supplier doesn't stock it. I may
pick up an aassortment next time I'm in the city (I'm a 2 hour drive
north of Toronto).

2) Any ideas why I get the rough thread, especially at the right end?

At the very end suggests deflection of the workpiece, though it
could be play in the gibs of the cross-slide or the compound. Or a
combination of them all.

I suspect you are right, possibly several things, none of which are bad
enough alone to be problem.

So -- you now have a checklist of possible causes. Someone else
may well think of something which I forgot to mention, so look at
whatever other followups appear, too.

Good Luck,
DoN.

P.S. Now that I have spent this time typing, I suspect that at
least
*one* other followup will have shown up. There were none when I
started typing.

Thank you very much for taking the time DoN. As you say, I now have a
list of possible causes to investigate. I have been "improving" this
lathe one step at a time as I find problems and learn how to deal with
them. This will be the next step.

Jon Elson wrote in
:

Other replies had much good info, but:


I set up the QC gearbox for 40 TPI, spindle for slowest speed (about
40 RPM), compound slide at 30 deg.

You might want to try threading at the highest speed you dare run at.
Since this is a very fine thread, you can probably do the threading
at several hundred RPM, at least.

I am turning to a groove at a shoulder. I am afraid that the tool will hit
the shoulder if it is too fast. I will experiment with higher speeds
though.


Right! Does it make a crunching or snapping sound when threading at
that end? If so, you may need either a tailstock center or a follow
rest to support the workpiece and keep it from climbing up over the
threading tool. Long, thin workpieces will try to do this, and you
can actually see the part jumping up and down as the threading tool
takes bites out of it. Even without the tearing, you'll never get a
proper thread when the work is flexing like that.

I think that the tailstock support is the first thing I am going to try.

Thanks for the suggestions Jon.

Rob

"Chief McGee" wrote in
news:duesc.19880$JC5.1768108@attbi_s54:

I agree. 1018 hrs is terrible to thread. But there are a few things
to try. You state that you turn a section to .500 dia.

Sorry finished part will be 3/8-40, I went to a test piece after the
trouble started.

... try going a little smaller. The book says you
can go to a minimum of .3691. Unless this is a very important part, I
would go to about .365 dia.. This will give you a flat on top of your
thread which should help with the burr.

I'll keep this in mind. I am trying to get as close to the "nominal" thread
form and size as possible.

Also use a small triangular
file to just kiss the burr. With the lathe running, hold the file so
that it is about 45 degrees to one side of the thread and let it ride
down the thread. Then hold it on the other side and let it ride to
the left again. Do this several times. Then, make one more pass with
the threading tool set at the final dimension that you used before you
used the file. This should clean up any burr you created with the
file.

I'll try that.

Thanks Chief,

Rob

"Chief McGee" wrote in
news:Lzesc.50512$gr.4957796@attbi_s52:

Also make sure the tool height is on center line.

Checked and double checked, it's as close as I can get it, and I'm pretty
picky about that.

Rob

"Greg O" wrote in
:

The lower carbon steels all cut and thread poorly. Higher carbon, to a
point, will cut cleaner, too high and it gets hard on tooling. Most
CRS cuts better than HRS. Best yet is leaded steel. The stuff cuts and
threads like butter, compared to plain 1018 HRS. Then again, choice of
material depends on the application.
Greg

Thanks Greg. I wasn't aware that the higher carbon steels would cut
cleaner.

Rob

Rob McDonald wrote:

I am turning to a groove at a shoulder. I am afraid that the tool will hit
the shoulder if it is too fast.

Does your chuck thread onto the spindle? If it does, is there a way to
prevent it coming loose or could you make such? My chuck is held to the
spindle with three bolts so I needen't fear it coming off when cutting
in reverse. Thus I place my threading tool _behind_ the work and cut
with the machine running "backwards" to the usual. The _huge_ advantage
of this is that there is zero chance of running into a shoulder. I
simply run off the end, retract the cross slide from its pre-set zero,
run back beyond the shoulder, hand move to the start, reset the cross
slide, advance the compound and take the next cut. I know it _sounds_
complicated but by the time you've done it twice it is faster than
running at such slow speeds.

Ted

After reading some of the answers to your post (and your other responses):

Point of honor: If you arbitrarily choose 80 sfm for the cutting speed of
your
1018, it yields a RPM of approx. 853 for 3/8 diameter. The stated 40 RPM is
extremely slow. Go as fast as your reflexes/skill will allow. Practice
until you
can approach 300 rpm. Your current 40 RPM translates into SFM of about 4??

Get some cutting oil, and brush on liberally for each pass. The old
fashioned
sulphur based cutting oil is quite good for single pointing.

Study the machinery handbook a bit more on thread form. A sharp vee
is not considered standard. With that in mind, and after stoning a slight
radius
on the end of your tool, it should be clear that you will achieve proper
thread
form before a sharp vee occurs on the OD. Once you have done a few threads
you will learn to gage the flat on the OD as a clue that you are almost
there.

Burrs happen when machining. Suggest removing with file or emery cloth
before reaching final thread depth. (Which you did!)

As to tool angles: When threading and using the compound rest at 30 degrees
a positive rake at right angle to the left side of the thread profile will
give best
results with the tool mounted horizontally. (for 1018) The back rake only
serves
to put everything except the tip of the tool below the center line of the
work.

As to the final pass producing roughness, it is VERY common. So before you
get
to that point, you start babying it. Extremely small infeeds when you
approach
full thread depth. Perhaps even a couple passes without any infeed at all.
(Known as spring passes)





"Rob McDonald" wrote in message
...
I hope somebody has the patience to read through this :-) I am trying to
include all the details because I don't know what I am doing wrong.


I recently tried to cut a 3/8-40 thread on a piece of 1018 HRS. First
pass was smooth. With later passes the surface seemed to get rough,

then before reaching final depth small sections of the thread tore out...
so I tried again:

I ground a new 60 degree HSS threading tool with 12 deg. relief on both
sides and 10 degrees side and back rake, and stoned the top and sides

smooth. It is mounted directly in a turret type tool post, (i.e. the tool
bit is horizontal, not sloped upward as in a rocker type tool holder).

I turned a 0.500 diameter section on a short bar. It is held in a three
jaw chuck, (no tailstock support).

I set up the threading tool on center height and perpendicular to the
surface.

I set up the QC gearbox for 40 TPI, spindle for slowest speed (about 40
RPM), compound slide at 30 deg.

First pass was just barely grazing the surface to ensure that there were
no surprises (i.e. mistakes in my setup), zeroed the collars.

I started by feeding in the compound 0.002", reducing progressively to
0.0005" for the last pass.

I measured the OD occasionally. It increased by 0.001" after about three
passes, i.e. it appears that a "burr" is being raised - is this

normal? I didn't expect it. I touched up the OD with a file before
proceeding.

I seem to be reaching the final thread form before I have cut as much as
I thought I needed from the Machinery's handbook, (0.01534" deep,
0.0177" on the compound at 30 degrees).

Finally on one pass I got a rather rough appearance to the thread at the
right hand end, although the rest of the thread still appears to be

smooth.

In case it's relevant I am doing this on a 10" Atlas lathe.

1) What can I do to reduce/eliminate the "burring"

2) Any ideas why I ge the rough thread, especially at the right end?

Rob

In article ,
Rob McDonald wrote:
Greg Menke wrote in
:

This one needs to be close fitting and smooth running so that wouldn't do
here. Besides, this is a point of honor now :-) I want to figure out what I
am doing wrong and make a good thread.

Hmm ... the needs specified above, plus the pitch makes it sound
as though you are making a micrometer thimble of some sort or other. If
you don't need the wear features of a hardenable steel (where you
ideally cut the threads oversized, harden, and then grind the threads),
and if you don't need to weld it, I would strongly suggest that you
contact one of the online metal vendors and get some 12L14. Get more
than you need -- you'll find other projects for it, and you'll love
working with it.

Good Luck,
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 ---

In article ,
Jon Elson wrote:
Other replies had much good info, but:


I set up the QC gearbox for 40 TPI, spindle for slowest speed (about 40
RPM), compound slide at 30 deg.

You might want to try threading at the highest speed you dare run at.
Since this is a very fine thread, you can probably do the threading
at several hundred RPM, at least.

Agreed -- as long as he has an adequate runout groove, so his
stopping point is not too critical. The only time that I thread without
a runout groove is on the CNC machine, where the tool automatically
retracts at the same point each pass. (I've never tried the trick of
threading to a hole, turning the spindle by hand the last turn or so.
That used to be seen on threads on old machine tools.)

[ ... ]

Tool deflection or workpiece deflection is very common in threading
operations. So, I'd expect it to take more infeed to get down to
final thread diameter. How do you measure it, with wires or triangles?
Without these special tools, measiring the true thread diameter is
almost impossible.

Agreed -- though if he has something portable enough to which he
is fitting it, that is quite possibly good enough. You can get thread
micrometers (either with permanent anvils for a single short range of
pitches, or with replaceable anvils, to cover a much wider range. The
same set of anvils works with both inch and metric (both 60 degree
threads), though you need special ones for Whitworth threads (55
degrees). As long as you stick with the same brand, you can use the
anvils from one micrometer with the other sizes. I've got 0-1" 1-2" and
2-3" Tesa (Brown & Sharp) thread micrometers sharing one set of anvils.
(All obtained in different auctions from eBay.) But they are expensive
for only a single thread.

The over-wires is the most accurate, as I can see the thread
mic's blade anvil deforming the thread if you don't use care. But
thread wires are awkward to handle -- though I have seen fixtures for
them to hold them to the micrometer anvil and spindle.

The only case when you can get the pitch diameter correct by
measuring the diameter over the crests is when adjusting a Geometric
style die head, as the thread form is complete in those.

[ ... ]

At the very end suggests deflection of the workpiece, though it
could be play in the gibs of the cross-slide or the compound. Or a
combination of them all.


Right! Does it make a crunching or snapping sound when threading at
that end? If so, you may need either a tailstock center or a follow
rest to support the workpiece and keep it from climbing up over the
threading tool. Long, thin workpieces will try to do this, and you can
actually see the part jumping up and down as the threading tool takes
bites out of it. Even without the tearing, you'll never get a proper
thread when the work is flexing like that.

Yep! He said "short" but he didn't (yet) say *how* short
relative to the diameter. The fact that he is still having problems
when going up from 3/8" to 1/2" suggests that it is either too long, or
that the chuck jaws need truing.

Enjoy,
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 ---

First off, lose the rake.
The complex geometry of the tool cutting into a curved surface, makes it
almost impossible to get a tool with rake to have the proper thread profile.
Back rake is only good for roughing out coarse threads and will need to be
followed by a finishing tool.
Side rake is only needed for course threads or very tough materials.

If you are in a situation that needs side rake, like production cutting
coarse threads, where a tool change would be non productive, or cutting
threads in copper or inconel, then do this...

Use only side rake. It should be perpendicular to the leading edge. This
way the leading edge
remains horizontal and cuts an accurate angle
on that flank of the thread. Then set your compound very precisely to 30
deg.
This way the accuracy of the trailing edge of the thread is formed
by the travel of the compound.

Either way, for 40 tpi you do not need any. Your tool should be flat.

Next, be sure that your tool has the proper clearance. The leading edge of
the tool needs more clearance than the trailing edge,
Look at the end of the tool with the cutting surface up. The junction of the
facets should appear to lean clockwise on a right hand external tool. For
left hand, it should lean counter clockwise.

I suspect this clearance is your problem. The lack of clearance causes the
tool to heel or rub against the thread before it can cut it.
It causes you to use excessive pressure because the edge of the tool cannot
cut and is instead forging the thread into the steel. Eventually you get
enough pressure, that the work rides over the tool snags it, and forces it
to cut where there is enough clearance, Usually, in the middle of the
previous thread.

Paul K. Dickman

Rob McDonald wrote in message ...
I hope somebody has the patience to read through this :-) I am trying to
include all the details because I don't know what I am doing wrong.


I recently tried to cut a 3/8-40 thread on a piece of 1018 HRS. First
pass was smooth. With later passes the surface seemed to get rough,

then before reaching final depth small sections of the thread tore out...
so I tried again:

I ground a new 60 degree HSS threading tool with 12 deg. relief on both
sides and 10 degrees side and back rake, and stoned the top and sides

smooth. It is mounted directly in a turret type tool post, (i.e. the tool
bit is horizontal, not sloped upward as in a rocker type tool holder).

I turned a 0.500 diameter section on a short bar. It is held in a three
jaw chuck, (no tailstock support).

I set up the threading tool on center height and perpendicular to the
surface.

I set up the QC gearbox for 40 TPI, spindle for slowest speed (about 40
RPM), compound slide at 30 deg.

First pass was just barely grazing the surface to ensure that there were
no surprises (i.e. mistakes in my setup), zeroed the collars.

I started by feeding in the compound 0.002", reducing progressively to
0.0005" for the last pass.

I measured the OD occasionally. It increased by 0.001" after about three
passes, i.e. it appears that a "burr" is being raised - is this

normal? I didn't expect it. I touched up the OD with a file before
proceeding.

I seem to be reaching the final thread form before I have cut as much as
I thought I needed from the Machinery's handbook, (0.01534" deep,
0.0177" on the compound at 30 degrees).

Finally on one pass I got a rather rough appearance to the thread at the
right hand end, although the rest of the thread still appears to be

smooth.

In case it's relevant I am doing this on a 10" Atlas lathe.

1) What can I do to reduce/eliminate the "burring"

2) Any ideas why I ge the rough thread, especially at the right end?

Rob

"Paul K. Dickman" wrote in
:

First off, lose the rake...

Thanks for the advice Paul

Rob



--

(DoN. Nichols)

Jon Elson
You might want to try threading at the highest speed you dare run at.

Don
Agreed -- as long as he has an adequate runout groove, so his
stopping point is not too critical. The only time that I thread without
a runout groove is on the CNC machine, where the tool automatically
retracts at the same point each pass. (I've never tried the trick of
threading to a hole, turning the spindle by hand the last turn or so.
That used to be seen on threads on old machine tools.)

Some of the old, old threads did stop on a radial hole. Done by hand, not
under power, by pulling on the flat belts, I presume.

For today's lathe I think the higher speed may produce a better finish--I think
of screw cutting in the back gears (the slowest way) more for larger threads.

If you cut to a groove, then grind your tool blank so as to use only the left
half of the end of the blank, instead of grinding the vee centered on the full
blank. This will allow the thread you form to get further up to the shoulder
of the work.

If you reduce the right end of the work to the minor diameter of the thread
also, this will give you a telltale as to when your toolpoint has reached that
diameter.
Frank Morrison

In article ,
Rob McDonald wrote:
(DoN. Nichols) wrote in
:

I accidentally mailed this (to a munged address), but I also
mailed it from a system which has no direct access to the outside world
(which I used for newsreading, among other things), so I was able to
recover the article and go back into usenet news to send it properly.

In article ,
Rob McDonald wrote:

... I recently tried to cut a 3/8-40 thread ...

1018 may not be the best choice -- and depending on where you
got it, it could be *very* bad.

I got it from a local steel supplier (Elma Steel) it could have come from
anywhere.

Yep. At least probably better than from Home Depot. :-)

I don't see you mentioning *any* lubricant

I used a cutting lubricant I had on and, but I doubt it's as good as any
of the ones you mentioned. It is time to invest in some good cutting and
threading lubricants.

O.K. The easiest to get is the pipe tapping high-sulfur oil from
Home Depot or just about any other hardware store. Molly-Dee I order
from MSC (one day delivery from them, and I seldom get off an order
smaller than $100.00 once I have decided that I'm going to call them. :-)

I ground a new 60 degree HSS threading tool with 12 deg. relief on
both sides and 10 degrees side and back rake, and stoned the top and
sides

O.K. Though ideally, there should be more relief on the
left-hand side than on the right-hand side to accommodate the helix
angle of the thread.

Good point, I hadn't thought of allowing for the helix angle.

For a 40 TPI with a 3/8" OD, I come up with only 1.22 degrees,
so your side relief should be sufficient here. With the 1/2", it is
even less.

[ ... ]

Hmm ... for 16 TPI, I start out with 0.010" per pass, and reduce
to perhaps 0.002" for the last pass or two. I also make two or three
repeats at the final depth.

Knowing that I had trouble already, and that my Atlas lathe is not very
rigid I wanted to minimize deflection/vibration.

O.K. One thing to consider, however, is that too small an
infeed results in the tip burnishing and sometimes work-hardening the
workpiece on one pass, and then digging under after one or more extra
passes.

Unless the depth of the thread is truly critical, I would check
depth of subsequent passes, and try to adjust the feed so you can take a
full depth pass (whatever works for you) for the final pass. Following
it with another pass at the same setting will burnish the finish a
little, if there was no spring to catch up to. (I'm used to my 12x24"
Clausing being rigid enough for pretty much any cut that I am willing to
risk.

I seem to be reaching the final thread form before I have cut as much
as I thought I needed from the Machinery's handbook, (0.01534" deep,
0.0177" on the compound at 30 degrees).

Hmm ... my threads program suggest the following for 40 TPI:

This value: Formed Single depth: 0.0135" corresponds to the value for an
internal thread in the handbook. I am using the value specifed for an
external thread.

That "formed" assumes that your threading tool has a tip rounded
or squared off just right to meet the spec for that thread. Mine
(except for the final column) assumes a sharp point on the threading
tool.

However, one other thing comes to mind -- how tight are the gibs
on your lathe? If they are too loose, the compound or the carriage
will rock to one side under cutting loads, thus possibly tearing out
the thread, even in the presence of adequate lubricant.

The gibs are tight, so I don't think this is the problem (but I'm going
to double check them anyway).

O.K.

The forces can also cause the tip of the tool to dip, placing it
below the centerline of the lathe.

The turret tool holder is quite rigid, and the tool is clamped very short
to minimize this.

Those both help -- though there are the various interfaces
between the carriage and the tool (cross-slide ways, pivot for the
compound, and compound ways) all contributing to give. Have you pulled
the compound out at the pivot and made sure to clean out any chips
before re-installing it? IIRC (and based on my old 6x18
Atlas/Craftsman), the Atlas design has a boss projecting from the
cross-slide, with a dovetail turned on it, and the compound has two
setscrews pushing in bronze or brass angled pushers to contact the
dovetail. The Clausing, by contrast, has a hole in the cross-slide, a
cylindrical plug on the bottom of the compound, and two holes 180
degrees apart going through the flange on the compound and T-bolts in a
circular T-slot surrounding the hole. A much more rigid mount. Since
Clausing and Atlas combined at some point (I hear stories saying that A
bought B, and others saying that B bought A), hopefully the 10" has the
more rigid design.

Also -- what size of tool stock did you use for the threading
tool? I generally go for at least 1/2" on my Clausing (where the
quick-change toolpost and holders will accept up to 5/8" shanks.)

O.K. How long is "short" compared to the diameter of the
workpiece? If there is more than 4 times the diameter sticking out of
the chuck, you will have deflection -- to an amount dependent on the
cutting forces involved.

Nowhere near 4X. Test piece is 1" diameter protruding 1-1/2" from the
chuck, the last 1" is turned down to 1/2" diameter with a groove at the
shoulder - this simulates the configuration I would be machining on the
real part.

O.K. That sounds pretty good.

I would support the end with a live center,

I'll try that. The fact that the problem is worst at the end of a
cantilevered workpiece makes me think "deflection."

And remember -- if the diameter is too small, a live center can
get in the way of the the tool and toolpost, so you may want to pick up
a half-center (actually a bit more than half) to give you more elbow
room. *That*, you will have to use with a lubricant on the center, as
there are no live half centers. :-)

The ideal lubricant for that is a lead compound, which is of
course very difficult to get these days. Older machines often had a
cavity in the tailstock holding some, with a dauber to transfer it to
the center. Lacking that, I would suggest an extra pressure lubricant
for the center -- perhaps a lanolin based case sizing lube from a store
which deals in reloading equipment.

An alternative is a follower rest.

That is on my wish list :-)

Good. Keep your eyes open.

Next -- what shape are the jaws in? A common wear pattern on

[ ... ]

A solution, if it is *just* the faces of the jaws, is to set them up
under load, and run a toolpost grinder (or even a toolpost mounted
Dremel with a grindstone) in a little at a time, until you get the
full length of the jaw faces cleaned up.

This is a definite possibility. The jaws are in lousy shape and I have
been considering grinding them as you suggest.

I presume that I don't need to mention being careful to keep the
abrasive grit from reaching the bed of the lathe. Cover with a cloth or
newspaper or aluminum foil. At a suggestion -- the newspaper wet with
oil will help to keep the grit on the paper.

[ ... ]

In case it's relevant I am doing this on a 10" Atlas lathe.

Another set of thoughts?

1) What kind of spindle bearings?

It is a babbit bearing headstock. I must admit I have had concerns here,
since it is an older lathe which is known to have spent part of it's life
in a low production environment. I lack the skills to confidently
determine it's condition.

O.K. The trick for this is:

1) Remove the chuck.

2) set up a dial indicator mounted on the headstock and measuring the
register of the spindle.

3) Take some wood dowel (broomstick is the common suggestion, if
it will fit into the spindle), and push down and pull up, noting
the change in reading of the indicator. Someone who owns a
plain bearing lathe should chip in here -- but I think that the
reading should be on the order of 0.001" deflection when dry
(e.g. after sitting overnight), and much lower when the spindle
was just being run, and thus has a good film of oil.

Lacking a wood dowel, I would consider aluminum or brass rod, so
it is unlikely to damage the spindle.

You can find web based information on pouring a new Babbitt
bearing in place, and whatever scraping may be needed.

[ ... ]

1) What can I do to reduce/eliminate the "burring"

File when you are done. This is normal -- especially with soft
gummy steels like you are using. Get some 12L14 to see what heaven is
like. Even with 12L14, I file after cutting to clean up the crests.

That was my first choice, but the local supplier doesn't stock it. I may
pick up an aassortment next time I'm in the city (I'm a 2 hour drive
north of Toronto).

Or -- use one of the on-line metals places. They cost more than
a local place -- but you don't have to get lots more than you happen to
need. Hmm ... I wonder whether MSC has any? Let's check the web site,
since that catalog is too big to use while I've got a keyboard in my
lap.

Nope -- The only 12L14 listed on their page is machinable
expanding collets, so I guess that the online places are your best bet.
Not too many industrial places stock the 12L14.

2) Any ideas why I get the rough thread, especially at the right end?

At the very end suggests deflection of the workpiece, though it
could be play in the gibs of the cross-slide or the compound. Or a
combination of them all.

I suspect you are right, possibly several things, none of which are bad
enough alone to be problem.

Which is why I listed all the possibilities that I could think of.

So -- you now have a checklist of possible causes. Someone else
may well think of something which I forgot to mention, so look at
whatever other followups appear, too.

[ ... ]

Thank you very much for taking the time DoN. As you say, I now have a
list of possible causes to investigate. I have been "improving" this
lathe one step at a time as I find problems and learn how to deal with
them. This will be the next step.

O.K. Good luck,
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 ---

--
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 ---

"Rob McDonald" wrote in message
.. .

snip

I ground a new 60 degree HSS threading tool with 12 deg. relief on both
sides and 10 degrees side and back rake, and stoned the top and sides

smooth. It is mounted directly in a turret type tool post, (i.e. the tool
bit is horizontal, not sloped upward as in a rocker type tool holder).

snip

2) Any ideas why I ge the rough thread, especially at the right end?

Rob


It is difficult to hand stone a threading tool of this size
without slightly rounding the edge on the last few thou, just where it
matters most. You will finish up with a keener edge by using the tool
as ground or, at most, topface only stoned. A really keen edge is
vital for successfull fine finishing cuts.

Feeding in at 30 deg with 10 deg side and back rake will
generate a slightly incorrect thread form although the error is pretty
small. Top rake should be at 90 deg to the LH cutting edge so that
this edge remains horizontal. Up to 10 deg rake can help particularly
when cutting coarse threads. At 40 TPI zero rake should be OK.

Unless you have overriding strength or wear resistance
requirements your problems would pretty much instantly disappear if
you changed to brass or a free cutting leaded mild steel.

Jim

(DoN. Nichols) wrote in
:

O.K. The easiest to get is the pipe tapping high-sulfur oil ...

I'll try to pick up something today.

... MSC I seldom get off an order
smaller than $100.00 once I have decided that I'm going to call them.
:-)

I feel your pain :-) For me it's BusyBee machinery and KBC tools.


... I hadn't thought of allowing for the helix angle.

For a 40 TPI with a 3/8" OD, I come up with only 1.22 degrees,
so your side relief should be sufficient here. With the 1/2", it is
even less.

It's a rather easy change to make, so I may do this anyway. Then I'll be
sure that it's not contributing to the problems.


[ ... ]

Hmm ... for 16 TPI, I start out with 0.010" per pass, and
reduce
to perhaps 0.002" for the last pass or two. I also make two or
three repeats at the final depth.

Knowing that I had trouble already, and that my Atlas lathe is not
very rigid I wanted to minimize deflection/vibration.

O.K. One thing to consider, however, is that too small an
infeed results in the tip burnishing and sometimes work-hardening the
workpiece on one pass, and then digging under after one or more extra
passes.

Unless the depth of the thread is truly critical, I would check
depth of subsequent passes, and try to adjust the feed so you can take
a full depth pass (whatever works for you) for the final pass.
Following it with another pass at the same setting will burnish the
finish a little, if there was no spring to catch up to.

You may be on to something, see my comments at the end.

(I'm used to
my 12x24" Clausing being rigid enough for pretty much any cut that I
am willing to risk.

While my experience is limited, it is mostly on much heavier equipment
than the Atlas. In school we used 12" swing Standard Modern-Lathes which
would probably be similar to your Clausing in rigidity, and from there I
went to running a 24" swing Monarch for a while before returning to
school. At the same time I am enjoying the challenge of learning to work
within the limitations of the 10" Atlas.

... there are the various interfaces
between the carriage and the tool (cross-slide ways, pivot for the
compound, and compound ways) all contributing to give. Have you
pulled the compound out at the pivot and made sure to clean out any
chips before re-installing it? IIRC (and based on my old 6x18
Atlas/Craftsman), the Atlas design has a boss projecting from the
cross-slide, with a dovetail turned on it, and the compound has two
setscrews pushing in bronze or brass angled pushers to contact the
dovetail. The Clausing, by contrast, has a hole in the cross-slide, a
cylindrical plug on the bottom of the compound, and two holes 180
degrees apart going through the flange on the compound and T-bolts in
a circular T-slot surrounding the hole. A much more rigid mount.
Since Clausing and Atlas combined at some point (I hear stories saying
that A bought B, and others saying that B bought A), hopefully the 10"
has the more rigid design.

I am not familiar with the 6" Atlas, but it sounds similar to the setup
on the 10" Atlas. It is a known weakness of the lathe.

Also -- what size of tool stock did you use for the threading
tool? I generally go for at least 1/2" on my Clausing (where the
quick-change toolpost and holders will accept up to 5/8" shanks.)

1/4" clamped as short as possible in the toolpost. It's what I had on
hand. I agree that larger would be better I among other things it would
allow me to let it project a little more.

... you may want to pick
up a half-center (actually a bit more than half) to give you more
elbow room. *That*, you will have to use with a lubricant on the
center, as there are no live half centers. :-)

The ideal lubricant for that is a lead compound, which is of
course very difficult to get these days. Older machines often had a
cavity in the tailstock holding some, with a dauber to transfer it to
the center. Lacking that, I would suggest an extra pressure lubricant
for the center -- perhaps a lanolin based case sizing lube from a
store which deals in reloading equipment.

I have the case sizing lubricant on hand. I'll add a half center to the
shopping list.


Next -- what shape are the jaws in? A common wear pattern on

[ ... ]

I presume that I don't need to mention being careful to keep the
abrasive grit from reaching the bed of the lathe. Cover with a cloth
or newspaper or aluminum foil. At a suggestion -- the newspaper wet
with oil will help to keep the grit on the paper.

OK, wetting the paper with oil sounds like a good idea.

It is a babbit bearing headstock. I must admit I have had concerns
here, since it is an older lathe which is known to have spent part of
it's life in a low production environment. I lack the skills to
confidently determine it's condition.

O.K. The trick for this is:

1) Remove the chuck.

2) set up a dial indicator mounted on the headstock and measuring
the
register of the spindle.

3) Take some wood dowel (broomstick is the common suggestion, if
it will fit into the spindle), and push down and pull up, noting
the change in reading of the indicator. Someone who owns a
plain bearing lathe should chip in here -- but I think that the
reading should be on the order of 0.001" deflection when dry
(e.g. after sitting overnight), and much lower when the spindle
was just being run, and thus has a good film of oil.

Lacking a wood dowel, I would consider aluminum or brass rod, so
it is unlikely to damage the spindle.

I guess my concern here is how hard to push. I want to find any play, but
I don't want to damage anything. A little leverage goes a long way :-)

You can find web based information on pouring a new Babbitt
bearing in place, and whatever scraping may be needed.

While it would be really interesting, it is probably more of a project
than I can undertake.

... Nope -- The only 12L14 listed on their page is machinable
expanding collets, so I guess that the online places are your best
bet. Not too many industrial places stock the 12L14.

I am in Toronto frequently, so it's not a really big deal I'll call
around the metal suppliers. I see now that I was spoiled in my youth. My
dad had a screw machine shop, and always had LOTS of 12L14 on hand in
many sizes, as well as an assortment of brass and stainless rod.

2) Any ideas why I get the rough thread, especially at the right
end?

At the very end suggests deflection of the workpiece, though it
could be play in the gibs of the cross-slide or the compound. Or a
combination of them all.

I ran a couple of trials last night:

The first attempt was the same setup as before, but at around 600 RPM. My
reactions are still adequate, but I wouldn't want try it with 16TPI :-)
There was no noticeable improvement.

Next I tried with a live center supporting the right end at 40 RPM. Due
to interference between toolpost and tailstock I had to go back to the
lantern toolpost. This improved the thread at the right end, without
making the rest any worse. Now the roughness and tearing are evenly
distributed.

I think your comment about work hardening may be the key. One would
expect to get progressively larger chips if the infeed is the same for
each pass. Instead, it was noticeably variable, as if it occasionally
"dug in" and took a larger amount on some passes. I am going to try
cutting it more agressively to see if that helps.

Rob

O.K. How long is "short" compared to the diameter of the
workpiece? If there is more than 4 times the diameter sticking out of
the chuck, you will have deflection -- to an amount dependent on the
cutting forces involved.

Where does this "4 times" rule of thumb come from? I am querying this
because deflection is much more sensitive to diameter than length. e.g.
comparing 1" diameter bar of 4" length to a .5" bar of 2" length, both
loaded with 100 lbs at the free end, the deflection is _twice_ as great
for the smaller bar. This is even worse if the deflection in proportion
to the diameter is considered.

BeamOut''(30E6,I_tube 1 .5)Beam 0 (4 100)
pos'n pt. couples shear bend. slope def'l
force stress stress
0 -100 -400 -169.8 4074 0 0
4 100 0 0 0 0.0005432 0.001449

BeamOut''(30E6,I_tube .5 .25)Beam 0 (2 100)
pos'n pt. couples shear bend. slope def'l
force stress stress
0 -100 -200 -679.1 16300 0 0
2 100 0 0 0 0.002173 0.002897

Ted

In article ,
Ted Edwards wrote:
O.K. How long is "short" compared to the diameter of the
workpiece? If there is more than 4 times the diameter sticking out of
the chuck, you will have deflection -- to an amount dependent on the
cutting forces involved.

Where does this "4 times" rule of thumb come from? I am querying this
because deflection is much more sensitive to diameter than length. e.g.
comparing 1" diameter bar of 4" length to a .5" bar of 2" length, both
loaded with 100 lbs at the free end, the deflection is _twice_ as great
for the smaller bar. This is even worse if the deflection in proportion
to the diameter is considered.

You're assuming a constant loading (100 lbs in this case). I
think that with smaller diameter workpieces, it is normal to take
lighter cuts, so the loading should scale, too.

Enjoy,
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 ---

DoN. Nichols wrote:

You're assuming a constant loading (100 lbs in this case). I
think that with smaller diameter workpieces, it is normal to take
lighter cuts, so the loading should scale, too.

Yes. This wasn't mentioned and is one of those things that anyone who
has done some machining would know but, for a newbie, it might not be
obvious.

Ted

Happy Father's Day to all the RCM and HSM folks out there to whom it
applies.

Brian Lawson,
Bothwell, Ontario.

Brian Lawson wrote in
:

Happy Father's Day to all the RCM and HSM folks out there to whom it
applies.

Brian Lawson,
Bothwell, Ontario.


Same to you Brian!
Marty

Happy Father's Day to all the RCM and HSM folks out there to whom it
applies.

Brian Lawson,
Bothwell, Ontario.
Right back at 'cha, Brian. Nice of you to mention it.
Ken.

Brian Lawson wrote:

Happy Father's Day to all the RCM and HSM folks out there to whom it
applies.

Brian Lawson,
Bothwell, Ontario.
I'll send a round of thanks out there as well and to Brian if it applies.
Martin

--
Martin Eastburn, Barbara Eastburn
@ home at Lion's Lair with our computer
NRA LOH, NRA Life
NRA Second Amendment Task Force Charter Founder

Hey guys,

A better than average looking auction coming up Saturday July 17/04
(tomorrow!!) just east of Kitchener, Ontario. Wish my budget this
month would let me go!! This place is just a few minutes north of the
401, just south-east (mostly east) of Kitchener.


http://mrjutzi.ca/2004-07-17-cat.html

Take care.

Brian Lawson,
Bothwell, Ontario