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
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
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
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?
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...
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
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.)
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.
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.
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?
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
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)?
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 touch up the OD with a file after *finishing* the thread. No
point until then.
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.
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
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.
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.
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. :-)
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.
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
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.
Other replies had much good info, but:
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.
Definitely, the burr is normal.
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
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.
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.
email@example.com (DoN. Nichols) wrote in
I got it from a local steel supplier (Elma Steel) it could have come from
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
Good point, I hadn't thought of allowing for the helix angle.
Test piece after the initial failure.
Knowing that I had trouble already, and that my Atlas lathe is not very
rigid I wanted to minimize deflection/vibration.
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
The gibs are tight, so I don't think this is the problem (but I'm going
to double check them anyway).
The turret tool holder is quite rigid, and the tool is clamped very short
to minimize this.
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
I'll try that. The fact that the problem is worst at the end of a
cantilevered workpiece makes me think "deflection."
That is on my wish list :-)
This is a definite possibility. The jaws are in lousy shape and I have
been considering grinding them as you suggest.
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.
Thanks for the suggestion.
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.
I will look into this.
Yes, this is what I get, possibly related to the battered chuck.
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).
I suspect you are right, possibly several things, none of which are bad
enough alone to be problem.
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
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
I think that the tailstock support is the first thing I am going to try.
Thanks for the suggestions Jon.
"Chief McGee" wrote in
Sorry finished part will be 3/8-40, I went to a test piece after the
I'll keep this in mind. I am trying to get as close to the "nominal" thread
form and size as possible.
I'll try that.
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.
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
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
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
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
on the end of your tool, it should be clear that you will achieve proper
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
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
results with the tool mounted horizontally. (for 1018) The back rake only
to put everything except the tip of the tool below the center line of the
As to the final pass producing roughness, it is VERY common. So before you
to that point, you start babying it. Extremely small infeeds when you
full thread depth. Perhaps even a couple passes without any infeed at all.
(Known as spring passes)
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.
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.)
[ ... ]
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.
[ ... ]
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.