In article ,
Jacek Zagaja jzagaja-at-poczta.onet.pl wrote:
Hi there Don 
Yes - terminology through communication is what I need far away. So I
should use cutter not the 'knife' for turning tools right?
"Cutter" or "Turning tool" or "lathe tool" all would work.
"Knife" implies a kind of cutting not normally found on a lathe.
Actually, "threading tool" applies specifically to what you are using.
I'm
studying Materials Engineering and turning is my temporary hobby that
allow me to realize some projects. For example integral spheres for
photometrical measurements.
Hmm ... for that, perhaps spinning of thin sheet metal, instead
of machining. Make two pieces (one with an access hole and one without)
joined at the "equator" (if you were talking about the planet instead of
a man-made sphere.)
2H13 is an old Polish label. Now we use European but they are not
intuitive for me so far. Do you know any site that deals with US.
Alloys nomenclature?
I'm sure that such exist, but what I currently use are two
books. One is _Machinery's Handbook_ (pretty much any recent edition),
and one is an older Jorgensen steel catalog. Since both are in English,
they may be hard for you to find. I don't know how available
English-language technical books from outside the country may be.
The carbide inserts are the only usable. Maybe ceramics can be right
too. There's something weird with turning speed for threads. Let
consider pafana.pl carbide inserts. Average turning speed for
stainless steel is 100 m/min. Now having 42 diameter I should set my
machine to:
n = 1000*Vc/pi*D = (1000*100)/(3.14*42) = 758 [turn/min]
This is some speed!
It is rather fast, given your need to cut a short thread, and
the lack of clearance. One thing which might help would be to turn the
tool upside down (adjusting to set the height of the point correctly)
and to cut in reverse, so you cut away from the shoulder. However, I
don't see provisions for a "runout groove" (where the metal is cut away
completely, to provide a space where the tool's motion can be stopped
(or in this case started) without messing up the thread which you are
cutting. Can you introduce such a groove into your design? It will
make the job a *lot* easier.
Stopping the machine will cost some time Oh BTW
how you name this small distance (synonym is paddock) where you must
set your cutter and turn on machine. This distance has smaller
diameter than thread.
I think that this must be the runout groove which I mentioned
before.
Note that you should not need to start and stop the lathe
spindle if you have a runout groove to place the threading tool in to
start, and a threading dial which will allow you to close the half-nuts
at the same reference point each time. (With metric threads, I
understand that the threading dial has a sliding gear with four
different sizes to engage the leadscrew, depending on the particular
thread to be cut. I've not had to work with this style before.
Anyway, with the spindle turning, you crank the point of the
threading tool (the one which you have illustrated would be for
threading towards the shoulder right-side up, you would need a different
one for the upside-down threading, given how little clearance you have.
(Note that I am not accustomed to using the brazed (silver soldered)
tooling, but rather the style with the removable inserts, where a
special pocket exists on the tool shank, and a clamp to hold the insert
in place. These are cheaper to replace inserts on, but what you have is
probably cheaper in initial purchase price.
Anyway -- you move the threading tool into the groove, and set
it to a very shallow first cut, lubricate the workpiece (I would
probably use "Molly-Dee" a molybdimum disulfide based cutting oil for
this, but I don't know what you have available. Once it is in to the
desired depth, wait for a mark to line up with the index on the
threading dial, and note which one you use (probably should just use the
'1' mark -- at the speed and pitch you are working with, the mark will
come around fairly quickly. Then, just as the '1' mark approaches the
index mark, quickly close the half-nut lever. This will start the
thread cutting -- hopefully away from the shoulder if the gear setting
is right, and the spindle is running backwards. Once it clears the end
of the thread, pull back up on the lever to disengage the feed. Then
crank the cross-slide back enough to clear the workpiece, and crank the
tip of the tool back to the runout groove. Then crank the tip back in
to the previous depth, and (just this once) stop there, and re-engage
the half-nuts lever as before. The tip should travel in the same groove
you just cut, without removing much (if any) metal. This is helping you
to be sure that the thread dial is at the right setting.
Once that is proven, crank the tip back out again, and move it
back to the runout groove. Then crank it in and go just a little
deeper. (I won't suggest absolute depths, as you will have to find out
what works with your material and your tool. However, as a starting
point, try 0.10 mm. It is a bit shallower increment than I would use at
the start of the cut, but not much. (I would normally be working in
inches, not mm, though I sometimes work in mm.) As you get deeper, you
need to make the increment a bit less, as you are removing more material
per cut. The final cut, you should repeat at the same depth a couple of
times, which will produce a smoother thread. Then take a file and clean
up the crests of the threads.
Note that US practice while threading usually has the compound
set to feed almost along one flank of the thread, taking most of the cut
off the other side. A common setting is 29.5 degrees, though 29 degrees
will work as well. With this technique, you bring the cross-slide back
in to the same depth and then add a bit more feed using the compound
each time. This means that you will have to correct the compound's feed
for the angle to get the right depth -- but you should also have some
way to measure the thread depth directly -- thread wires and a
micrometer, or if you have access to one, a thread depth micrometer with
the right anvils for you 1.0 mm thread pitch.
Normally, the angle of the compound is to feed it in and a bit
towards the headstock side. With the reversed spindle you would use the
same -- or with no reversal, you would need to shift it to the other
side. Apparently, UK practice is to just feed in square, which would
give you a little less to worry about, but which might not produce as
good a thread. Certainly, cutting towards the shoulder would require a
lot faster reflexes if you want to get the maximum speed out of the
carbide tooling.
Note that the size of the lathe, and the rigidity and power will
determine whether you can use carbide tooling to get a better
finish. Your "2H13" appears to be one of the European steel
designations, and I am not familiar with it. But 13% Cr would
probably make that a rather tough steel. Perhaps Ed Huntress could
pop up with a close equivalent in US steel grades?
My lathe is rather powerful enough (1800 turns/min)
Speed is only one point. There is also the power of the motor.
I am used to it being expressed in HP (horsepower), but European motors
tend to express it in KW instead. My motor is 1-1/2 HP, which should be
somewhere around 1.2 KW or so.
and my spindle
handle 100 mm rollers. Take a look:
http://tme.szczecin.pl/~jacek/Myslov...alworking.html
Hmm ... I see the brazed (silver-soldered) carbide threading
tool. I was sort of expecting the lathe, instead.
Now -- if you really *have* to cut to the shoulder and not have
a runout groove, what I would suggest using for the machine would be a
CNC lathe -- as that can cut and withdraw the tool at precisely the same
point each time, so the end of the thread just lifts out of the groove.
2H13 can be toughened so that 60-70 HRC is possible but I don't think
it was toughened. I can check with Vickers hardness test after cutting
my work. The surface is struggled because of hard shavings fall (I
don't know if 'fall' is good here, maybe flow down or something).
I'm not quite sure what you mean by "fall" above.
However, one consideration, even if the material starts out
annealed (maximum soft state), it may work harden -- and I suspect that
a steel with that much chromium will do so. This may require you to
make deeper threading cuts than I would otherwise like to make.
It may even be that it would be better to grind the threads instead
of to try to cut them -- but this will require a rather expensive
setup.
Yes however in my city, a common pitch is 1.2 and I need 1.0 with 42
diameter (mm). Also the length of thread is small - max. 5 mm.
So -- at most 5 complete threads, and probably less. Certainly
less if you make a runout groove.
Are you doing this as a hobby, or are you in a commercial machine
shop? The tools which would be standard in such a commercial shop
are less likely to be found in a home shop for hobby use.
As I wrote this is a hobby for University purpose. Imagine that we
have Technology Hall. They have digital lathes from Sandvik but they
"digital lathes" are probably what I would call "CNC lathes".
"CNC" stands for "Computer Numerical Control" in English.
don't know how to cut thread with good surface for right price. It is
also some relation problem. I did ask first can the chief do it for
me. He told me he doesn't have a time and went away to a tools room. I
did ask another guy. He shook his head. Now all the peoples (it was
vacation time) staying and looking at my work. It looks like (I can't
put drawings on my server for a while):
------------------
| |
| 70mm dia ---- |
|---------- | | |
| | /xxxx | | A |
---------------- |--------------------- ---- |
| ^ | |-
| | -----------------------|-|
- lathe mount | |42mm dia B | |
(spindle) | | ---------------------- |-|
| | | |-
---------------- |--------------------- -----|
| | \xxxx | | A |
|---------- | | |
^ | -----|
| | |
cut it here ------------------
xxxx - is an area of thread (42mm dia and 1 mm pitch). As you see the
diameters is 70 vs. 42 so the side (flange) is a problem for them
The want the thread to be reversed. That is technologically logical. I
told them I didn't have right cutter to perform A notch and what is
important to have absolute match (on axis) of thread with B opening.
The chief who is really nervous threw some insults at me that if I am
wise then I can do it myself and polishing will be to expensive for me
and went away again. As you see I'm trying did as he said
O.K. Are you using a live center on the tailstock to support
the free end of the workpiece? That would reduce chatter (vibration of
the workpiece as you cut). I *think* that 'B' is supposed to be a hole,
though it appears to stick out a bit. Is the 'A' part a circular
groove? If so, is the inner diameter of that the same as the 42 mm of
the other end? If that is the case, and if the part does not need to
resist lots of twisting force, I would think that it would be easier to
start with a workpiece just big enough to cut the threads on the OD, and
turn the 42 mm parts on each end. Them make the 70 mm diameter piece
with a hole just slightly below 42 mm (perhaps 41.94 or so) and heat the
70mm diameter piece to expand the hole, and slide it onto the other part
after the threading is completed. It will quickly shrink and become
close to immovable -- how much depends on the actual sizes of the shaft
and the hole.
Anyway -- looking at other ways to make something (sometimes of
two or three pieces, instead of just one) might make it easier to make.
As an indication of the sizes of lathes, Mine is an old Clausing
which will swing 12" (300 mm) diameter over the bed, and somewhat
smaller (at least 6" (150 mm) over the carriage. I consider this on
the large end of hobby lathes, though there are others here with
larger machines. Mine is sufficiently rigid to be happy with carbide
tooling and reasonably tough jobs.
I would say the same instead of threads
Carbide tools can give a smoother surface to the cut, but they often
require higher speeds and more rigidity from the lathe than
equivalent HSS tooling can. Carbon steel requires *much* slower
speeds or the tool overheats and looses its temper.
That is so. I will try to use ready thread cutter (carbide soldered to
the grip) and grind it so that it can be used with that flange.
When grinding carbide tooling (you will need something better
than the typical bench grinder), you should wear a breathing mask to
keep the dust out of your lungs. It can be bad after a time.
It is really late now (about 2:30 AM), and I am going off to
bed. I hope to get back to your next message before it is quite this
late -- but I will be at a long meeting tomorrow evening, so I may not
make it back in time.
I hope that this has been some help.
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 ---