Turning and finishing a mirror finish on mild steel
Jim Stewart
IC engine and I've not been able to get the
quality of finish that I'd like.
The flywheels are about 1" thick and 4" in
diameter. I was working on the face of one
last night. The problem is the small digs
the cutting tool occasionally makes. I can
polish out the overall surface to a mirror
finish with successively finer grades of
sandpaper, but I cannot remove the digs with
the coarsest grade of sandpaper I have.
Can anyone suggest a tool shape and feed that
might give me a better finish. My tool is
slightly rounded with the recommmended angles
for steel.
Robert Swinney
Are you sure the marks are dings and not chatter marks? I'd bet chatter.
Try running your lathe at "dead slow" to reduce chatter. Try to keep
sandpaper away from your lathe also.
Bob Swinney
"Jim Stewart" <jste...@jkmicro.com> wrote in message
news:3dGdnXqpz_b...@omsoft.com...
Roy
edge, and it comes from the material your cutting building up opn the
cutting tools edge., Its known to drag or make marks in an overall
good looking finish randomly. Try using a diamond hone to polish up
your cutting tools edge a bit, and make it more slick. that sometimes
helps a great deal....You can get them at Wal MArt in the sporting
good section for under $6.00 or so.....
--
\\\|///
( @ @ )
-----------oOOo(_)oOOo---------------
oooO
---------( )----Oooo----------------
\ ( ( )
\_) ) /
(_/
The original frugal ponder ! Koi-ahoi mates....
Harold and Susan Vordos
Jim,
You're experiencing the "joy" of machining what must be mild steel, or low
carbon steel. Without the addition of an element for free machining, that's
the nature of the stuff. The only way you can get around the tearing is
to take a cut that is deep enough, and also run fast enough. That requires
the use of carbide, and depth may have to be more than .025" in order for
the material to machine without tearing. Surface finish then comes out with
a high luster instead of a dull appearance. The alternative is to run
with high speed, fair amount of positive rake, with the cut well lubricated,
and accept the finish that you get, polishing progressively after machining
until you've removed the intermittent tearing that occurs.
If you want to avoid this condition, use other materials. The materials
available for production machines avoid that problem by the addition of lead
or other elements, or in the case of stressproof, the material undergoes
considerable cold working, improving its properties immeasurably. It
generally machines without tearing.
For free machining, you can choose from several alloys of mild steel----some
of which are 12L14, 1213,1215,1117, &11L17. Stressproof, while free
machining, has a higher carbon content and can be heat treated. It would
not be classified as a mild steel as a result, but a medium carbon steel.
If, by chance, your flywheel is cast gray iron, there has to be a problem
with your tool geometry. It's not known for tearing, due to the nature of
the material.
Harold
Jim Stewart
Yup, it's mild steel. I thought it was a good deal
at $.60/lb, but maybe not now...
The frustrating thing is that the tool will cut
beautifully for maybe a tenth of an inch and then
for no reason dig in. I was hoping that there was
some magical tool geometry that might help.
I don't think I can take a .025" cut and hold the
tolerance that I want, but I will do some tests
on a piece of scrap. I will also play with a greater
positive rake and diamond stoning the tool.
Thanks for the advise.
Chuck Sherwood
>>>might give me a better finish. My tool is
>>>slightly rounded with the recommmended angles
>>>for steel.
I have the best luck with very sharp HSS toolbits,
good cutting oil to prevent a buildup on the toolbit nose
and a slow cutting speed of about 50.
One time I used a carbide toobit at high speed
with smoking hot chips and I got a almost chrome looking
finish. I never could duplicate it though!
I have the same problem sometimes with CI flywheels
but not as bad as with crummy steel. I use very
coarse emery paper (80-100) to get the marks out
followed by finer grits to get the finish. It might
not be a prefect surface anymore but it doesn't matter
for a flywheel.
Fred R
>
> The frustrating thing is that the tool will cut
> beautifully for maybe a tenth of an inch and then
> for no reason dig in. I was hoping that there was
> some magical tool geometry that might help.
>
> I don't think I can take a .025" cut and hold the
> tolerance that I want, but I will do some tests
> on a piece of scrap. I will also play with a greater
> positive rake and diamond stoning the tool.
>
What Harold and Chuck said, plus I'll repeat some advice I got here when
I was having a similar problem: do all the dances to the Rigidity God,
(Make sure you are facing the direction for the intended type of
Rigidity or you'll get distracted from machining.)
including minimum tool/holder overhang, snugged gibs, lock unneeded
slides. Made all the difference for me.
--
Fred R
"It doesn't really take all kinds; there just *are* all kinds".
Drop TROU to email.
Mike Henry
I had a similar problem turning some smaller CRS stock with a HSS bit and it
was suggested to take a deeper cut using a bit with about a 1/32" radius on
the tip. That worked much better for me.
Harold and Susan Vordos
"Mike Henry" <Michae...@msn.com> wrote in message
news:dreo4...@news4.newsguy.com...
Yep. There's a minimum amount that you can take without tearing, and it's
far more than one generally takes for finish cuts, especially if you're
working to tight tolerance. Once you go below that minimum, tearing is
guaranteed with mild steel. It's the nature of the critter, and always has
been. When you work to tight tolerances you learn to turn oversized by a
half thou, then polish for size and finish. 'Or, if you're fortunate to be
so equipped, you leave .010"/.015" and grind. Unlike many other materials
(aluminum, most of the copper alloys, even stainless steel), you can't take
light cuts with any success when machining mild steel, not on a lathe.
Strangely, it mills quite nicely with end mills cutting on the periphery.
Harold.
David Billington
in Wichita about 1981. Whenever you took a cut on the outside of the
piece you always ended up with what looked like scratches running
parallel to the axis of the piece. The lecturers hadn't seen it before
and they were time served machinists, it turned out to be inclusions in
the round HRS bar which had been drawn out in the rolling process. Crap
bar I guess, I had not seen this problem again until a couple of weeks
ago when I was grinding some HRS angle, it showed the same symptoms.
Ace
removal for finished size.
Guess that was to sort of allow for what you are referring to, plus HRS has
a lot of size variations, etc.
"David Billington" <d...@djbillington.freeserve.co.uk> wrote in message
news:43DB763D...@djbillington.freeserve.co.uk...
Jim Stewart
> I'm turning 2 flywheels for a working model
> IC engine and I've not been able to get the
> quality of finish that I'd like.
I received an email from a reader who suggested
grinding a tool to take a shear cut. The way
mine ended up is like a small roughing tool
with high rake angles laid on it's side.
I was able to take .005" cuts and get a beautiful
finish. I also tightend up the gibs and locked
the axis that I wasn't using. I used a slow
speed and feed, trying to make sure that I didn't
heat things up and work-harden the stock.
Thanks all for the useful suggestions.
Yermother
--
For full context, visit https://www.polytechforum.com/metalworking/turning-and-finishing-a-mirror-finish-on-mild-steel-471022-.htm