Re: Thumb Calibration

Reed, the rpm probably is a little high for dry cutting, but the feed
is right in line with what you'd normally use on a half inch end mill.
It's about .002 per tooth. At your 400 rpm with 4 flutes, a .002
feed per tooth would work out to 3.2 ipm. At .9 ipm, the cutter is
making almost 3 times as many cuts per inch as it needs to, and the
life of the edge is highly dependent on how many times that edge makes
a cut. Also, the very thin chip has little ability to carry heat away
from the cut. As Fred said, the scale on HR is also somewhat akin to
dragging the cutter up the driveway. When cutting with the end of an
endmill, the instant the corner is no longer sharp, the cutting
ability of the tool is gone. Any dull area quickly generates heat
which softens the adjacent edges and dulls them which generates even
more heat which.....you get the picture. If you were to get rid of
the scale and run about 600 rpm at 5 ipm, with some cutting (not
lubricating) oil laid down in the path of the cut, the life should be
pretty good. Generally speeds and feeds are based on about 45
minutes actual cutting time. You could make your 30 inch cut in 6
minutes at 5 ipm, so, as you can see, at the right speeds and feeds
you can do quite a bit of cutting before the tool requires sharpening.

--- In CAD_CAM_EDM_DRO@yahoogroups.com, "reed_irion" <Reed_Irion@h...>
wrote:

> Have you tried these speeds and feeds ? I'm really suprised. 7.6 ipm
> seems really agressive. But then again I have no frame of reference.
> Haven't I heard something about the chip carrying away most of the
> heat at higher speeds and feeds ?
>
> Maybe some of the participants could just throw out some specific
> instances of speeds and feeds vs. material when using smaller mills?
> Like minimills?
>
>
> --- In CAD_CAM_EDM_DRO@yahoogroups.com, Steven Ciciora
> <sciciora@A...> wrote:
> > I am no machinist, but sort of like when I was a kid and wanted to
> be a
> > rock star, I pretend I'm one on the weekends.
> >
> > I use ME Consultant 2.0 to calculate my speeds and feeds.
> While "Hot
> > rolled mild steel" was not listed as an option, when I
> chose "Steel - Low
> > carbon (1020)" and plugged in the .5" 4 flute hss end mill, 0.1"
> deep, 0.5"
> > width of cut, it returned 821 RPM, 7.6 ipm, 0.474 HP. For this
> material,
> > it uses 107.5 sfpm. The program does a lot more, but I mainly use
> it for
> > speeds and feeds. I also bought kwiktrig, but when I just tried to
> run it,
> > the executable seemed to have disappeared, and when I re-installed
> it, it
> > told me the eval time limit has expired :-(
> >
> > A google search should turn up places to download these programs.
> >
> > Good luck,
> >
> > - Steven Ciciora
> >
> > At 05:32 PM 7/12/2004 +0000, you wrote:
> > >I am trying to get an idea of rules of thumb for speed and feeds
> > >that work.
> > >
> > >This weekend I was milling my first few parts with EMC and I
> noticed
> > >that the cutters dont fare quite as well as they did when I was
> > >doing it by hand.
> > >
> > >I made a .1" deep cut in hot rolled mild steel at .9 ipm for about
> > >30 inches. The HSS tool died quite suddenly from overheating, with
> > >no gradual degradation. It was working fine with little smoke from
> > >the cutting oil then- poof, blue chips burned cutter... The
> machine
> > >has a 2 HP motor and was running about 400 rpm.
> > >
> > >Should I switch to carbide ? I never liked them because I chip
> them
> > >easily, but the EMC is much more patient than me so maybe this wont
> > >be a problem. How much improvement will I get from carbide ? Will
> > >the flood coolant system make a big difference ?
> > >
> > >What are other users experiences with speed/feeds in various
> > >materials ?