Re: [CAD_CAM_EDM_DRO] Cutting speeds

> Ian Wright wrote:
> >
> > Hi,
> >
> > I know this will sound like a really purile question and I'm really aiming
> > it at those who do small work on desktop machines but here goes...
> >
> > How do you decide on an appropriate feedrate for materials and cutters you
> > haven't used before? For example, say you were presented with a piece of
> > titanium sheet and asked to cut out several identical parts using, say, a
> > dental burr - how would you decide on the best feedrate to use or, at least,
> > choose one that wouldn't break the tool or dull its cutting edges? I know if
> > I'm working on my manual lathes or miller that I can adjust the speeds and
> > feeds to get optimum performance simply by using my ears and the feel of the
> > handwheels but this isn't possible with a cnc machine as you have to program
> > in a feedrate and then just hope its Ok.

First, there is an optimum cutting surface speed for combinations of
workpiece and tool materials. Generally, the harder stuff needs to
be cut at lower speeds. There are tables in all sorts of documents, from
the 1940's Atlas lathe book, to machinery's handbook, to tables published
by cutting tool manufacturers.

Once you have a surface speed for the material/tool combo, you can calculate
spindle RPM. For turning, it would be the diameter of the workpiece that
is used, for milling it would be the tool diameter. in either case,
RPM = SFPM * 12 / ( Pi * D ) where :
SFPM is the recommended surface feet per minute for the material
D is diameter in inches

Once you have RPM, you can figure out how many cutter teeth
will dig into the workpiece every revolution. (For lathes, it is
always 1.) For a 4 tooth cutter, you get 4 bites per revolution,
so at 1000 RPM you get 4000 teeth/minute.

From cutting tool info, you can figure out an acceptable feed rate,
in feed/tooth. If a particular tool has an acceptable feed of .002"/tooth
(that might be reasonable for a 1/4" end mill in aluminum) you can
feed at 8 IPM, using the above example.

To get specific, using my handy-dandy McDonnell Douglas speed and
feed calculator, pure titanium should be cut with HSS tools (not recommended)
at 100-125 SFPM, or with carbide at 225-250 SFPM. They recommend
end milling with .006"/tooth on a 1" end mill, and multiply this by tool
diameter for smaller ones. So, a 1/8" cutter should be fed at .00075"
per tooth. Work hardening will make this impractical, so you might do better
with less depth of cut, and a lot more feed.

For a 1/8" diameter carbide cutter, you will need to turn the tool at
about 1000 RPM, and you can calculate the feed per tooth depending
on the number of teeth on it (which is sometimes real hard to determine
on the little rounded burrs).

Jon