Assuming the general ~3" diameter gear cutter, and assuming you are
making gears of relatively mild stuff, then about 150 RPM and about 5
IPM feed. But, just calculate it very much like an end mill.
Water-base cutting fluid should be fine.
DoN's admonition above is well put; form cutters and slitting saws are
run much slower than run-of-the-mill cutters. I would start with 1/4
to 1/2 of the speed as determined by classic means. Let's see: 4xCS/
dia=4x80/3=106rpm. (assuming low carbon steel work piece) I would
start off with 30 rpm for a 3" dia. cutter.
As these cutters are quite robust one can use a fairly aggressive chip-
per-tooth feed. How much depends on the surface finish required,
horse power of the spindle, and rigidity of the set-up. I'd try .004"
to .006" chip per tooth. Assuming a 12 tooth cutter the feed in
inches per minute becomes 12x.004x30=1.44" say 1.5 inches per minute.
Too low a feed increases cutter wear.
For cutting steel a sulphurized cutting oil is best when using form
cutters. For a one-off any good cutting oil would suffice.
Let us know what you decide and how it worked out for you.
Well ... first I would need to know what metal you will be
cutting. The cutter alone does not define the speeds. (And if you want
RPM, we'll need the diameter of the cutter.)
As for the feed -- we would also need to know the number of
teeth on the cutter -- feed is usually specified as feed per tooth, so
the more teeth the faster the total feed you can get away with.
You can look these up in _Machinery's Handbook_ -- which is
where I would go to calculate these once I knew the specifics of the
workpiece material and the number of teeth.
Or -- if "some gears" does not translate to enough to make time
consumed particularly important, I would aim for perhaps 50 to 70% of
the maximum speed, and perhaps as low as 50% of the calculated feed.
Those speeds and feeds are for a company turning out the maximum number
of pieces in a day, considering the tradeoffs between the number of
minutes per piece and the time lost to changing tooling. With the
recommended speeds and feeds, it is *assumed* that you are willing to
sacrifice some tool life for more parts in a day.
Perhaps the ideal (for such a factory) would be speeds and feeds
which would call for replacing the cutter once a day -- at the change of
shifts. For your own tools this is probably not optimum, unless someone
is paying you to make a lot of these.
I would run about 60 surface feet per minute (sfm) and use either water
based coolant or a mister with coolant in it. You could run faster but
it will save the tool to run at 60 sfm. You could also use sulfur oil
and either mist or paint it on the cutter. The final decision of speed
comes from looking at the color of the chips and how much heat you are
generating, all revelent on the sharpness of the tool, the type of
coolant and the sfm of the cutter. To get the most life out of the tool
you want the chips to come off shiny with no discoloration and the
coolant not steaming from the heat.
John, thanks. I will try to hook up the rotary indexer to my CNC mill
tonight, so that I can do the entire job automatically without needing
to press the button on the indexer. The mill itself would
electronically "press the button".
If I do that, I do not particularly care of the job takes 10 minutes
or 30 minutes due to too conservative setting of the feed. I can just
start the job and go home to do something else. Plus, I have to worry
less about rigidity.
I would say, I will start at 80 RPM or so. at 3 inches diameter, it
gives me 62 FPM.
Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here.
All logos and trade names are the property of their respective owners.