Re: [CAD_CAM_EDM_DRO] cutting speed and feed for 3/4" dovetail cutter

marble_h@... wrote:

> Can anyone tell me what the feed and cutting speed is for it
>
> I have been cutting at 160 rpm's and a feed of .002 per rev but I
> snapped the cutter ,boy $59.00 down the drain and I have 15 more cuts
> to do..

What is the diameter? How many cutting edges? What is the
tool made of (HSS, I'm guessing)? What is the workpiece material?

You first figure the correct surface speed in Feet/Minute, based on
tool and work materials. For HSS cutters on mild steel, it is about 100 SFPM.
For HSS on aluminum alloy, it is 600 or so.

Now, a dovetail cutter has a varied diameter, so you have to come up
with a compromise speed. But, using the widest diameter of the cutter
should be good. RPM = SFPM * 12 / (diameter * Pi)

For 100 SFPM with a 2" cutter, the RPM should be about 190.

Now, most dovetail cutters have a lot of cutting teeth. So, you take a
guess at chip load per tooth, multiply by number of teeth, and RPM, and
you get feed rate in inches/minute. So, for a 16-tooth cutter, and a chip
load of .002"/tooth, you get feed= .002" * 16 * 190 = 6 IPM.

Now, one thing is you should mill the center of the dovetail out as far as
you can with a standard end mill first, so the dovetail cutter only needs
to remove the material under the dovetail itself.

If you are doing this in aluminum or steel, you need to use a coolant to
keep the cutter and work cool, and flush away the chips. Cast Iron is
usually cut dry, or with a touch of cutting oil.

Jon