Feed Rate question for tapered bits

[Darryl Kerney]

I have the Amana 46282-K 1/16" tapered and just ordered the 46280-K 1/32" tapered as well, 1/4" shank,
my question is, so i am clear on it, are the feed rates they say 1x on the chart for the diameter, meaning a 1/4" deep cut ?
IF SO, does that mean you can go quite a bit faster if only cutting 1mm on a finishing pass that's left over from the roughing machining allowance ?

[adze_cnc]

The Amana product page lists:

• tool diameter: 1/16"
• shank diameter: 1/4"

The PDF file lists: Tool Reference #: 46282-K 1/16" Dia

It would be logical to presume that for the tool diameter in the 1xD, 2xD, etc. that they are not referencing the "shank diameter".

[Darryl Kerney]

OK thanks, i was a bit unsure about that but it makes sense now.

[Darryl Kerney]

As for part 2 of my question, 1/16" = 1.5875mm,
so for a 1mm cut on a finishing pass is it ok to go faster ?
i have been and it seems to be ok but will that wear out the bit faster and reduce quality much ?

[Rcnewcomb]

Going too slow will wear out the bit faster.

From CNC Cookbook:

In the diagram, the cutter edge radius centerline travels along the yellow lines. If the radius is too large relative to the depth of cut (bottom), all the force goes to pushing the chip under the edge. This is the “rubbing” effect you’ll hear talked about when feed rate and hence chip load are too low. Tool manufacturers will tell you that too little feed is just as bad for tool life as too much feed (or too much spindle rpm).
Below a certain level, chips will not form and the cutter will “plow” across the workpiece causing plastic deformation and considerable heat. If you’re cutting much less than the cutting edge radius, you’re rubbing and not making clean chips. That will heat the tool and material and drastically reduce tool life.

[Darryl Kerney]

Thanks !

[chemstock]

The cut is made at the rotating velocity of the tool tip, larger bits for the same RPM have faster tool tip speeds.In turn, these tools can support higher chip loads.
small diameter tools have considerably lower tool tip velocities and as a consequence lower chip loads. Going faster places a sideload on the bit that ultimately cause it to break. Quite common since I buy my 1/8" tools in packages of 10 but buy my 1/2" tools as a single.

For the tapered bit, the chip load should be based on the smallest diameter. The taper allows for a higher side load and the larger sections of the taper will easily make the cut. The base of the taper will have the lowest tip speed and will not be able to support the same chip load as further up.. As mentioned below, going too slow will cause heat build up since the chip load also provides cooling for the tool. The happy medium will depend on the wood you are milling. If we were to label soft maple as "1" for cutting speed, seasoned white oak would be about "1/3 to 1/2", soft woods would be about "2". The caution about softwoods is that the the tool can embed since the fiber is yielding elastically at the tool tip. This will cause a bit breakage, a stall in the spindle or (worse) a stall on the stepper motors on the CNC. Seems counter intuitive but it is more important to have sharp tools for softwoods

I also have to reduce the cutting speed (and RPM) for extended length bits, The side load will cause vibration and ultimate tool failure.

All theory aside, I run the cutting speed up to the point where the tool breaks, and the back off about 15%. Do that a few times and you will know what your setup can handle. Be aware, bits that break can cause shrapnel that fly all over the shop.