Hi Chris..

Here is something I developed in the early Ninety's.

Maybe it will help you get a better grip on what you are working with.

WHAT FEED RATE...?

Manufacturers of cutting tools make charts and cardboard slide
rules that are supposed to tell us what feeds and speeds to use
when milling various materials. It appears most of this
information is derived from lathe work and is rehashed for use on
the milling machine. The cutting process of milling is about ten
times more complex than turning. So I find this approach less
than adequate.

The intermittent cutting, the various chip thickness as the tooth
enters and leaves the work, the changing tool geometry created as
the tool and the work both move together independently, the
different manufacturers cutter geometries which may work
marginally well in some materials and "Oh boy!" in others, and
the cutter buried in the cut creating a "fire" the coolant has a
tough time reaching are all factors which make milling feeds and
speeds a difficult puzzle to solve.

The recommended milling speeds and feeds distributed by various
sources are basically inconsistent; unless one data chart is a
duplicate of another. I also think some of this data was
documented when railroads were still using steam engines.

What's the answer?

First of all, we are talking about end milling and drilling with
standard high speed steel and solid carbide cutting tools.

Secondly, we are talking about what the tool itself can handle,
not the setup or how husky the machine is. The setup should be
rigid and the machine should be beefy enough to "work" the tool
without causing noticeable vibration.

We can use the recommended surface cutting speeds for the
different materials; but not without forethought. When figuring
RPM stay on the light side if the cut is deep. Proper coolant
flow may not be available to carry away the heat, so the tool
will "give up" prematurely. Remember, the recommended cutting
speed is used to determine the highest production RPM with the
tool on the outside of the work and drowning in lots of coolant.
There is no slowest speed.

The RPM is figured by multiplying 4 times the Cutting Speed
divided by the Tool Diameter. The 4 is approximately equal to
12" divided by 'Pi'. This is necessary so inches can be converted
to feet and diameter to circumference.

RPM = 4 x Cutting Speed / Tool Diameter

The Feed Rate in Inches per Minute of a rotating tool is figured
by taking the Chip Load per Tooth, times the Number of Teeth in
the cutter, times the spindle RPM.

Feed Rate = Chip Load per Tooth x Number of Teeth x RPM

These two formulas have been around a long time; and they work in
conjunction with each other. The RPM is easy to figure, you have
the Cutting Speed and the Cutter Diameter; so with a little math,
Presto! You can figure the Feed Rate because you know the RPM,
Number of Teeth in the cutter and the Chip Load per Tooth.

Wait just a minute! What about Chip Load per Tooth ?

Chip load per tooth and accurate feed rates are what this article
is all about.

Premise one

Cutting tools of different diameters from the same manufacturer
and of the same series have the same geometry and therefore look
the same under various powers of magnification. An 1/8th inch
end mill magnified 4 times looks just like a 1/2 inch end mill.

Premise two

A smooth piece of material doesn't look any different to a 1/16th
inch diameter tool than it does to a 5/8 inch diameter tool.
Therefore we can look at one tool diameter as being a percentage
of another tool diameter.

So lets play the percentages.

There are three basic conditions in end milling. The slotting
cut where 100% of the tool diameter is cutting and the trough
left behind affords limited chip flow. The roughing cut where
the tool is only using 65% of its diameter and has an open side
for sufficient chip removal (65% is chosen to make the overlap at
the right angle corners during successive side passes). And the
finish cut which takes 3% of the tool diameter or less.

During slotting, the tool sees the highest cutting force as it is
removing maximum material, therefore it works best at about
2/3rds the roughing cut feed rate. This important fact allows us
to increase a pocket-clearing feed rate by 50% except for the
initial slotting cut which would be programmed as usual. This
makes a nice production increase when spiraling a pocket inside
out; because we are not "locked" into the slower feed rate of the
initial "slotting" cut.

A given end mill diameter has an optimum "metal-peeling"
strength. The factors which try to overcome this strength
include, material toughness, percentage of end mill diameter
cutting, and depth of cut. Additional tool length reduces this
strength a lot; so keep it stubby.

An end mill's Depth of Cut should be figured as a percentage of
its diameter. Depth of Cut for all tool diameters will then be
easy to figure. Tool depth for pocket clearing in brass and
aluminum works well between 1/2 to 2/3rds end mill diameter.
Steel is tougher so use 1/4 to 1/3 end mill diameter. This
constraint is imposed by the initial "slotting" cut.

Well here we are at chip load per tooth. So how do we figure it
for different tools?

Empirically! Drive the tool, what ever size it is, to it's
maximum comfortable productive limit. Then write down this data:
feed rate, number of teeth in the cutter, rpm, and tool diameter.

We can now figure a Feed Index Number.

FIN = Tool Diameter x RPM x Number of Teeth / Feed Rate

Divide a different tool diameter by the Feed Index Number and we
immediately have the Chip Load per Tooth for that tool. This
assumes of course, we are working in the same material under
similar cutting conditions.


Each of the three basic cuts has its own Index Number. The
Slotting number is related to the Roughing number by a factor of
2/3rds; and the Finishing number can be adjusted to suit surface
finish. The Feed Index Numbers we use for 6061 aluminum and 360
brass a Slotting, 117; Roughing, 84; Finishing, 70. These
numbers are quite productive; but still allow us to run a tool
all night long and have finished parts when we come in the next
morning. For slotting with a 1/16th inch (.0625) end mill we
divide .0625 by 117 to yield a .00053 chip load per tooth. This
times 2 teeth times 3000 rpm equals 3.2 inches per minute feed
rate. For roughing use Index number 84 to reach a feed rate of
4.5 inches per minute. Roughing with a 1/2 inch end mill at 2000
rpm and 3 flutes we figure 36 inches per minute.

The feed rate formula now reads:

Feed Rate = RPM x Number of Teeth x Tool Diameter / Feed Index
Number

This concept works for drilling too. You can eliminate the number
of teeth from the formula if two flute drills are all you use.

FINDrill = Tool Diameter x RPM / Feed RateDrill

Feed RateDrill = RPM x Tool Diameter / FINDrill

This approach allows you, as a specialist in your own shop, to
develop feed rates based on the brands of cutting tools and types
of material you work with.

Advantages of this system include: more productive feed rates with
unfamiliar tool diameters, ease of programming actual feed rates,
fewer broken tools, and realistic feed rates for quoting jobs.

A corollary situation developed while drilling. We noticed in
drilling aluminum and brass at our popular RPM of 3000, we could
use the decimal size of the drill and multiply it by 100 to
figure the feed rate in inches per minute. Therefore a 1/8th
inch drill who's decimal diameter equals 0.125" would be
programmed at a feed rate of 12.5 inches per minute. This also
worked for drill diameters up and down the decimal chart.
Naturally if the RPM of 3000 is to fast for the application then
lower the feed rate in the same proportion as the RPM.
Copyright STAN DORNFELD 1989

Feed Rate Corollary

Assuming there is enough RPM available, theoretically speaking,
different diameter end mills will be fed at the same rate.
Here's how:

Material 316 SST with a surface speed of 50 feet per minute. The
end mill is a .75 diameter three flute.
Four times the cutting speed divided by the tool diameter gives
266 RPM. The end mill diameter divided by the index number, 117,
gives a chip load per tooth of, .0064,



Depth of cut depends on material toughness and the ability of an
end mill to eject chips.

Stanley Dornfeld

"Chris S" wrote in message
om...
Hi everyone, I am currently a student and my teacher hasn't been able
to give me a real direct answer and everyone I ask just gives me what
DOC they use but I want to find out how to get the DOC.

Basically I was taking to deep of cuts and keeping the feed rate high
which I realized was wrong. So I am basically trying to find a formula
or a log or something that will help me determine a DOC.

For example I am cutting 6061-T6 Aluminum at using a 1/4 4 Flute
endmill with a FPM of 75 and a DOC of 0.025" and a Spindle Speed of
6000 since that is when the machine max's out. I understand where the
RPM, IPM, and FPM comes from and how to calculate them. I just have no
idea where the DOC comes from. So if anyone could explain it or give
me a formula it will greatly be appreciated.