[Paul_S]

Ether a 2 or 3 flute end mill can be used in aluminum. Steel it would be better to use the 3 flute.

It is important to know what surface speed you are going to use with the cutter. This is dependant on the material being cut and the material of the cutter.

Aluminm using a High Speed Steel (HSS) end mill will use typically a surface feet per minute (SFPM) from about 400 to 800. This is used to calculate your spindle revolutions per minute (RPM.)

Carbide cutters in aluminum would use 800 and up SFPM.

Steel will depend on a number of factors. Type of steel, and hardness. For an example: 303 CRES (corrosion resistant steel) using a HSS end mill, typically 70-110 SFPM. Carbide end mill would be 110-225 SFPM.

Surface feet per minute affects tool life the most. So use the lower end for rough cuts and the higher end for finishing.

Your feed rate is dependant on inches per flute of your end mill. And chip size if it is ether too small or too large will also reduce your tool life, second to spindle speed.

There are tables for material and end mill type of inches per flute and chip size or chip load.

And easy way to estimate chip load is to use an index value. For example: .010 per flute for a 1 inch dia two flue end mill in aluminum. .003-.004 per flute for a 1 inch dia 3 flute end mill in a steel.

So if we use a 1/2 cutter in steel. .003 x .5 = .0015. And using 70 surface feet per minute. The RPM = 12 x SFPM / (PI x dia) so given 70 SFPM the RPM calculates to about 535 RPM. The feed wil be in IPM = RPM x number of flutes x IPT, so given 535 RPM and 3 flutes at .0015 per flute the IPM calculates to 2.4 inches per minute.

For cuts less than the full width of the cuter increase the roughing feed IPM x square root (tool dia / width of cut)

It is generally recommended, not to exceed 60% or 75% the width of the cutter. So say, 60% width to cutter dia, the 2.4 IPM calculation is corrected to 3.1 IPM (3.09 = 2.4 * sqrt( .5 / .3) )

The faster you can remove the materal the better. But not too fast. Calculate your cubic inches per minute. CIPM = width x depth x IPM.

1. typically in steel, your width of cut and depth of cut should not be more than dia of the cutter squared (dia x dia.)

2. Know the horse power (hp) limits of your spindle of your machine tool. The material will have a CIPM/hp rating. Or sometimes given as unit hp/CIPM.

Aluminum is typical from 2.5 - 6 CIPM/hp or .4 to .17 unit hp.

303 is .7 for CIPM/hp or 1.4 unit hp.

You need to check your calculated CIPM divided by CIPM/ph (or times the material unit hp) to find the hp requirment. It should be less than what is available at the spindle at a given RPM.
This so not to overload your spindle and cause tool breakage and worse yet, machine damage.

Finishing feed rates would be done faster. And depending on whether the finish cut is an end cut or a peripheral side cut. And a finish feed rate is what will give you the required finish.

And end cut will typically be slower by 1/4 to 1/5 feed to a peripheral cut. A 32 roughness average finish will be 50% the feed of a 125 roughness averge finish for a peripheral cut or a end cut with a ground radii. Otherwise 32 roughness average will be 25% the 125 roughness averge (Ra.)

To calcalute a 125 Ra finish use an index of .0405 * square root of the dia. And the feed is NOT per flute but by inches per revolution for peripheral finish cuts. So at 535 RPM using a 1/2 dia cutter feed for a 125 Ra finish calculates to 5.3 IPM (inches per minute.)

For 125 Ra finish the index value of .0405 x sqr(tool dia) * RPM
For 63 Ra finish the index value of .0287 x sqr(tool dia) * RPM
For 32 Ra finish the index vaule of .0205 x sqr(tool dia) * RPM

To correct for a RMS (root mean square) finishes:

For 125 RMS finish the index value of .0382 x sqr(tool dia) * RPM
For 63 RMS finish the index value of .0271 x sqr(tool dia) * RPM
For 32 RMS finish the index vaule of .0193 x sqr(tool dia) * RPM

RPM = SFPM * 3.82 / tool dia inches
SFPM = RPM * tool dia / 3.82
IPM = IPT * number of flutes * RPM
IPT = index chip load * tool dia * sqr( tool dia / cut width)
cut width =< tool dia