Formula for in horizontal milling

The cutting force depends on the geometry of the cutting tool. Which I would say is available from the tool manufacture. There are other factors involve as to how fast you feed the material through. Most tool manufactures have a list of feeds and speeds on their products.

The formula to use is :

F_t = K(hp_c)/[N(C_rpm)(W)(H)]

where:

F_t = feed per tooth (chip thickness), inches [also called cpt]

K = machinability factor, in³/min/hp_c [for aluminum use 2.5 - 4.0]

hp_c = horsepower available at the cutter [80 - 90% of motor rating]

C_rpm = rotation of the cutter, rpm

W = width of cut, inches

H = depth of cut, inches

................... and

N = number of cutter teeth

Hi, Guest!

That's beautiful. The OP is trying to determine the rpm. So do we isolate the C_rpm and rework the equation to solve for that?

Mark

Hi, Guest!

What does "Feed Per Tooth" refer to?

Mark

The easiest explanation is - the thickness of chip material that each cutting edge of a tool removes with one pass.

A generic value for aluminum is 0.011"

thanks i think that formula should work ill give it a try........

Are you talking about a key for a lock or a key for locking a pulley or gear onto a shaft?

The surface feet per minute (sfm) for aluminum ranges from 365 to 735 for high speed steel cutters and 835 to 1355 for carbide cutters. The formula for calculating rpm is

RPM=(sfmx3.82)/diameter.

Equally important is your feed per tooth or feed per flute in the case of endmills. That formula is:

inches per minute/ (number of teeth x rpm)

How much feed per tooth you can get way with depends upon the geometry of the cutter. If it is a very small diameter say less than 3/13" or a fine tooth slitting saw I try not to exceed .001 per tooth. If you are milling with a carbide insert facemill with polished inserts and agressive geometry you might get to .003-.004" per tooth. You will not burn up a cutter with aluminum, but you can go so fast that the aluminum melts and loads up your cutter. Too much chip load (feed per tooth ) will also cause cutter breakage. If the cutter chatters or makes a screaming sound then you are probably spining it too fast or feeding it too slow.

As with any machining setup you should remember baisic machining rules the first of which is always clean. Then come sharp, rigid, square, concentric, correct feeds and speeds, correct cutter geometry, and proper lubrication. If something is not comming out right, go back to these baisic rules and you will most likely find the answer.

As for forces, I don't know how to calculate them, but most manual milling machines have motors ranging from 3/4 up to 3 HP.

The rpm is limited by the surface feet per minute the cutter can withstand in the given material. This is primarily dependent on the material of the cutter. With variation of 10x or better.

Power is determined by cubic inches per minute cut. More or less.

Choose or find out the cutter type. Get help if need to find out what SFM or SMM if metric it will withstand. Compute circumference. Determine RPM. Estimate feed. The cutting heads snap off on this type cutter if over loaded so keep it light about 0.001 per tooth. unless you can use carbide inserts on a fly-cutter head then consult the manufacturer for specs on feed.

If you can design the system so the cutter is below the work and the chips fall free it will work about twice as well as if the cutter is above the work.

If you can get hold of a Machinery Handbook you can find more detailed information.

If you don't mind my asking, where did you study engineering?

You will need variable speeds if you are planning to use different mill cutter diameters.

Aluminum cuts comfortably at 900 R.P.M. using a Ø.500" cutter with a lubricative coolant. Ø.250" should run between 1200-1600 R.P.M. if you have good chip removal (air or high coolant pressure). The slowest speed you will probably ever use (for very large diameter keyway or channel cutters aking BIG chips would probably be 300 R.P.M.

p.s. Feed rate of material into the cutter should be capable of adjustment as well.