If you don't want to understand it and just want the numbers, use one of the calculators already mentioned.
If you want to understand it, this is covered in all the decent training books (like Moltrecht's
Machine Shop Practice). Here's one way to do it,
from scratch. To those outside the US, I apologize for the imperial units.
First, you need to know the target cutter surface speed in feet/minute. This is primarily a property of your cutter material and workpiece material, and you can look it up in hundreds of places (!). 100 SFM is a good starting point for HSS in steel. 300 SFM is a good starting point for carbide in steel. 1000 SFM is a good starting point for carbide in aluminum. If you have any doubts, you can
look it up. And if your machine can't go that fast, you can almost always go slower! Call this quantity
CS.
Second, you need to know how many teeth your cutter has. Basically, how many bites will the cutter take each revolution. Call this
T. You also need to know the diameter and width of your cutter Call these
D and
W. These are all things you can measure on your cutter.
Third, you need to make an estimate for chip load, or bite size, per tooth. 0.001 to 0.003 is a good starting point. Go small for delicate cutters or ones with little chip clearance space. Go large for coarse tooth cutters and soft materials. Call this
CL.
Fourth, you need to know how much HP your machine has at the spindle. Call this
HP.
Fifth, you need to know the power factor for the workpiece material. This is how many cubic inches of material can be removed per minute, per horsepower. 1 is a good starting point for steel. 2 is a good starting point for cast iron. 3 is a good starting point for aluminum. (You can look up these power factors, too, but the tables aren't on every bathroom wall the way the cutting speed tables are.) Call this quantity
PF.
From these seven quantities, you will now compute spindle speed, feed speed, and depth of cut
in that order.
Spindle speed
SS in RPM: CS = SS * D/12 * pi. Therefore SS = CS / (D/12 * pi).
Explanation: You know how fast (CS) you want the edge of the cutter to go. That is directly related to the size of the cutter (D) and the speed it spins at (SS) by grade school geometry. The factor of 12 converts from inches to feet.
Example: Target surface speed of 100 SFM, cutter diameter of 4 inches. Spindle RPM is 100 / (4/12 * 3.1416) = 95 RPM. Your machine probably doesn't have that speed. Pick the closest available speed. If in doubt, go lower.
Let's try a different example: Target surface speed of 1000 SFM, cutter diameter of 0.5 inches. Spindle RPM is 1000 / (0.5/12 * 3.1416) = 7600 RPM.
Feed speed
FS in inches per minute: FS = CL * T * SS.
Explanation: The cutter is taking (T) bites every revolution, and it revolves (SS) times a minute. To make the desired chip load (CL), the cutter must advance that far on every bite.
Example: Spindle RPM is 100, chip load target is 0.001, cutter has 12 teeth. Feed is 0.001 * 12 * 100 = 1.2 inches per minute. Your machine probably doesn't have that speed. Pick the closest available speed. If in doubt, go lower.
Let's try a different example: Spindle RPM is 500, chip load target is 0.005, cutter has 6 teeth. This would be typical of coarse aluminum cutters. Feed is 0.005 * 6 * 500 = 15 inches per minute. Can your machine feed 1/4" every second? If not, go lower.
Depth of cut
DOC in inches: HP * PF = FS * W * DOC. Therefore, DOC = (HP * PF) / (FS * W).
Explanation: Your machine cannot remove more than HP * PF cubic inches of material per minute. Every minute the cutter is covering an area FS by W. The maximum DOC is the third dimension to the volume the cutter removes every minute.
Example: Feed speed is 1.2 inches per minute, the cutter is 0.5 inches wide. You have a 5 HP machine, and you are cutting steel so the PF is 1. DOC = (5 * 1) / (1.2 * 0.5) = 8.3 inches.
THAT is why horizontal milling machines can rip the doors off a Bridgeport. Can you sink a 1/2" endmill 8 inches deep in steel on a turret mill? No, you cannot. Neither the machine nor the endmill will stand up to it. They don't make 1/2" endmills with 8" flutes for good reason! You're not going to find many 21"+ diameter horizontal milling cutters, either, and you won't find them on puny 5HP mills. So we won't be cutting 8.3" deep. But in this example, you can sink a typical 4" to 8" horizontal cutter all the way to the arbor (about 1" to 3") without maxing out the potential DOC.
Let's try another example: Feed speed is 1.2 inches per minute, the cutter is 6 inches wide. You have a 5 HP machine, and you are cutting steel so the PF is 1. DOC = (5 * 1) / (1.2 * 6) = 0.7 inches. That's not a 6" diameter flycutter; that's a slab cutter cutting chips a full 6" wide.
Important:
- SS too fast means CS too fast, which will burn your cutter. SS too slow is less productive, but not harmful.
- CL too big may break your cutter. CL too small may rub rather than cut, burn your cutter and/or work harden the material. Therefore, you can't push FS too high or too low.
- If your machine or cutter is loose or flexible, you can't get close to the potential PF. Reduce DOC to avoid breaking your machine or cutter.
- Same consideration applies to delicate workpieces. You may have to reduce DOC to 10% or even less of the potential value.
- Your machine may have less than rated HP at low SS. Antique gearbox machines don't have that problem. Modern invertor machines often do.