What's new
What's new

Process of figuring feeds and speed??

stephon0913

Plastic
Joined
Aug 12, 2011
Location
Portland, OR
Hello all
i have never been taught a "proper" way of finding speeds and feeds when programming for a part. I usually take an educated guess and go from there. I just want to ask is there a process that other programmers go thru to figure these numbers. Im trying to take the time and setup my mastercam tool library with all accurate info so i dont have to change them everytime and potentially something go wrong. Any advice is more than welcome.
 
Be a machinist instead of just a "programmer"? Not to be a smart ass, but it takes experience to know what to set feeds and speeds at..... sure, you can go to any insert makers books and see that this or that insert is supposed to run at 487 sfpm in 4130 and the feed per tooth or per rev is supposed to be such and such.....

But that is all variable, radius size on the insert, surface finish requirement, rigidity of not only the part, the work holding, but also the machine. Available hp makes a difference, is it in a 40 taper machine, 50 taper, 8000 pound lathe or 20,000 pound lathe.

Way too many variable to say anything specific with any authority... although... I suppose we could say 200 sfpm and .003" per tooth feedrate and the rest of us will always beat you on a quote..... :D
 
There is no "proper" way as far as I know.

A classic engineering answer: it all depends.

If you are always machining parts that are similar and have similar materials, shapes, and tools; life is pretty easy. That is rarely the case. I always go to the manufacturer. This is a reason to use tools from a good source with plentiful information. A Kennametal catalog has about 75 pages of info on speed, feed, best practices, chip thinning, insert failure, etc.

I'm almost always working with cast aluminum.

Turning, keep it under 4000 SFM, .015/rev .3 depth (on diamter) to rough, .010/rev .06 (on diameter) to finish.

Drilling with solid carbide, 700 SFM .0125/rev. Maybe peck after 3X depth.

Insert drill, 1000 SFM and .007/rev.

Face mill, 2500 SFM .006/tooth. Any deeper than .15 at 75% step over and they start to sing.

End mill, 1500 SFM .008/tooth. When it breaks, you went too deep.

Then there is the fun stuff. SAE port tools usually run about 25% of what they recommend or they chatter. PCD throws out all the rules of SFM. Most of the time you can run max spindle RPM.

Those numbers run pretty well for us. When we get iron or steel, we have to go back to fundamentals to figure feeds and speeds.
 
Maybe Im missing something here, if I understand the question correctly the answer if easy. RPM = cutting speed x 3.82 / Dia of cutter, or the part on a lathe. IPM is #of teeth x RPM x feed per tooth. I do also like to refer to the manufacturers recomedations as well. I love how sandvik puts it right on the insert box. I have never been fond of the cam system generating my feeds and speeds, to many variables.
 
Last edited:
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.
 
Last edited:
Re: sfriedberg's post:

1 - Highlight all
2 - CTRL-C
3 - open word doc or other text editor
4 - CTRL-V
5 - Save as "how to do speeds and feeds"
6 - Print
7 - Tape to wall near machine.
8 - Tape to wall of bathroom.

Great post - thanks for taking the time to spell all that out, in a succinct, easy to read manner.

Brent
 
I wish I got this speech as an apprentice!
Good stuff.

But I have one correction. SurfaceSpeed can be too slow and be harmfull.
If you are too slow built up edge will occur, especially in sticky materials, and result in poor tool life.

I've shown up to a shop running in Inconel. Told them to double SurfaceSpeed and tool life increased by 12x!
 








 
Back
Top