[Dakmotron]

I've been browsing around the web for a while now trying to get some kind of solid answer about SFM but I can't seem to find it. From what I've read so far:

Lets say I'm machining Aluminum that has a diameter of .500. I've read so many different things but one of the charts I've seen for SFM says it should be 150-400. So lets say...400 that would mean my max rpm would be 3200? But what if I'm cutting something that .202 in dia. it says my max rpm shoud be ....7920?

I just need someone to explain to me how deciding feed rates and sfm actually works...I've really been learning on the fly and have been getting by making parts that are ok...but I know they can be better.

Thanks for any help.

[fizzissist]

Good news. We can fix this.

SFM means Surface Feet per Minute. In the case of a lathe, it would refer to the largest dia being machined. In the case of a milling machine, it would refer to the portion of the cutter with the largest diameter.

Let's say we're talking about a 1/2"dia endmill, High Speed Steel (HSS), going to machine a chunk of aluminum. The book says 150-400 SFM.
Instead of trying to remember or look up a formula right now, think of the concept. You can always go back to the concept and derive the formula!

How many feet is the edge of that tool, the circumference of that .5"dia endmill, going to traverse at say, 200SFM?
Multiply the dia x pi, and you get 1.5708 inches. Divided by 12 that's .1309 feet. Ok, so how many revolutions to get .1309ft go 200ft in a minute?
I get 1,529 revolutions per minute. ..... So a 1/2" endmill at 200SFM would run at 1529RPM.
.... A piece of 1/2"dia aluminum in the lathe would rotate at....<drum roll> .... 1529RPM.

Now, the chip load? For a 1/2"dia HSS endmill with 4 flutes in aluminum you might want to cut .003" per flute in your mill. How fast should you feed the machine?
Well, ya got the RPM set, and there's 4 edges, so 4 x .003 = .012" per revolution. RPM x feed per revolution gives you the Inches Per Minute (IPM). Here, it's 1529 x .012", and that's 18.35IPM feed rate.

If you go to a proper carbide 2fl endmill, and you've got the horsepower and rigidity, spin that puppy up to 2500SFM and you're in the range of 20,000RPM and 200IPM.... That's what the big boys can run.

Next, what SFM to use? Depends on the tool you're using and the material you're cutting, how you're using it, and what type of operation. That's a different lesson...

[dcoupar]

It sounds like you're talking turning. If your part is 0.500 or 0.202, or even 10", program G96 (Constant Surface Speed) S400 (400 SFM), and let the control take care of the proper RPM for that SFM.
You may want to precede that with a G50 Snnnn to limit the RPM as the tool approaches center.

[Machineit]

To be real simple and basic, SFM which should be SFPM (Surface Feet Per Minute), it is the relationship of the cutting tool to the surface of the material being cut.

In a mill where the tool turns and the material is stationary, it is the speed that the surface of the endmill move or turns. This remains constant and the same no matter what area of you part you are working on, a small hole in the center to an outside diameter of 1 foot, because the tool is the part that is turning. On a 1/2" diameter endmill, the surface will move approximately 1.57 inches or .1308 feet in one revolution. One of the only times you might change the speed is like a small or deep hole where you can't get the coolant in as well and you reduce the speed to reduce the change of over heating the tool or work piece.

On a lathe the work piece or material turns and the tool is basically still or only changes position but not speed. Therefore, most of the time the surface speed changes as the tool moves in and out or around the material. If you take a .05" cut down the surface of a 3 inch bar the surface speed will be determined by the 3" diameter. If you do another pass down that same material at .05" deep, the surface speed will be based on the remaining 2.950" diameter. If you do a face cut on that material it will start out as SFM at 3" and as you go to the center of the part where the SFM is theoretically zero (so very high RPM). Therefore, the work piece will be constantly increasing in RPM all the way to the center. As "dcoupar" said, most lathes are programmed with CSS (constant surface speed) where the control increases the spindle speed as the tool moves closer to the center of the part.

The SFM is of course different for almost every material that you machine (Aluminum, Brass, Cast Iron, Steel, Stainless Steel, Inconel and on and on) and changes for the different tools that you use, IE. Steel, High Speed Steel, Cobalt, Carbide, Ceramic, etc. That is where the real challenge comes in and why there are so many charts to help you figure it all out.

Unfortunately the best information you can possess is experience, and that is what you do hot have. Starting in manual machining is the best way to start learning, but seldom happens these days. If the CAM program can't figure it out, that's the end.

Too low a RPM or SFM and the tool will chip or break and/or you will not be productive at removing enough material per minute of shop time. Speed is power when you talk about tools or pretty much anything else. Take a piece of straw (the grass kind) and in a tornado it can be sped up enough to penetrate a tree several inches. Now, try to slowly push that straw into the tree, it will never happen. The same applies to tools. If you normally would take a .02" cut with a carbide lathe tool at 300 SFPM fine, but turn that tool into the part .02" and try to slowly turn the part to make that cut, you will break the tip off of the tool. You need the speed.

On the other side, too high a speed will cause damage to the tools too. The ability of the tool and material to dissipate the heat of the friction of the cutting will be overcome and the tool will usually burn or melt. Once this occurs, cutting stops and breakage and tool seizing happens. We have all seen that endmill stuck in the material, or that drill the seized and will be part of that material forever more.

Unfortunately, most charts and graphs are not as helpful as you would like. Your example of 150 to 400 for the aluminum shows this. 150 SFPM or over 2 1/2 times faster than that at 400 SFPM. Wow, that's helpful! But, that is life and they are depending on your experience, machine type, rigidity, available coolant type (or none), etc..

Have fun learning and use common sense as you learn. Usually best to start at the lower number then change as you see how it machines. Remember also that machining everything at the absolute maximum RPM and CHIP LOAD is for production runs where small amounts of time add up to a lot of time over thousands of parts. If you are making one or two parts and you push it too far or fast and break a tool or mess up a part, that is usually a money looser. Just pushing that drill too hard once and causing you to ruin a part and have to take time to change tools costs money. Finish your part and save that tool for another job.

Have fun------Mike

[fizzissist]

... I keep forgetting....
Spend all this time and effort trying to offer genuine help to someone, and don't even get an acknowledgment that it's been read.

[Machineit]

... I keep forgetting....
Spend all this time and effort trying to offer genuine help to someone, and don't even get an acknowledgment that it's been read.

+1

Yeah, so frustrating isn't it. Man! (chair) But, once in a while you do get a person who is glad for the help and says so.

I mean, I didn't really have anything to do for the two hours it took me to figure out how to phrase what I wanted to say so that someone who knew nothing might be able to understand it!

I was being sarcastic if it was not obvious. I also have a business to run!


Mike

[newman55598]

I'm new to this and appreciate all the info that is on these forums and the people willing to share their experience as most people will not help with those tips and tricks that they spent a lifetime learning just to broadcast it to the public. Thanks again

[fizzissist]

newman55598..... You just made some good points with us. A little appreciation can go a long way!

[Machineit]

+1