SFM?

[classictom]

Could someone explain SFM to me? Is it the same as IPM? I am new to milling and would like to start using proper feeds and speed instaed of guessing.

Thanks
Tom

[laka]

SFM and IPM are different.

SFM (SFPM) is Surface Feet per Minute = Distance in feet the cutting edge (or workpiece on lathe) travels in one minute. Since a tool on a mill is rotating, you have to do some calculations to convert this linear measurement, into circular equivalant.

IPM is calculated from SFM, RPM, and chipload.

RPM = (SFM x 3.82)
-------------
Cutter (or workpiece) diameter

IPM = (RPM x Chipload per flute x # of flutes)


ie: 1/2" 3 Flute endmill - 350 SFM - 0.003" chipload per flute

RPM (S) = 2674
IPM (F) = 24.066

If you were to roll the 1/2" diameter tool down a hill at 2674 RPM, in one minute it would have travelled 350 Feet down the hill. Circumference (1.57" x 2674RPM = 4198" = 350 Feet)

When I was first learning, I would grab a Kennametal catalogue and look at all the formulas in the back. I found that it helped me get my head around it. I still use these formulas everyday.

You should never need to guess a SFM, every tool supplier usually will list their recommended SFM's for their products for different materials. You will notice that softer materials will have a higher SFM, and harder materials will have a lower SFM.

hope this helps

[Eurisko]

Well said.
Here's another example:

Let's say you want to drill a .500 inch diameter hole in an aluminum alloy using a high speed steel drill.

According to the reference manuals, a HSS drill should be able to handle 200 SFM in this alloy.

RPM = (SFM x 12) / (pi x drill diameter)

= (200 x 12) / (3.14 x .500)

= 1528

Another reference tells us that the proper feedrate for a .500 diameter drill in this material is .008 inches per revolution (IPR).

Multiplying our RPM (1528) x IPR (.008) gives us a feedrate of 12.2 inches per minute (IPM).