

SFM Formula?
When I first went to a local trade school, and we were figuring SFM for drilling, we were taught the formula sfm=4xcutting speed dividedby tool dia.. I've been doing cnc milling for now 10 yrs. and always had a programmer with the exception of one shop. today, my programmer gave me a different formula thats sfm x 2.82 (ithink) x tool dia. which one is right. i found that if i tried to figure 100sfm in cast iron using a .120 (#31)twist dr. @.0025ipr i get a different result using each. and then me and said programmer got into a little tift about his speed and feed of the .120 drill. he had prog. for 325rpm @ 1ipm. seemed way tooooooooooooooooooooooooo slooooooooowww to me, so i gave his little formula a try and came up with about 3200rpm @ 8ipm. the said i was crazy. i tried it any way, and whuddya know, 4 hole, .3 dp @ about 1 min as opposed to his way @ about 4mins. i figured his sfm to be about 12. again, which one is right?
jts

SFM does not equal RPM.
The Revolutions Per Minute formula is correct, but not for Surface Feet per Minute as you say:
4 x Cutting Speed / work diameter = RPM. (IIRC, 4 is just an approximation used for Pi)
SFM is close to the formula your programmer gives, but is actually:
diameter x .2618 x RPM = SFM

RPM = sfmX 4/diameter of cutter
The actual value for the constant 4 is 12/ Pi or 3.8197.
The other formula is pretty close and easier to use.

Originally Posted by Arthur.Marks
SFM does not equal RPM.
Actually, there is ONE case where SFM=RPM. When the diameter (of part or tool) is 3.82".

I have heard of both but I personally use 3.82 x SFM / D

The formula in the Titex book (I think that's where I got it?) uses 3.8

Think Snow Eh!
Ox


SFM Formula
I developed and used the simplified formula for teaching RPM for cutters since the earliest days of CNC, its
SFM times 4, divided by the tool diameter.
Its not quite accurate, the 4 should be 3.82, but it gets you so close, and it is easy to do in your head.
A .5" drill in Mild Steel, using 100 SFM= 100 times 4, divided by .5= 800 RPM.
In those days I worked for Swedish Machine Tool and we manufactured a 50 HP CNC lathe with a 10 step gearbox, it had no G96, so we had to figure the closest RPM for each cut.
My job was to install the machine and teach the customer to make their first part or two.
I learned in a hurry that I better develop a lot of easy to remember shortcuts and this was one of them.
So is the info on my "Simplified Math for CNC" DVD, nobody in any of the shops I trained, had any idea how to figure angles, radiusangle tangent points, etc.
"Keep it as simple as possible" and good luck: Heinz.
www.doccnc.com

3.82 x CS ft/min
 = RPM
D in
UNITS of measure ...
you have to convert inches of tool dia to inches traveled in one revolution
pi times the tool dia in inches gives you the total inches traveled in one rev
but your still using inches....so....
then to change the tools diameter to feet ....divide it by 12...
Now remember how to divide fractions?... invert and multiply? right???
So you left with 12 divided by pi... how much is that ??... 3.82 and change
But as Heinz and others have pointed out... 4 is close enough

thnx for all your help guys, i realized i made a few mistakes like the rpm thing and it was 3.82 not 2.82 . thnx again for the info.
JTS

Actually, this made me look up something I've been wondering for a long while... what about Metric formulas?
318.3 * CS / Diameter = RPM
That is, where Cutting Speed is expressed in surface meters per minute and the Diameter is expressed in millimeters. Surprisingly, though, my Machinery's Handbook v28 has only surface feet per minute charts for materials. I realize I could convert them, but...
Is there a Metric edition of Machinery's Handbook??

SFM = ( RPM x DIA ) / 3.82
RPM = ( SFM x 3.82 ) / DIA

Now how about feed rate of end mills and drills? sorry for hijacking the tread but this seems like the logical next step in the post.

Originally Posted by zach123
Now how about feed rate of end mills and drills? sorry for hijacking the tread but this seems like the logical next step in the post.
Go until your snap it off and then back off just a touch.


I went to trade school in the 80s
We were taught 4*cs/dia=RPM
wher cs = cutting speed in SFM and
dia = tool (or part in a lathe) diameter in inches.
I get 5% more productivity using 4 vs 3.82
Joe

Originally Posted by zach123
Now how about feed rate of end mills and drills? sorry for hijacking the tread but this seems like the logical next step in the post.
Depends on the size of the cutters. Larger cutters can feed faster.
Endmills
Solid carbide endmills for steel, +/ 30%:
1/4": 0.001 IPT (inches per tooth)
3/8": 0.0015 IPT
1/2": 0.002 IPT
Solid carbide endmills for aluminum:
1/4": 0.003 IPT
3/8": 0.005 IPT
1/2": 0.006 IPT
Converting IPT into IPM (inches per minute):
IPM = RPM * IPT * Z (number of flutes)
Drills
HSS: ~100SFM for steel, 200300SFM for aluminum
Cobalt: +25% over HSS
Feed:
1/8": 0.003 IPR (inches per revolution)
1/4": 0.007 IPR
3/8": 0.010 IPR
1/2": 0.013 IPR
5/8": 0.016 IPR
3/4": 0.019 IPR
IPM = RPM * IPR
Since the vast majority of drills are 2 flute, we use IPR instead of IPT.
These are general guidelines, YMMV.
Sol
Glacern Machine Tools

I use the 3.82 formula, and when I double check it against a lathe job that's running in SFM, it comes out perfectly at all diameters.
But I can't figure out why the 3.82 is correct, when it seems to me it should be PI.

Originally Posted by Dave K
I use the 3.82 formula, and when I double check it against a lathe job that's running in SFM, it comes out perfectly at all diameters.
But I can't figure out why the 3.82 is correct, when it seems to me it should be PI.
3.82 = 12/pi

Originally Posted by 706jim
3.82 = 12/pi
Ok, I see mathematically this is correct, but I still don't understand why this wouldn't be correct?
SFM X Pi/ diam. = RPM.
Posting Permissions
 You may not post new threads
 You may not post replies
 You may not post attachments
 You may not edit your posts

Forum Rules

Bookmarks