Page 1 of 2 12 LastLast
Results 1 to 20 of 29

Thread: SFM Formula?

  1. #1
    OKKHM1250 MAN is offline Plastic
    Join Date
    Feb 2010
    Location
    Buffalo'ish
    Posts
    9

    Default 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

  2. #2
    Arthur.Marks is offline Stainless
    Join Date
    Nov 2008
    Location
    Chicago, IL
    Posts
    1,524

    Default

    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

  3. #3
    706jim is offline Stainless
    Join Date
    Jun 2006
    Location
    Thunder Bay Canada
    Posts
    1,251

    Default

    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.

  4. #4
    metaltech is offline Hot Rolled
    Join Date
    Feb 2007
    Location
    midcoast U.S.A.
    Posts
    930

    Default

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

  5. #5
    evansmachine is offline Cast Iron
    Join Date
    Dec 2007
    Location
    Monmouth, OR
    Posts
    347

    Default

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

  6. #6
    Ox's Avatar
    Ox
    Ox is online now Diamond
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    17,793

    Default

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



    -----------

    Think Snow Eh!
    Ox

  7. #7
    Arthur.Marks is offline Stainless
    Join Date
    Nov 2008
    Location
    Chicago, IL
    Posts
    1,524

    Default

    Quote Originally Posted by metaltech View Post
    Actually, there is ONE case where SFM=RPM. When the diameter (of part or tool) is 3.82".
    Learn something new everyday! haha

  8. #8
    Heinz R. Putz is offline Hot Rolled
    Join Date
    Mar 2006
    Location
    Columbus, Ohio
    Posts
    907

    Default 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, radius-angle tangent points, etc.
    "Keep it as simple as possible" and good luck: Heinz.
    www.doccnc.com

  9. #9
    Gary E is offline Diamond
    Join Date
    Jan 2006
    Location
    Houston, TX
    Posts
    5,852

    Default

    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

  10. #10
    OKKHM1250 MAN is offline Plastic
    Join Date
    Feb 2010
    Location
    Buffalo'ish
    Posts
    9

    Default

    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

  11. #11
    Arthur.Marks is offline Stainless
    Join Date
    Nov 2008
    Location
    Chicago, IL
    Posts
    1,524

    Default

    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??

  12. #12
    Kallam is offline Cast Iron
    Join Date
    Feb 2006
    Location
    South Carolina
    Posts
    265

    Default

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

  13. #13
    zach123 is offline Aluminum
    Join Date
    Nov 2008
    Location
    mn,usa
    Posts
    143

    Default

    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.

  14. #14
    Kyle Smith's Avatar
    Kyle Smith is online now Hot Rolled
    Join Date
    Apr 2008
    Location
    Helmer, Indiana, USA
    Posts
    939

    Default

    Quote Originally Posted by zach123 View Post
    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.

  15. #15
    OKKHM1250 MAN is offline Plastic
    Join Date
    Feb 2010
    Location
    Buffalo'ish
    Posts
    9

    Default

    Quote Originally Posted by Kyle Smith View Post
    Go until your snap it off and then back off just a touch.
    thats great!

  16. #16
    scudzuki is offline Stainless
    Join Date
    Aug 2008
    Location
    SouthEastern Pennsylvania
    Posts
    1,027

    Default

    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

  17. #17
    Glacern's Avatar
    Glacern is offline Aluminum
    Join Date
    Feb 2008
    Location
    California
    Posts
    154

    Default

    Quote Originally Posted by zach123 View Post
    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, 200-300SFM 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

  18. #18
    Dave K is offline Diamond
    Join Date
    Mar 2004
    Location
    Waukesha, WI
    Posts
    6,120

    Default

    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.

  19. #19
    706jim is offline Stainless
    Join Date
    Jun 2006
    Location
    Thunder Bay Canada
    Posts
    1,251

    Default

    Quote Originally Posted by Dave K View Post
    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

  20. #20
    Dave K is offline Diamond
    Join Date
    Mar 2004
    Location
    Waukesha, WI
    Posts
    6,120

    Default

    Quote Originally Posted by 706jim View Post
    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.

Page 1 of 2 12 LastLast

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •