Results 1 to 10 of 10
  1. #1
    Nick H is offline Aluminum
    Join Date
    Jun 2007
    Location
    Westfield, WI
    Posts
    85

    Default Tapping speed and feed formula needed

    I'm looking for a formula to plug in proper feeds and speeds on a cnc lathe that does not have rigid tapping.

    I'm trying to cut a 1/4-32 ID thread with a tap and have no clue where to start for rpm and feed rate. (floating tap holder)

    So if anyone could punch up this example and show me how to you got the feeds and speeds so I can learn to use it properly that would be most appreciated.

  2. #2
    doug925's Avatar
    doug925 is offline Titanium
    Join Date
    Nov 2002
    Location
    Houston, Texas
    Posts
    2,434

    Default

    I get my tapping SFM by looking at Vega Tap's recommended SFM sheet.
    Surface footage info is available from most tap mfgr's.

    As far as FPR goes I use the pitch of the tap. But if you are using a floating (tension/compression) holder, then you might want to feed in a bit laggin of the pitch.

    IE 1/4x32 tap = 1/32=.03125" per revolution So for a T/C holder I might feed in at .03 IPR, and feed out at .03125"

    So for 1000RPM, to feed in @ 30 IPM, and feed out at 32.IPM.
    (1000rpm x .03" =30 inches per minute)

    Doug.

  3. #3
    3t3d is online now Titanium
    Join Date
    Nov 2004
    Location
    WI
    Posts
    3,879

    Default

    1/4-32. Is that for a glow plug?

  4. #4
    Nick H is offline Aluminum
    Join Date
    Jun 2007
    Location
    Westfield, WI
    Posts
    85

    Default

    Quote Originally Posted by 3t3d View Post
    1/4-32. Is that for a glow plug?
    Not that I know of.. just a feature on a part for a customer.

  5. #5
    apestate is offline Stainless
    Join Date
    Mar 2003
    Location
    San Francisco, CA
    Posts
    1,018

    Default

    Program a slower feed rate on the way in and the correct feed rate on the way out.

    You can easily figure out how far the tap holder will extend by figuring the number of turns you want to cut. Let's say you want the tap to extend 1/4" on the in feed, and you want the tap to go 3/4" in.

    1/32 = .03125
    .750 / .03125 = 24 turns
    .250 / 24 = .0104... so reduce the feed rate on the infeed by .0104.

    G97 G00 X0 Z.25 M03 S200
    G01 Z-.750 F.0209
    M05
    G97 G01 Z.375 F.0313 S200 M04

    Clack, tap holder snaps back.

  6. #6
    Curt B's Avatar
    Curt B is offline Cast Iron
    Join Date
    Aug 2007
    Location
    Edmonton,Alberta,Canada
    Posts
    375

    Default

    Quote Originally Posted by Nick H View Post
    I'm looking for a formula to plug in proper feeds and speeds on a cnc lathe that does not have rigid tapping.

    In this case the time your spindle takes to slow down, reverse direction, and get back to speed are what will determine what you can use regardless of what's right for a given tool/workpiece material. The faster you go the worse it is.
    Last edited by Curt B; 11-04-2008 at 11:48 AM. Reason: spelling

  7. #7
    706jim is offline Stainless
    Join Date
    Jun 2006
    Location
    Thunder Bay Canada
    Posts
    1,244

    Default

    Quote Originally Posted by 3t3d View Post
    1/4-32. Is that for a glow plug?
    I bet it is.

  8. #8
    apestate is offline Stainless
    Join Date
    Mar 2003
    Location
    San Francisco, CA
    Posts
    1,018

    Default

    Quote Originally Posted by Curt B View Post
    In this case the time your spindle takes to slow down, reverse direction, and get back to speed are what will determine what you can use regardless of what's right for a given tool/workpiece material. The faster you go the worse it is.

    Yeah, that's why I said 200 rpm. I also believe M05 between the two feeds is the best way. I've tried going straight from M03 to M04 and even at low rpm it sounds a little clunky. You'll have to try it and see, Nick.

  9. #9
    SwissPro's Avatar
    SwissPro is offline Hot Rolled
    Join Date
    May 2006
    Location
    Illinois
    Posts
    957

    Default

    The best way I've found is to feed in at 90-95% of the thread lead going in. The way out I feed at 100% but it doesn'y matter much either way.

    Also you should use G32 instead of G01. This way if some bonehead has the feed rate overide turned up or down it won't break anything. Most controls execute the M05 after the commanded position has been reached. So the best way to program is like this:

    Assuming 85 SFM for mild steel - 85/0.25*3.82=1299
    Feed rate - 1/32=0.03125 0.0325*.95=0.0297
    Hole depth = .5 so take .5*.95=0.475 and use 0.475" for your programmed Z-depth

    G97M03 S1300
    T1212;
    G0 X0 Z0.08;
    G32 Z-0.475 F0.0297 M05;
    M04 Z 0.08 F.03125; (G32 is modal here)
    G04 P1000;

    You can also put a dwell in between the two G32 lines. Most small lathes don't need it, but a larger lathe with a big chuck might need a little time to stop before the spindle reverses. In that case program your approach further away and you depth shallower and use the Z-axis offset to bring the depth in.

  10. #10
    apestate is offline Stainless
    Join Date
    Mar 2003
    Location
    San Francisco, CA
    Posts
    1,018

    Default

    SwissPro, you nailed it.

    I thought I remembered M05 being on the end of the feed line but I wasn't sure. That does work excellent. Also I forgot about changing the depth of feed!

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
  •