24,000 6-32 holes to make, how fast can I go?
Close
Login to Your Account
Page 1 of 5 123 ... LastLast
Results 1 to 20 of 87
  1. #1
    Join Date
    Sep 2006
    Location
    Long Island, New York
    Posts
    667
    Post Thanks / Like
    Likes (Given)
    284
    Likes (Received)
    105

    Default 24,000 6-32 holes to make, how fast can I go?

    The material is 1/8" thick cold rolled. It came on a coil before it was stamped, it's pretty soft.
    I have OSG Hypro cut taps. Last time I ran them at 2560 RPM, I think the Brother TC-31A machine is capable of tapping at up to 8000 rpm.

    How fast can you push a 6-32 cut tap (drilling .110 dia.)?

  2. #2
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    3,185
    Post Thanks / Like
    Likes (Given)
    1378
    Likes (Received)
    4159

    Default

    I would just get them started and chase them by hand.

    on second thought, if your brother will tap at 8K, that's where 'd start

  3. Likes Volitan, Joe Miranda, jrmach, aj, PegroProX440 liked this post
  4. #3
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    8,095
    Post Thanks / Like
    Likes (Given)
    910
    Likes (Received)
    3896

    Default

    I would wonder how fast the machine would actually accelerate and reverse in that short distance. Pretty sure there is a point where increasing the programmed RPM does nothing to decrease the cycle time. i would just call the machine builder and ask them.

  5. Likes Booze Daily, Hardplates, chet liked this post
  6. #4
    Join Date
    Sep 2006
    Location
    Long Island, New York
    Posts
    667
    Post Thanks / Like
    Likes (Given)
    284
    Likes (Received)
    105

    Default

    Quote Originally Posted by Dualkit View Post
    I would wonder how fast the machine would actually accelerate and reverse in that short distance. Pretty sure there is a point where increasing the programmed RPM does nothing to decrease the cycle time. i would just call the machine builder and ask them.
    I've noticed that with our older Haas's but the Brother gets up to speed in no time flat.

  7. #5
    Join Date
    Jun 2012
    Location
    Davis Junction, Illinois
    Posts
    196
    Post Thanks / Like
    Likes (Given)
    69
    Likes (Received)
    47

    Default

    Compare the cycle time to using a thread mill. No spindle accel/decel to wait for.

  8. Likes Joe Miranda liked this post
  9. #6
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    762
    Post Thanks / Like
    Likes (Given)
    110
    Likes (Received)
    391

    Default

    Quote Originally Posted by Archer120x View Post
    Compare the cycle time to using a thread mill. No spindle accel/decel to wait for.
    You serious, Clark?

  10. Likes wheelieking71, PegroProX440 liked this post
  11. #7
    Join Date
    Oct 2004
    Location
    Elyria Ohio
    Posts
    1,872
    Post Thanks / Like
    Likes (Given)
    3579
    Likes (Received)
    796

    Default

    Quote Originally Posted by Archer120x View Post
    Compare the cycle time to using a thread mill. No spindle accel/decel to wait for.
    And no broken taps! A broken thread mill is waaaay easier to deal with.

  12. #8
    Join Date
    Oct 2016
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    352
    Post Thanks / Like
    Likes (Given)
    796
    Likes (Received)
    228

    Default

    Had to be an engineer that specified 6-32 threads

  13. #9
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    743
    Post Thanks / Like
    Likes (Given)
    221
    Likes (Received)
    322

    Default

    I doubt the spindle would ever come close to reaching 8000 rpm in that short of a time period.

    Never used one on a cnc but take a look at this YouTube

  14. Likes Volitan, Brian, mr.greenman, TheOldCar, aj liked this post
  15. #10
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,409
    Post Thanks / Like
    Likes (Given)
    219
    Likes (Received)
    1684

    Default

    Quote Originally Posted by Archer120x View Post
    Compare the cycle time to using a thread mill. No spindle accel/decel to wait for.
    Cycle time will be way faster tapping. My S700 gets up to 6k-8k RPM in a fraction of a second, like literally a blink of an eye. I would estimate actual in-the-machine cycle time per tapped hole would be ~1 second.

    Drilling accurately might be more challenging with tap vs. threadmill, but with 24K holes to do, I would be spending some time to dial in the hole size, then get on with it and tap.

    Heck, I could add a tool break check, and still be faster tapping than threadmilling.

    Regards.

    Mike

  16. Likes Hardplates, TeachMePlease, Volitan, Tichy liked this post
  17. #11
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,269
    Post Thanks / Like
    Likes (Given)
    842
    Likes (Received)
    1273

    Default

    I guess it depends on whether it's 24000 pcs with 1 tapped hole or 1 pc with 24000 tapped holes.
    Or somewhere in between.

  18. Likes charlie gary liked this post
  19. #12
    Join Date
    Dec 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    806
    Post Thanks / Like
    Likes (Given)
    246
    Likes (Received)
    474

    Default

    Do you need to drill and tap? Through hole right? The Brother has a drill/tap cycle G177 for DRAPs. A tap with a drill tip. I've used them on several occasions and this could be one of those 'right' applications. Cycle time with one of those around the 2 second range for drilling and tapping.

  20. Likes Bobw, Philabuster, mountie, wheelieking71 liked this post
  21. #13
    Join Date
    Dec 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    806
    Post Thanks / Like
    Likes (Given)
    246
    Likes (Received)
    474

    Default

    Quote Originally Posted by Hardplates View Post
    I doubt the spindle would ever come close to reaching 8000 rpm in that short of a time period.

    Never used one on a cnc but take a look at this YouTube
    He has the best tapping cnc, a tapmatic would not improve the tapping ability in most cases.

  22. Likes Winterfalke liked this post
  23. #14
    Join Date
    Sep 2006
    Location
    Long Island, New York
    Posts
    667
    Post Thanks / Like
    Likes (Given)
    284
    Likes (Received)
    105

    Default

    It's 6,000 pcs with 4 tapped holes in each.

    The DRAP sounds interesting too. Yes it's a thru hole in a 1/8" part. I've seen those things before but the ones I saw were shit quality so I forgot about them. Maybe I'll look into a good brand after I get this thing running.

    I like Larry Dickmans idea of using the max as a starting point

  24. #15
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    743
    Post Thanks / Like
    Likes (Given)
    221
    Likes (Received)
    322

    Default

    Quote Originally Posted by BROTHERFRANK View Post
    He has the best tapping cnc, a tapmatic would make it tap worse.
    Never used a Brother. It would be interesting to see what the average rpm is while tapping

  25. #16
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    507
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    179

    Default

    Quote Originally Posted by Archer120x View Post
    Compare the cycle time to using a thread mill. No spindle accel/decel to wait for.
    Great idea. And 6-32 could be cut in one pass. It would partially depend on the tightness and screw comp settings of your machine as to how fast you can run it and still maintain an acceptable amount of circularity. I mean small thread mills in small holes make for very small circular tool paths. Some machines are better at this then others.

    If the holes are fairly close to to each other I suggest trying all your rapid moves, even in and out of the hole, in a high feed G1 instead. I do this when creating HSM tool paths. Keeping the return to start point, which at times can be very close, at a high feed rate in lieu of rapid.. (250-500ipm) My Fanuc driven Mori machine moves quicker like this and the motors seem to like it a lot better. It's actually how I discovered the concept. I was getting an overheat or overload error on the servos during an HSM path. I guess dumping all the power it had into trying to get up to full rapid in a quarter or half inch was too much to ask. The only thing I did to get rid of the alarming was switch all my G0s to high feed G1s and no more problems. It also seemed to run faster and smoother.

    Ha... imagine producing a job with 24,000 tapped holes and never reversing the spindle. Sounds crazy but who knows? May be that the machine and overall program time would also like the idea.

    I see this no reverse tapping story told to the right crowd at the right time will likely get you a free beer to boot. :-)

    Dave

  26. #17
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,076
    Post Thanks / Like
    Likes (Given)
    4626
    Likes (Received)
    3059

    Default

    Quote Originally Posted by Hardplates View Post
    Never used a Brother. It would be interesting to see what the average rpm is while tapping
    They are pretty insane when tapping. I'd be surprised if the average rpm isn't the programmed rpm or damn close to it.
    I tap 8k holes every 2 months or so in 6061, #4-40 threads. And it doesn't mess around. There isn't a machine that compares to a Brother when tapping even our brand new Okuma mills don't even come close to the tapping efficiency.

  27. Likes DrHook, hanermo, Winterfalke liked this post
  28. #18
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,409
    Post Thanks / Like
    Likes (Given)
    219
    Likes (Received)
    1684

    Default

    Quote Originally Posted by 13engines View Post
    Great idea. And 6-32 could be cut in one pass.
    In cold-rolled steel? (I'm assuming that's what the OP meant when he said "It came on a coil".) 6-32 threadmill has a tensy tiny minor diameter, like .065". Not saying it can't be done single-pass, but I would predict that thread size consistency would be a challenge.

    Regards.

    Mike

  29. #19
    Join Date
    Sep 2006
    Location
    Long Island, New York
    Posts
    667
    Post Thanks / Like
    Likes (Given)
    284
    Likes (Received)
    105

    Default

    Quote Originally Posted by Hardplates View Post
    Never used a Brother. It would be interesting to see what the average rpm is while tapping
    I've used those tapmatics in a mid-90's vintage Fadal and they are the bees knees.
    This Brother was made for this though. Even though it's an older 1999 model they made the spindle super light weight so the accel/decel and reversing of the spindle is damn near instant. It's like it's either on or off.

  30. #20
    Join Date
    Sep 2006
    Location
    Long Island, New York
    Posts
    667
    Post Thanks / Like
    Likes (Given)
    284
    Likes (Received)
    105

    Default

    Quote Originally Posted by Finegrain View Post
    In cold-rolled steel? (I'm assuming that's what the OP meant when he said "It came on a coil".) 6-32 threadmill has a tensy tiny minor diameter, like .065". Not saying it can't be done single-pass, but I would predict that thread size consistency would be a challenge.

    Regards.

    Mike
    Yes CRS, I can't get a number but I'm told it's "about 1/4 hard." It's really soft stuff.


Tags for this Thread

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
  •