How do you make sure a drill is correct on a lathe?
Close
Login to Your Account
Results 1 to 17 of 17
  1. #1
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    49
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    2

    Default How do you make sure a drill is correct on a lathe?

    Couldn't decide between here and CNC Machining for a sub-forum. I'm trying to figure out how to make sure a drill is centered and true on a 2 axis lathe, with a 12 tool turret, 5/6 are drill/boring bar holders. (All examples, just going to call it a Mazak Quick Turn 200, because it's not limited to this machine) The tool eye is messed up as far as I understand.

    I kinda ramble a lot, but there is a TLDR at the end.

    The main problem I see is for drills with a carbide insert tip and solid carbide drills. There are also issues with drills that are too big for the holders we have. We have some kind of drill collet holder. (is there a special name? I keep finding mill related tools) It's got a maximum collet size of .450~ or something. If we have a drill bigger then that, we have to "turn it down" which is a whole other deal of problems. What are these called and where can I find bigger ones? (So I can maybe suggest purchasing one) I think the biggest I found was a ER 20 or something like that. The carbide tipped drill has it's own holder with flats, to go into the turret spot for drills. I like to orientate drills so the flutes go straight to the other drill holder. I believe this would make on of the corners of the flute line up to the tool eye for measuring... If it worked. But other people don't seem to do this and I think it causes issues or the collet was dirty.

    The solid carbide drill is always in the collet holder, which is in a adapter, and then in the turret. This is supposed to be a + or - .002" hole and it's always nearly out of tolerance, Maybe even one side of the hole is bigger than the other. They also always chip right away, but we have to keep using them... A co-worker has me kinda scared when using carbide. Just about how it will explode if it's off center or vibrates too much. I don't want to be the one to break the $500 tool... I've tried looking up how to make sure they're centered and find videos about manual lathes and a tailstop style drill. There is a X 0 written on the side of the machine. I have no idea how accurate it is. One time I was trying to indicate the base of the carbide tipped drill's holder and it essentially told me it was off in the rotation of the turret. As that was the method I was told for checking drills by someone. I think that would be Y axis if it was a active tooling lathe?

    TLDR, How do you make sure a drill is running true and center on a lathe?

    Thanks,
    Higgins909

  2. #2
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    I dont have a tool setter so I put an indicator in the chuck and sweep the bore of the tool holder. This works great as long as your drill is straight and your holder is in decent shape.

  3. #3
    Join Date
    Sep 2011
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    27,746
    Post Thanks / Like
    Likes (Given)
    7561
    Likes (Received)
    8632

    Default

    Quote Originally Posted by Evlyn View Post
    I dont have a tool setter so I put an indicator in the chuck and sweep the bore of the tool holder. This works great as long as your drill is straight and your holder is in decent shape.
    All-manual, here.

    We keep "drill blanks" to-hand. US and Metric sets. Same size as the drills. Of course. Easier to sweep than a hole. So they are more all-around relevent than random ground rod or dowel pins. Which also work. Just not necessarily in the self-same holder or collet the drill will be going into.

    NB: Good idea to FIND OUT what that 'limited to .450"' collet system actually is? Shouldn't be a deep, dark mystery?

    Having to now-and-then turn down shanks on consumable items? Damned hard to justify THAT as anything but necessity allowed to slither into bad habit. Cheaper. most days, to eliminate the need.

    Has rubber? See Ortlieb. All-metal, alternating ended slits? ER? TG?

    There are more, but hardly an INFINITE number.

    Good idea to know about such things, their pluses and minuses. whether you have them TODAY or have input towards choices to make in the future.

  4. #4
    Join Date
    Mar 2013
    Location
    Surbiton, surrey, UK
    Posts
    1,622
    Post Thanks / Like
    Likes (Given)
    1997
    Likes (Received)
    1039

    Default

    You could mount something nice and round in your turret, say a dowel pin etc. Turn down a pin of equal diameter in the chuck then indicate the difference (im guessin from the tailstock in your case).
    This video gives the jist. The approach avoids possible indicator sag error when sweeping holes.

    Edit:-
    Wes did a set of videos on cnc alignment, a good watch to help you understand the most important bits.

    Cheers
    D

  5. Likes memphisjed liked this post
  6. #5
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,220
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2655

    Default

    indicator in chuck and indicate dowel pin in drill tool holder in tailstock.
    .
    be aware often cause of tram error tailstock is leaning down or to the side. so the longer tool can measure .010" off center and a short tool might measure .001" off center
    .
    and of course some longer drill bits for what ever reason are curved or not straight. that is drill tip off center usually varies with different drill bits in the holder. and sometimes position changes depending on how tight it is
    .
    most do not ever expect a drill to hold a tight tolerance drilled hole. sure sometimes its within <.002" but often its not. usually hole is bell mouth that is hole is bigger the first .100 in depth. and of course deeper holes are often curved or wavy (not straight) especially if drilled at higher feed rates
    .
    also if drill bit is reharpened off center it makes a bigger hole. i have seen very much sharpened off center drill bits, drill over size over .020" especially if no pilot hole was drilled first. so even if drill tip position is "exact" drill might still drill over size. usually badly off center sharpened drill was cause it wasnt in drill grinder chuck correctly and went unnoticed. its rare but i have seen it happen.

  7. #6
    Join Date
    Jun 2008
    Location
    Bellingham, WA
    Posts
    4,029
    Post Thanks / Like
    Likes (Given)
    962
    Likes (Received)
    2180

    Default

    One way to get a drill to cut close(r) to size is to first bore the hole with a bit a 32nd undersized and then finish the hole with the correct bit. This way the 2nd bit act more like a reamer and grind centering of the bit becomes relatively unimportant. Requires two steps but you ARE using a turret.

    Denis

  8. #7
    Join Date
    Sep 2011
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    27,746
    Post Thanks / Like
    Likes (Given)
    7561
    Likes (Received)
    8632

    Default

    Quote Originally Posted by dgfoster View Post
    One way to get a drill to cut close(r) to size is to first bore the hole with a bit a 32nd undersized and then finish the hole with the correct bit. This way the 2nd bit act more like a reamer and grind centering of the bit becomes relatively unimportant. Requires two steps but you ARE using a turret.

    Denis
    Drills make s**t-lousy reamers, actually. Hard on the drill. Hard on the predictability of the hole as well.

    More better to HAVE at least the few reamers one USES, even if not a "full set" of over/unders as was once more common.

    Or make a "D" reamer, right on size. Fast enuf', torch-hardened.

    "D"'s don't cut fast as DRILLS. Accurate enough, but not much as ever gets any slower but wax and Nitric Acid dropper. No place for the chip, so yer CONSTANTLY clearing.

    They do rather better as reamers, however. Still need lots of clearing, but the pre-existing bore itself provides space for chip.

  9. #8
    Join Date
    Apr 2004
    Location
    Modesto, CA USA
    Posts
    7,016
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1180

    Default

    I bought a hndfull of center drills from the bay. Included were a few nicely made, maybe even ground, dead centers. But with very slow taper like about 15 degrees. I chuck one in the lathe and use it to rough set tool height and check drill bit nose side to side.
    I suppose it could be used to locate a center punch mark or round hole in a four jaw set up.
    Bill D.

  10. #9
    Join Date
    Nov 2003
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    5,056
    Post Thanks / Like
    Likes (Given)
    176
    Likes (Received)
    1561

    Default

    My thoughts on doing this in the lathe.

    1. If you want an accurately sized and ROUND hole, use a reamer for the final step. Use one with a long shank so it can "find" it's own center in the previously drilled and slightly undersized hole.

    2. If you want the hole well centered, the lathe is your friend. Having the work turn while the drill bit is stationary is a really good way to get excellent concentricity. You need to use a short, and relatively inflexible drill bit. Even if it is slightly off center, it should cut a centered hole. So using a short carbide bit that is slightly smaller than the final diameter will produce a well centered hole that may be a bit larger than the drill's diameter, but it will still leave some meat for the reamer to remove in the final step.

    So drill first to get a well centered hole and then use the reamer to get it to an accurate size and completely round. Should get you well within 0.001" in both size and concentricity.

    That is how I would do it.

  11. #10
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    747
    Post Thanks / Like
    Likes (Given)
    111
    Likes (Received)
    386

    Default

    I throw a dowel in the tool holder and sweep it from the spindle. Same on a Y-axis lathe, same on a Swiss.

  12. #11
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,640
    Post Thanks / Like
    Likes (Given)
    1222
    Likes (Received)
    2603

    Default

    It sounds like the Turret needs to be mechanically realigned. Indicate the Holders bore, using an Indicator being held by the Chuck. Not a mag base on the Chuck. Use the offsets to get it to X zero. Then you'll see how far out of rotation the Turret is. If it's out more than "a lot", fix it.


    R

  13. #12
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    1,029
    Post Thanks / Like
    Likes (Given)
    1137
    Likes (Received)
    673

    Default

    Quote Originally Posted by Rick Finsta View Post
    I throw a dowel in the tool holder and sweep it from the spindle. Same on a Y-axis lathe, same on a Swiss.
    This. And I like to use a coax indicator as you can have sag with a test indicator that will throw off readings.

    As Rob said, if your x is zero and y is off. You'll need to realign your turret.

  14. Likes pmack liked this post
  15. #13
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    10,196
    Post Thanks / Like
    Likes (Given)
    3459
    Likes (Received)
    3646

    Default

    I have seen drills poorly pointed start off center on manual lathes so with a part that has no OD finish stock I tool bit scalp a small centering cut to the part end..likely it (the drill) will travel fairly good down the lathe center axis that way..I would not expect a reamer or a small then bigger drill to make better the centering of a bore.
    Reamer and/or smaller then bigger drills do make/correct the size. often a drill will cut at tenths over micrometer check size with smaller then bigger drilling.

  16. #14
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    278
    Post Thanks / Like
    Likes (Given)
    201
    Likes (Received)
    131

    Default

    Check out a Haimer Centro. I use it(in the collet chuck) with a ground pin in my ER25 lathe holders to do this, then switch the pin out for a drill. Pricey, but really nice.

  17. #15
    Join Date
    Nov 2014
    Country
    BELGIUM
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    We have a Mazak quickturn 200 at work and the Turret needs realignment at frequent intervals (wich is not normal with no crash causing this we think). And yes we notice that immediately when the turret is off when the drilled holes are oversized.
    We do the realignmet with an indicator in the chuck and running it inside a toolbar holder as said here before and then drilling goes perfect again...(for a while) :-)

  18. #16
    Join Date
    Apr 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default

    Same here, confirm turret is aligned. Then indicate a precision ground diameter, dowel pin, old endmill shaft or even the toolholder bore itself. You have to make sure the turret alignment is correct first.

  19. #17
    Join Date
    Nov 2003
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    5,056
    Post Thanks / Like
    Likes (Given)
    176
    Likes (Received)
    1561

    Default

    Yes, do align that turret as best as you can. But for accurate holes, my approach would be:

    1. Use a SHORT spotting drill to start the hole. Carbide would be best because it does not flex so it is acting more like a boring bar than as a drill. The depth of this cut will be less than or equal to the cone made by the cutting edges of that drill bit. This will produce an accurately centered starting dimple for the next drill.

    2. Use a full length HSS drill to make a hole that is a bit smaller than final size. If that final size is fairly large (over about 1/2") then use a HSS pilot drill first (1/4" to 3/8" or so). Again, this should produce a well centered hole as the drill(s) can flex a bit to drill on center. This is an advantage of turning the work in a lathe while the drill bit is stationary.

    3. Use a reamer for the final operation. This will follow the properly centered hole already drilled and finish it to an accurate size and, with the multiple flutes, keep it very round.

    Asking one drill, HSS or carbide, long or short, or whatever characteristics it may have, to do all of the above is asking a lot. Perhaps you can make that work in a production situation and perhaps not. I guess the question would be is if the number of unacceptable parts that are avoided is worth the extra time needed for several operations as opposed to just one.


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
  •