Results 1 to 15 of 15
  1. #1
    emt2688 is offline Cast Iron
    Join Date
    Mar 2006
    Location
    Norfolk, NE
    Posts
    258

    Default small hole drilling

    Need to drill about 200, .024 diameter holes through .094 thick 304 stainless steel.

    Using a machining center with 10,000 rpm available, what would you recommend for speeds and feed (IPM), and pecking length. What I have available in house is just some HSS Jobber drills, black coated (basic drills).

    Also, I can either flood it, or micro drop it (preferred). Which would you use?

  2. #2
    PhillipM is offline Cast Iron
    Join Date
    Aug 2008
    Location
    Rotherham, UK
    Posts
    490

    Default

    For cheap jobber HSS drills - 2300rpm, 1ipm.

    I'd flood it myself, single peck at .06.

    You can probably go up to about 6krpm on the and feed accordingly but they should be a decent start point without knowing whether the drills are decent or not.

  3. #3
    chip_maker's Avatar
    chip_maker is online now Stainless
    Join Date
    Jan 2006
    Location
    ct.
    Posts
    1,057

    Default

    I'd run it at 40-50 feet per min @ 45'/min your at about 7163rpms, 2300 is way to slow. as far as feed goes I would start at .0005/rev, maybe even less. keep the drill as short as possible too.

  4. #4
    StreetSpeed's Avatar
    StreetSpeed is offline Hot Rolled
    Join Date
    Oct 2008
    Location
    NY
    Posts
    614

    Default

    I would definitely try and get a straight flute carbide drill, if I had to do 200 of those holes. Don't know the speeds and feeds, but I can say it'll be way faster than an HSS drill, and it'll go the distance once you get everything dialed in.

  5. #5
    Dualkit is offline Diamond
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    4,412

    Default

    Carbide circuit board drill?

  6. #6
    T-BONIMUS is offline Aluminum
    Join Date
    Dec 2008
    Location
    OREGON
    Posts
    112

    Default

    dont know if you have cts... but mitsibushi has a micro with coolant holes that will work well (no peck)

  7. #7
    Metalcutter's Avatar
    Metalcutter is offline Titanium
    Join Date
    Sep 2005
    Location
    San Diego
    Posts
    2,793

    Default

    Quote Originally Posted by emt2688 View Post
    Need to drill about 200, .024 diameter holes through .094 thick 304 stainless steel.

    Using a machining center with 10,000 rpm available, what would you recommend for speeds and feed (IPM), and pecking length. What I have available in house is just some HSS Jobber drills, black coated (basic drills).

    Also, I can either flood it, or micro drop it (preferred). Which would you use?
    I don't care for flood because you might be drilling for twenty minutes and find the drill broke on the first hole. *s

    Tulon Circuit board drills are VERY good tools.

    Chip load is a little shy of .0004" per flute. Find an rpm on your machine which runs smooooooth!

    It really doesn't matter what the rpm is as long as the chip load is the same, or you exceed the cutting tool's ability to handle the heat.

    The smaller the drill (tool) the more you need absolute concentricity. Think of a 1" drill running out .010" -- No big deal. Worry that down to a .024" drill and the runout gets a bit tight. Around .00024" TIR

    The first peck is good for 3 to 3.5 diameters. After that .5 diameter per peck.

    I've drilled .020" holes at 1000rpm and .6 ipm with this pecking idea just to show my help you don't need a million rpm to drill holes.

    Put a 1" travel indicator on the "Z" axis and see how it reacts when peck drilling. Slow everything down to a walk so you can see what is going on. Look for it to snatch the drill out of the hole while it is still taking a cut. I don't think you will see any dwell before it retracts. If so, that fact is very hard on the drill's cutting edges.

    I'd build a special routine bit by bit reversing the feed for a revolution before the rapid up.

    You can get away with it in the softer materials but sst is mean.

    These are what I've found to be good things.

    Best regards,

    Stan-

  8. #8
    jbexplorer's Avatar
    jbexplorer is offline Aluminum
    Join Date
    Sep 2008
    Location
    San Jose, California
    Posts
    118

    Default

    I would run 8500 RPM at 15. IPM and peck 1/3 the drill dia. Flood coolant. And use a http://www.guhring.com/drills.shtml

    JB

  9. #9
    tt12no is offline Plastic
    Join Date
    Aug 2008
    Location
    Northern Cal.
    Posts
    14

    Default

    I would run that hss drill in collet holder @ 5570 rpm, 3.3 ipm, .006 pecking.
    When You get done with the drilling; Let' s know what combination used to do the job. Good luck to You.
    tt12no

  10. #10
    Chris59's Avatar
    Chris59 is offline Aluminum
    Join Date
    Nov 2006
    Location
    Jupiter, Florida
    Posts
    205

    Default

    Stan, that was interesting about the reverse being hard on the drill. I never noticed that before. I'll check that out. Thanks.

  11. #11
    Metalcutter's Avatar
    Metalcutter is offline Titanium
    Join Date
    Sep 2005
    Location
    San Diego
    Posts
    2,793

    Default

    Quote Originally Posted by Chris59 View Post
    Stan, that was interesting about the reverse being hard on the drill. I never noticed that before. I'll check that out. Thanks.
    Hi there Chris59...

    There is more on it in an earlier thread if you'd like to read it.

    http://www.practicalmachinist.com/vb...830#post822830

    Best regards,

    Stan-

  12. #12
    Chris59's Avatar
    Chris59 is offline Aluminum
    Join Date
    Nov 2006
    Location
    Jupiter, Florida
    Posts
    205

    Default

    VERY interesting stuff. Thanks again, Stan.
    Chris

  13. #13
    GarlicDude's Avatar
    GarlicDude is offline Cast Iron
    Join Date
    Apr 2006
    Location
    Gilroy, CA
    Posts
    263

    Default

    If it's SST sheetmetal good luck, the skin on SST sheet is some of the nastiest stuff to drill that I've encountered.

    Best,
    Steve

  14. #14
    emt2688 is offline Cast Iron
    Join Date
    Mar 2006
    Location
    Norfolk, NE
    Posts
    258

    Default

    For what its worth, I used 4000 rpm and 2.0 ipm. Pecked it every .008 and used microdrop mister. This combo worked about the best.

    The part was actually tubing, with 8 holes around the perimeter. It was .250 OD x .062 ID.

    I changed bits often on the parts, just for insurance purposes. Time wasn't as much a matter as scrapping a high dollar part.

    Thanks for all the suggestions, and for all the info provided!!

  15. #15
    SeymourDumore is online now Diamond
    Join Date
    Aug 2005
    Location
    CT
    Posts
    6,248

    Default

    EMT

    Glad you've worked it out.
    Thankfully I don't even have to spend a second worrying about holes under 1/8 into anything with a holepopper at my disposal.
    Just for future reference, an EDM holpopper eats a job like this for breakfast.
    Most start at .4mm up to 3mm in increments of .1mm, but some of the higher end ones can handle electrodes down to .0005".
    They also drill very fast, your hole for example would have taken 20 seconds at most per hole and would have produced no burrs at all.

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
  •