Drilling 18-8 bolts
Close
Login to Your Account
Likes Likes:  0
Results 1 to 9 of 9
  1. #1
    Join Date
    Jul 2016
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    310
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    37

    Default Drilling 18-8 bolts

    I have this job drilling 1/4" SHCS 18-8 x 3/4" length with a 9/64 hole. My present operation uses cobal 135 split point, 1200 rpm and 2 ipm feed, pecking at 0.075" mostly

    G98 G83 X? Y? Z0.8041 R0.1124 I0.24 J0.075 K0.08 P0 F1.956 to be exact.

    I am prepping the bottom of the hex with a .125 endmill to make it flat, otherwise the drill wanders too much. The main issues are #1 speed, and #2, rats nests. I have a jig that holds 120 pieces, so I almost have to keep an eye on the whole process. Also, I basically need to change the bit after 120 pieces.

    I have done some experimenting with carbide drills, and my experience is that it rats nests a little, and after about 15 holes it snaps, pretty much at the different feeds and speeds I tried.

    My machine is a VF2, without through hole coolant. Any ideas on a better process?

  2. #2
    Join Date
    Feb 2007
    Location
    Utah
    Posts
    207
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    6

    Default

    I drilled several hundred steel grade 8.8 bolts and found the thread rolling and head forging made for a huge variation in toughness along the depth. I would guess 18-8 will be similar. Your drill diameter puts the cut right in the work hardened region of the threads too.

    I had better results using cobalt for longevity, carbide worked great for several holes then one catch on a hard spot and it snapped. Maybe try a carbide spade drill to start the hole down to 2-3x diameter depth then change to a cobalt twist drill.

    spade here:
    https://www.mscdirect.com/product/details/83245803

    I also used some heavy tapping oil on top of the head. It was a lot of babysitting unfortunately.

  3. #3
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,284
    Post Thanks / Like
    Likes (Given)
    15065
    Likes (Received)
    11134

    Default

    18-8. Basically 304. But shittier (more shitty?) since its been cold worked.

    I've found the biggest problem I have in work hardening materials when drilling, is the
    retract. The very beginning of the retract.

    I hand code my drill cycle and then run it as a sub. Feed in, then feed out a bit,
    then either fast feed or rapid out.. Then back in, but above where you stopped cutting,
    and then start going again. You can also come WAY out of the hole to give the coolant
    a better shot of getting down into the bottom of the hole, and also give you a
    greater chance at getting rid of your birds nest.

    The reason I do this is because 304 work hardens. The chip is fricken hard, and its pretty
    easy to rip the cutting edges off of the drill on a retract. Even if you have a cycle that
    has a dwell before retract.. YOU ARE DWELLING ON 304!!!! in other words RUBBING. You really shouldn't
    do that.

    Also if you take the 5 or 10 minutes to hand code, you could add in some chip breaks in between
    your pecks to attempt to eliminate your birds nest problem. Feed out .010 or so and then keep
    going down.

    Just my 2 cents.

    Edit: One way to check if your problem is with the rapid retract without having to reprogram. Turn your
    rapids way down and see what happens. When I only have a few quick holes to do, instead of wasting
    time coding, I'll just run it with the rapids in the basement.

  4. #4
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    8,509
    Post Thanks / Like
    Likes (Given)
    1039
    Likes (Received)
    4234

    Default

    With 18-8 aka pretty much 304 I have the best luck using Titanium-Nitride (TiN) Coated Cobalt Steel drills. Carbide is great but they are pricey and any shock, like change in material condition or a little runout or misalignment and they break without warning.

  5. #5
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    9,587
    Post Thanks / Like
    Likes (Given)
    2248
    Likes (Received)
    6641

    Default

    Ditch the 1/8" endmill. Use a stout carbide 9/64" drill (meant for SS, not fiberglass), around 3Krpm and 7ipm for ~.1" Dp to establish hole location. Tune the feed to get where the chips fling off the flutes on retract, you can add depth if you find a stable area that gives adequate tool life. G81 or coded G1 to control retract.

    Follow up with the cobalt drill at ~2200rpm and 5ipm, feed to just above hole bottom and start a G1 peck sub as Bobw suggests, but with a fairly short cut (start at .03"), and tune S/F to get chips that don't nest. This may require going in fairly hot, but always feeding above the last floor to avoid ramming in, pulling back to cleanly end the current chip (so not pulling the edges off the drill).

    If nothing helps eliminate bird nests, you can set up a stripper plate (think like a slot or the "V" of a thread gage, as a diving board off a 1-2-3 block - bring the drill into the notch near the collet, feed up to strip off the nest. Reverse spindle if you must.

    Work on your fixture plate array from the furthest points from coolant towards the coolant side (presumably left to right). This helps direct chips away from the "not yet drilled" heads and lessens chips falling into the screw heads before the drill gets there.

    Smaller, heavier chips will be worse if they do fall into the heads before the drill gets there (or between the carbide and the cobalt), so you might decide the a nest that you can strip off winds up being better, but that's dependent on how aggressive your coolant spray is and the spacing of the bolt array on the fixture. I'd rather have a little more space for the bolts and give plenty of room for the chips to fall in between the heads.

    Hope this is of some use...

  6. #6
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,990
    Post Thanks / Like
    Likes (Given)
    1311
    Likes (Received)
    2821

    Default

    Quote Originally Posted by friesen View Post
    I have this job drilling 1/4" SHCS 18-8 x 3/4" length with a 9/64 hole. My present operation uses cobal 135 split point, 1200 rpm and 2 ipm feed, pecking at 0.075" mostly
    You're running 45ish SFM and .0008" per cutting edge, per rev in 18-8!!! I'd be running .002" per side, per rev.

    Birds nests occur when you're chip isn't heavy enough to break off. So you've got to make them break.

    I have NEVER had good results using solid carbide Drills in 18-8 (304). Good ole black oxide HSS.

  7. #7
    Join Date
    Jun 2020
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    58
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    20

    Default

    If you have a lot of holes to do something like a coolant inducer begins to make a lot of sense.
    Quite a few companies make them, but they are all probably fairly expensive.
    New Baby Collet Type | BIG KAISER

    The only magic bullet is thru spindle coolant, which an inducer provides.
    9/64th is a small drill, but with TSC you should have much more success.

    Another trick with peck drilling is to retract and reverse the spindle which can help to fling off the chips, then advance again.
    Stringy Chips Wrapped Around Your Tools? Mark Has a Solution! – Haas Automation Tip of the Day - YouTube This video explains the topic well.

    Rob is right, you need to feed hard enough to force the chips to break.

  8. #8
    Join Date
    Jul 2016
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    310
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    37

    Default

    I think I'm going to try some of the suggestions here, especially hand coding exit and entry. I do wonder what value coatings could be, something like this ? 9/64 - .1406" Cobalt 130deg Screw Machine Length Drill TiAlN Coated MariTool

  9. #9
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    9,587
    Post Thanks / Like
    Likes (Given)
    2248
    Likes (Received)
    6641

    Default

    I think that a TiAln coating is more appropriate when cutting dry, and for 18-8 I'd rather have coolant. I'd stick with quality uncoated cobalt, perhaps a more exotic version from a Titex/Guhring/Nachi with a more free cutting tip than a simple split-point.


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
  •