Drilling 17-4 Rc35
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 33
  1. #1
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    461
    Post Thanks / Like
    Likes (Given)
    99
    Likes (Received)
    123

    Default Drilling 17-4 Rc35

    First 17-4 parts. Cutting the overall shape and putting slots in went well. I used a cobalt U size drill to start the slots. Today, I need to put a couple U sized holes 1.5" deep. The drill broke on the first hole (did two holes yesterday without issue). I was running it 225 RPM, 22mm/min (just under 1 IPM), flood coolant, ER25 collet on a Speedio. Material report says HB313 which I believe to be around Rc35. Any advice?

    hole.jpg

  2. #2
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,640
    Post Thanks / Like
    Likes (Given)
    1222
    Likes (Received)
    2602

    Default

    I don't memorize the letter sizes, and I don't care enough to look it up. You don't mention the condition of the material so that doesn't help. It would help if we knew what style of Drill, Peck amount and if the hole is through or not. It would also help to explain what "Drill broke" means exactly, like in half?

    R

  3. #3
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    461
    Post Thanks / Like
    Likes (Given)
    99
    Likes (Received)
    123

    Default

    U is .368". The material is in the annealed state. Hole is blind, but it drilled a couple through holes yesterday in .750" thick material. It pecked once yesterday when the first hole didn't go through, so I went back and finished it. I was planned to peck this hole once, but it didn't make it that far. Drill is cobalt jobber from McMaster. Tip is pretty mangled. I heard a pop and stopped it a second or two later.

    I need to ream it to be .375". I have a cobalt reamer for that. A local place has carbide 9.3 and 9.4mm drills for 80 each. I thought cobalt would be able to do this though.

    Thanks

    broken-drill.jpg

    drill.jpg

  4. #4
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    461
    Post Thanks / Like
    Likes (Given)
    99
    Likes (Received)
    123

    Default

    feed per rev is just under .004" Maybe not enough?

  5. #5
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,750
    Post Thanks / Like
    Likes (Given)
    4355
    Likes (Received)
    2883

    Default

    If you're running it on a Speedio, buy a coated carbide drill.
    If you buy crap tooling thinking you're saving money, you're wrong a lot of the time.
    A .368" carbide drill isn't going to break the bank, it will pay for itself in no time.
    BUT
    if that's the only drill I had, I would run it around 30-40 sfpm with a .006" ipr feed for starters with flood coolant.

  6. #6
    Join Date
    Sep 2015
    Country
    CANADA
    State/Province
    Ontario
    Posts
    96
    Post Thanks / Like
    Likes (Given)
    46
    Likes (Received)
    36

    Default

    Broken drill looks like too much feed.

    I would increase your speed a bit and cut back the feed, myself.

  7. #7
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,640
    Post Thanks / Like
    Likes (Given)
    1222
    Likes (Received)
    2602

    Default

    Now were cooking. Annealed can be pretty gummy, unless you have TSC I wouldn't use Carbide. And I would peck Drill it for sure. I would at least double the RPM, 21 SFM is really slow, and I would jack the chipload up to .0057" but only with the RPM increase. At that super slow RPM you need about 10 miles of Rigidity. I would definitely change to Stub length/Screw Machine 135º split point Drill.

    As a rule of thumb, in the Annealed condition-I treat it like 304.

    R

  8. Likes Bobw, CosmosK liked this post
  9. #8
    Join Date
    May 2011
    Location
    Milford, Ct
    Posts
    131
    Post Thanks / Like
    Likes (Given)
    43
    Likes (Received)
    27

    Default

    I'd be around 50-65sfm, (approx 540-700rpm), and approx .003/.004 per rev., flood coolant, and you should be good. 35rc isn't anything to be scared of.

  10. #9
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    461
    Post Thanks / Like
    Likes (Given)
    99
    Likes (Received)
    123

    Default

    I found this older thread: link

    Based on recc's from that thread, I should be about .007" per rev. I also saw 35-50 SFM. I'm going to get a couple more cobalt jobbers and try again. 400 RPM, .0064" per rev pecking maybe 1/2". Thanks for the help.

  11. Likes Mtndew, litlerob1 liked this post
  12. #10
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,049
    Post Thanks / Like
    Likes (Given)
    13918
    Likes (Received)
    10720

    Default

    17-4 in condition A can be a little unpredictable. No were near as bad as 304,
    but it can vary a bit.. And it still has its sticky stainlessy properties.
    Again not as bad as 304... Nothing sucks more than 304...

    One thing I have found in workhardening stainless.. You have to be careful with
    your pecks.. That chip is nasty, and if you rapid out of the hole without
    cutting the chip off first, you can rip the cutting edges off of the drill...

    Generally pretty easy to add a dwell (But don't let it rub of course ).. I longhand it when
    I have to, feed back out .020" or so, then rapid, or fast feed back in to the same
    point..

    If I'm only doing a couple holes, I'll just turn the rapids way way down.


    Another thought.. Stainlessy stainlesses can be nasty when you break out the back side.
    Sometimes its productive to make sure everything is nice and cool down at the bottom
    before breaking through, you may have damaged the drill on the through holes...

    Another random though.. Speedio.. Are you out of the hole long enough to get coolant
    into the hole before it goes back in.. Another little thing I do when I long hand my
    drill cycles.. Not always, depends, I'll come up quite a bit further than my clearance
    plane to make sure I get a new batch of coolant down into the bottom, and it also
    leaves a bit more room for any chips on the drill to go away...

    Quick story.. Lathe, and not stainless. 1-5/16" drill in 4140 I think it was.. Going
    almost a foot deep.. Just a twisty drill, it was only 40 parts.. If I ran full
    rapids, the bottom of the hole and the end of the drill would melt down.. If I ran
    25% rapids, everything came out great.. Of course a well meaning employee saw the
    rapids turned down, and turned them up and I ended up with a melted drill...

  13. Likes CosmosK liked this post
  14. #11
    Join Date
    Sep 2008
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,712
    Post Thanks / Like
    Likes (Given)
    1141
    Likes (Received)
    988

    Default

    Quote Originally Posted by CosmosK View Post
    I found this older thread: link

    Based on recc's from that thread, I should be about .007" per rev. I also saw 35-50 SFM. I'm going to get a couple more cobalt jobbers and try again. 400 RPM, .0064" per rev pecking maybe 1/2". Thanks for the help.

    Last place I worked we ran tons of 17-4/15-5/13-8, drill were always Cobalt. Can't help on feeds/speeds though.

  15. Likes CosmosK liked this post
  16. #12
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    461
    Post Thanks / Like
    Likes (Given)
    99
    Likes (Received)
    123

    Default

    Got a couple new cobalt drills. Re-ran the ops with the slot, then changed drill in case the exit did something. Got through the holes, seemed fine:

    400 RPM, .0064" per rev (39 SFM). I used chip breaking macro every 10mm (retract 0.5mm not full). I started making some sounds the last few mm, I assume chips getting bunched up, but got through the holes.

    Thanks all for the help!

  17. Likes litlerob1, eaglemike liked this post
  18. #13
    Join Date
    Jan 2018
    Country
    UNITED STATES
    State/Province
    New Hampshire
    Posts
    35
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    19

    Default

    RC 35 is usually what we get at H1100, are you sure it's in solution A? It definitely likes being cut in a hardened state better. You really shouldn't have too much trouble drilling it with a half decent cobalt drill. We use a macro to dwell exactly 1.5 rev before retract for the peck and that works great for us even deep skinny holes.

  19. #14
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    133
    Post Thanks / Like
    Likes (Given)
    109
    Likes (Received)
    17

    Default

    I have had good luck on my cnc lathe running 17-4 H900 around 43r using I think a letter Q carbide drill from MariTool. I am running like 170sfm .0015 feed and pecking every .100 flood coolant with a total depth of around 5/8. Just got through with a 120pc run and the drill is still good.

    Carbide Screw Machine Drills (stub length) - MariTool

  20. #15
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    461
    Post Thanks / Like
    Likes (Given)
    99
    Likes (Received)
    123

    Default

    Quote Originally Posted by TCasals View Post
    RC 35 is usually what we get at H1100, are you sure it's in solution A? It definitely likes being cut in a hardened state better. You really shouldn't have too much trouble drilling it with a half decent cobalt drill. We use a macro to dwell exactly 1.5 rev before retract for the peck and that works great for us even deep skinny holes.
    report says solution annealed.. HB 313 which is around 33-34 Rc. I had looked around for bar stock in H1150 and couldn't find any. This is my first 17-4 job, so I probably need to find a better supplier. I got this material from online metals. The report says Bollinghaus Steel, South Africa.

    Yeah, I got a 4mm carbide drill and made some holes at 5200 RPM.. nice. It's a small job, so I'd like to get through it without the $80 drill. Seems to be working. Thanks

  21. #16
    Join Date
    Sep 2008
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,712
    Post Thanks / Like
    Likes (Given)
    1141
    Likes (Received)
    988

    Default

    Quote Originally Posted by TCasals View Post
    RC 35 is usually what we get at H1100, are you sure it's in solution A? It definitely likes being cut in a hardened state better. You really shouldn't have too much trouble drilling it with a half decent cobalt drill. We use a macro to dwell exactly 1.5 rev before retract for the peck and that works great for us even deep skinny holes.
    That's why some organizations (like NASA) don't like 17-4/15-5 H1150, because you can't do a hardness test and determine whether it's annealed or heat treated. Not an issue with H1025 (or standard ht) or H900

  22. Likes TCasals liked this post
  23. #17
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,640
    Post Thanks / Like
    Likes (Given)
    1222
    Likes (Received)
    2602

    Default

    Cosmo, just curious. In post #12 you said it sounds a little crunchy the last couple mm, you suspect it's chips. But you are using chip break Macro.

    Why aren't you just Peck Drilling, to get the chips out of the hole?

    Most of Machining, is generating a hard enough chips that it breaks off of the work piece. So the chips are hard. Even when they aren't hard, they're still the worst part of the Machining process (particularly when hole making). Get rid of them.

    I understand trying to reduce cycle time, but not if one hole takes 8 hours, because your brain is stuck doing it a certain way. Sometimes we kick our own asses.

    R

  24. #18
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    461
    Post Thanks / Like
    Likes (Given)
    99
    Likes (Received)
    123

    Default

    Quote Originally Posted by litlerob1 View Post
    Cosmo, just curious. In post #12 you said it sounds a little crunchy the last couple mm, you suspect it's chips. But you are using chip break Macro.

    Why aren't you just Peck Drilling, to get the chips out of the hole?

    R
    I didn't want to come down on a chip. I should probably have done full retract way back and blowgunned the hole between pecks. Time is not an issue. This job has eaten most of my week so far and it's not worth that much.

  25. #19
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,640
    Post Thanks / Like
    Likes (Given)
    1222
    Likes (Received)
    2602

    Default

    That is a reality also. Coming down on chips sucks too. But the breakage I see in your pictures looks to me like swarf in the same space as the Drill.

    But a part of the basic geometry of a Twist Drill, is to help chips come out of the hole when the Drill comes out. Like I said, sometimes I get so stuck with the original intent or plan of attack that it ends up bad for me. When stuff starts to get difficult, I try and take a step back and ask myself if this is the bast way, after all.

    R

  26. Likes CosmosK liked this post
  27. #20
    Join Date
    Jan 2018
    Country
    UNITED STATES
    State/Province
    New Hampshire
    Posts
    35
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    19

    Default

    Quote Originally Posted by triumph406 View Post
    That's why some organizations (like NASA) don't like 17-4/15-5 H1150, because you can't do a hardness test and determine whether it's annealed or heat treated. Not an issue with H1025 (or standard ht) or H900
    I suppose there's something to be said that we only ever see these figures on our HT certs when the material comes back, but I assumed cond. A was way softer. Definitely better ways to test it, but being obligated to charpy test our parts every time sucks too.

    OP, I would suggest finding a different supplier than online metals if you are doing any volume, but getting 17-4 in anything other than cond. A has been a crapshoot for us so far. We've just gotten used to shipping directly to our HT vendor.

  28. Likes CosmosK liked this post

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
  •