Drilling 20mm in mild steel tips
Close
Login to Your Account
Results 1 to 20 of 20
  1. #1
    Join Date
    Nov 2011
    Location
    Sussex, UK
    Posts
    19
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Drilling 20mm in mild steel tips

    Hi guys,
    Have a Hurco VM10 (quite a small mill) and need to drill 20mm x 40 deep into 140 off Mild Steel billets.
    Would you guys use a series of drills working up to 20mm or just spot and then straight to it?
    It’s a good quality HSS bit but have no through coolant on machine.
    Thanks in advance.

  2. #2
    Join Date
    Jan 2019
    Country
    SWEDEN
    Posts
    190
    Post Thanks / Like
    Likes (Given)
    56
    Likes (Received)
    22

    Default

    Just spot and boom. The general rule is high speed low feed. For HSS that means low speed lower feed. 20mm 40mm deep is cake. Vc ~30, G83 cycle, peck every five millimeters or so (I know that's super chicken but think of it as a starting point,) feed rate .15 to test the waters then 0.2. Mild steel is 80%+ of what I run.

    ETA: Got head stuck in my ass removed faulty info.
    Last edited by Tichy; 11-17-2019 at 05:19 AM.

  3. #3
    Join Date
    Jan 2013
    Location
    Plainfield, Indiana, USA
    Posts
    1,737
    Post Thanks / Like
    Likes (Given)
    1313
    Likes (Received)
    926

    Default

    Not familiar with that mill, but an 8 or 10 mm pilot drill should help drill on size and lower power requirements.

  4. #4
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,104
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2625

    Default

    Quote Originally Posted by newtoid1986 View Post
    Hi guys,
    Have a Hurco VM10 (quite a small mill) and need to drill 20mm x 40 deep into 140 off Mild Steel billets.
    Would you guys use a series of drills working up to 20mm or just spot and then straight to it?
    It’s a good quality HSS bit but have no through coolant on machine.
    Thanks in advance.
    .
    most important thing is length of drill bit stickout and length of tool holder. obviously depending on part and setup you might need a long drill to reach even when hole is not that deep. or you might only have long length drill bits available
    .
    longer drill bends easily obviously so hole not straight and drill can break easier
    if you use 364 rpm at 75mm/m feed you will need about 1.8hp, obviously if you use higher feed you have to think about
    .
    1) spindle stalling or rpm slowing down or unstable rpm
    2) drill bit bending
    3) drill bit vibration increases with drill bit length usually
    4) hole oversize amount
    5) hole straightness
    6) sudden tool failure and part damage and machine damage
    7) drill thrust or force on the part can bend part or move part depends on setup
    .
    chips wrapping around drill bit can be a problem, if you cannot stop and manually pull them off the flutes. pecking helps but stubborn chips often require a backwards CCW rotation and strong coolant flow after drilling to help unwind chips off drill bit. that is if you want chips removed automatically rather than manually pull them off
    .
    usually many create a database of a standard tool setup that is tool length tool holder length etc to standardized tolerances then record part material and feeds and speeds tried and record any sudden tool failures over the years and 1000's of holes drilled. then you can see what feeds and speeds cause more sudden tool failures and massive costs of part damage and machine damage. that is if going faster trying to save 2 minutes a hole is causing 20 hours extra rework a year or adding 6 minutes a hole in rework than often going slower is actually faster
    .
    many a long drill or a deep hole needs maybe different feeds and speeds for higher reliability. most start with moderate settings rather than take a chance with even a 2% sudden tool failure rate. 2% is like every 100 car trips you get into 2 car crashes requiring towing the car and $10,000's in repair costs. 2% can be a lot. obviously if part cost over $10,000. and a week of labor into it you have to be more concerned about not damaging the part if sudden tool failure occurs. or would boss be upset if part was scrapped. telling the boss you scrapped a part trying to save 2 minutes drilling time usually doesnt go over very good.

  5. #5
    Join Date
    Jan 2019
    Country
    SWEDEN
    Posts
    190
    Post Thanks / Like
    Likes (Given)
    56
    Likes (Received)
    22

    Default

    Quote Originally Posted by DMF_TomB View Post
    longer drill bends easily obviously so hole not straight and drill can break easier
    if you use 364 rpm at 75mm/m feed you will need about 1.8hp
    A new Hurco VM10i provides 15hp power and 65nm torque; should be no problem for him to run a 20mm HSS drill at any speed it can take.

  6. #6
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,728
    Post Thanks / Like
    Likes (Given)
    1539
    Likes (Received)
    1764

    Default

    Quote Originally Posted by newtoid1986 View Post
    Hi guys,
    Have a Hurco VM10 (quite a small mill) and need to drill 20mm x 40 deep into 140 off Mild Steel billets.
    Would you guys use a series of drills working up to 20mm or just spot and then straight to it?
    It’s a good quality HSS bit but have no through coolant on machine.
    Thanks in advance.
    Download the free trial of HSM advisor to get you started.
    Advanced CNC Speed And Feed Machinist Calculator - HSMAdvisor

    I think some of their feeds/speeds are a little aggressive (keep in mind your machine-setup rigidity when using the calculator), BUT it will get you in the ballpark and you can easily compare speeds/feeds for different materials so you start to understand what is/isn't appropiate...

    Quote Originally Posted by Tichy View Post
    Just spot and boom. The general rule is high speed low feed. For HSS that means low speed lower feed. 20mm 40mm deep is cake. Vc ~30, G83 cycle, peck every five millimeters or so (I know that's super chicken but think of it as a starting point,) feed rate .15 to test the waters then 0.2. Mild steel is 80%+ of what I run. Think you'll end up with something like 600RPM F120.
    What? 120ipm mmpm...? Either way tooooooo fast.

  7. #7
    Join Date
    Jan 2019
    Country
    SWEDEN
    Posts
    190
    Post Thanks / Like
    Likes (Given)
    56
    Likes (Received)
    22

    Default

    Quote Originally Posted by Mike1974 View Post
    What? 120ipm mmpm...? Either way tooooooo fast.
    Hum well that's embarrassing. Recalculating (Vc30 F.15-.20) I end up with 478RPM and F72 as a starting value with potential for around F95. (mm/min) A good HSS drill should be capable of that depending on the quality of the material.

    Not quite sure how I managed to screw that up, guess I have to blame the beer.

  8. #8
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,561
    Post Thanks / Like
    Likes (Given)
    1204
    Likes (Received)
    2540

    Default

    Why the fuck are you two talking Inches and mm, in the same thread? It's too time consuming to track. Brits use Inches too, it's okay.

    OP, I'd start at 350 SFM (1698 RPM). I would go with a .012" chip load (.787"×.0156"×2 flutes=.0236"). With that you'll end up with 40 IPM.

    JMO

    R

  9. #9
    Join Date
    Jan 2019
    Country
    SWEDEN
    Posts
    190
    Post Thanks / Like
    Likes (Given)
    56
    Likes (Received)
    22

    Default

    Quote Originally Posted by litlerob1 View Post
    OP, I'd start at 350 SFM (1698 RPM).
    ?!

    Well, that's... ambitious

  10. Likes Bobw liked this post
  11. #10
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,687
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1449

    Default

    Quote Originally Posted by litlerob1 View Post
    OP, I'd start at 350 SFM (1698 RPM). I would go with a .012" chip load (.787"×.0156"×2 flutes=.0236"). With that you'll end up with 40 IPM.

    JMO

    R
    Hello Rob,
    You do realize the OP is talking HSS drill and Mild Steel workpiece material?

    Regards,

    Bill

  12. #11
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,561
    Post Thanks / Like
    Likes (Given)
    1204
    Likes (Received)
    2540

    Default

    Ha!!

    I thought "mild steel" meant Butter, that's all.

    R

    So 100 SFM (485 RPM). Same chipload, so 11 IPM.

  13. #12
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    270
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    86

    Default

    I'd try 473 rpm and 165mm/min (6.5ipm) This is approximately 2.28kw. You're only at two diameters depth so try no pecking to start. You should be producing a pretty good chip, though it may not break on it's own. If you're getting a little wrap around try one high speed peck (G73) a little over halfway down and see if that solves any chip control problems. At this depth the chips should find there way out without a full retract. If one peck doesn't work try two. Can't imagine you'd ever need more at this depth. BTW these suggestions are with coolant applied externally.

    Dave

  14. #13
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    1,020
    Post Thanks / Like
    Likes (Given)
    210
    Likes (Received)
    618

    Default

    450 rpms and 3.0 ipm with a chip break cycle every .07 and done


    Sent from my iPhone using Tapatalk Pro

  15. #14
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    270
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    86

    Default

    Quote Originally Posted by D Nelson View Post
    450 rpms and 3.0 ipm with a chip break cycle every .07 and done
    With a 0.100 clearance plain and a tip length of 0.236 (118 deg) and an after the hole thru length of 0.075 you're looking at 1.986" of tool travel per hole. This suggestion equals 29 pecks for a single hole AND a 0.0067 ipr which is a tiny chip load for a drill this size. I'm sorry D Nelson... you're out of your mind!

    Been watching too many NYC-CNC videos? :-)

    Dave

  16. #15
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,728
    Post Thanks / Like
    Likes (Given)
    1539
    Likes (Received)
    1764

    Default

    Quote Originally Posted by 13engines View Post
    With a 0.100 clearance plain and a tip length of 0.236 (118 deg) and an after the hole thru length of 0.075 you're looking at 1.986" of tool travel per hole. This suggestion equals 29 pecks for a single hole AND a 0.0067 ipr which is a tiny chip load for a drill this size. I'm sorry D Nelson... you're out of your mind!

    Been watching too many NYC-CNC videos? :-)

    Dave
    Maybe being a bit anal about semantics, but a chip break does not retract out of the hole in my world. A peck drill does.

    I agree .07("?) is awfully light, but the drill is only retracting .01" or so depending on how your machine is configured...

  17. Likes TeachMePlease liked this post
  18. #16
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    270
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    86

    Default

    Quote Originally Posted by Mike1974 View Post
    Maybe being a bit anal about semantics, but a chip break does not retract out of the hole in my world. A peck drill does.

    I agree .07("?) is awfully light, but the drill is only retracting .01" or so depending on how your machine is configured...
    To be honest, I wasn't considering whether it was chip breaking or full retract. In this situation, just 29 of anything is off the charts if you ask me. Maybe if you were running lights out and absolutely positively couldn't have a chip wrap of any kind. (Besides the fact you wouldn't be using a standard drill bit anyway.) But come on... we're talking a two diameter deep hole here. A well played drill feed/speed setup has a descent chance of not needing any pecks at all. Though granted you may end up with some big gnarly chips to deal with. Like my original suggestion said, a couple chip breaks may be needed... tops. If anything just to keep your chip conveyor from clogging up if you have one.

    To each their own for sure, though I thought the 0.07" suggestion was way off the mark. (Let alone the feed rate.) I'm older-ish and can forget things, yet I can't recall using more then 6-12 pecks/chip breaks in my life.

    Dave

  19. #17
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    1,020
    Post Thanks / Like
    Likes (Given)
    210
    Likes (Received)
    618

    Default

    I have to chip break or the material ends up all around the bit at that size but all shut up and let you have at it


    Sent from my iPhone using Tapatalk Pro

  20. #18
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    270
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    86

    Default

    Quote Originally Posted by D Nelson View Post
    I have to chip break or the material ends up all around the bit at that size but all shut up and let you have at it
    Hi DNelson,

    Sorry but didn't mean to ream you out. If you were standing here in my shop and I walked up to you machining this in the way that was described, I would have giving more of a ribbing then a calling out. We're all just trying to do things the best we can. Basically I'd offer some suggestions and see what you thought. It would be easy enough in the immediate aftermath to see who had the better solution to getting the job done. And it wouldn't surprise me at all if it was some combination of both of our ideas. I'm no mister-know-it-all, and have certainly had my path straightened out by others plenty of times.

    Maybe you know this already, but I'd like to offer a generalization about drilling. If you're getting rat nests around your drills in any continuous chip material, the number one reason is going to be too slow of feed. 3ipm at 450rpm (0.0067 ipr) is below what I would consider the very minimum feed for a 20mm drill in mild steel. I'd say the range is anywhere from about 0.009 ipr at the very least, all the way up to 0.02 ipr if the stars were aligned. Anyway... next time you notice a bit of rat nesting going on, give that feed dial a couple three clicks to start and see what happens. If you have horsepower limitations, then that's a whole other deal. Regardless... have a nice day.

    Dave

  21. #19
    Join Date
    Jan 2019
    Country
    SWEDEN
    Posts
    190
    Post Thanks / Like
    Likes (Given)
    56
    Likes (Received)
    22

    Default

    Quote Originally Posted by 13engines View Post
    Maybe you know this already, but I'd like to offer a generalization about drilling. If you're getting rat nests around your drills in any continuous chip material, the number one reason is going to be too slow of feed.
    Correct. I see this using SC all the time. I run my 5.0mm drills at .17 feed in mild steel with only air coolant. They work and they don't break.

    This puts me at odds with the common wisdom at my workplace being "high speed low feed" for mild steel. Somewhat.

    I have not tried this approach with HSS tools. When the OP asked for advice about HSS I thought "let's give him something safe to start with." Reason being I don't use HSS for production in anything but aluminum and plastic if I can avoid it, well, except taps.

    However I'm very interested in learning more.

  22. #20
    Join Date
    Nov 2011
    Location
    Sussex, UK
    Posts
    19
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Thanks for all the advice guys. I’ve taken all of it on board and decided to splash out on a solid carbide drill. 800 RPM and 240mm / min from WNT. Decent sized chips flying out.
    40 parts so far and the drill stills looks new. Spindle load hits 100% out of 150% but no stalling issues.


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
  •