Help with a hole - High productive solution
Close
Login to Your Account
Page 1 of 4 123 ... LastLast
Results 1 to 20 of 73
  1. #1
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    2

    Default Help with a hole - High productive solution

    Application: Hole size Ø3mm, Length= >50mm.
    Currently using a HSS-E drill with pecking, but unfortunately the cycle time using this is very high.
    Can you guys suggest a more high-productive alternative to this?

  2. #2
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,776
    Post Thanks / Like
    Likes (Given)
    109
    Likes (Received)
    1234

    Default

    How long per hole?
    Machine?
    Material?

    Regards.

    Mike

  3. #3
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    2

    Default

    Quote Originally Posted by Finegrain View Post
    How long per hole?
    Machine?
    Material?

    Regards.

    Mike
    3-4 min per hole.

    Material: Alloyed Steel

    Machine: VMC

  4. #4
    Join Date
    Oct 2005
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    11,992
    Post Thanks / Like
    Likes (Given)
    18503
    Likes (Received)
    6285

    Default

    Gun drill, hi-pressure coolant, no peck

  5. Likes jancollc, KFALCON954, adama liked this post
  6. #5
    Join Date
    Jan 2013
    Location
    Plainfield, Indiana, USA
    Posts
    1,617
    Post Thanks / Like
    Likes (Given)
    1181
    Likes (Received)
    845

    Default

    Coolant thru drill; prolly need at least 200 psi thru spindle coolant.

  7. #6
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,217
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2389

    Default

    depends on cost of part and if drill breaks does that scrap part and require another part made.
    .
    if it takes a hour to remake a part and the cost and time to replace broken drill is over $10. than 3 minutes drilling aint bad.
    .
    i have seen reduce drilling time 2 minutes. then spend hours remaking 10% of parts and over hour wasted and over $100. replacing broke tooling and data often says total time loss at end of year is 20 minutes per part increase in time trying to drill faster trying to save 2 minutes a part.
    .
    just saying often when you look at actual time and costs at the end of the year its often surprises some. sometimes a less than 2% sudden tool failure rate can be increasing costs 10% or more per part even when it might happen on only 2 parts per 100 parts
    .
    i have seen many a time a 10% increase in feed or increasing peck distance then sudden tool failure rate increases to 2% of parts. unless data recorded its often written off as a unimportant and rare failure. often takes some studying of actual costs at end of year to realize how big a problem it is.

  8. #7
    Join Date
    Feb 2014
    Location
    Sunny South West Florida, USA
    Posts
    2,261
    Post Thanks / Like
    Likes (Given)
    9198
    Likes (Received)
    2654

    Default

    Use the right drill. Like this one: CrazyDrill Cool XL 2 x d

  9. Likes tay2daizzo8 liked this post
  10. #8
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    634
    Post Thanks / Like
    Likes (Given)
    45
    Likes (Received)
    223

    Default

    Quote Originally Posted by bobbybrown23 View Post
    3-4 min per hole.

    Material: Alloyed Steel

    Machine: VMC
    What alloy? What hardness?

    What speeds/feeds are you using currently?

    While "VMC" tells us you're doing it in a mill, you'd need to say whether through spindle coolant is available to you, and if you have high pressure (200+ psi) for it. Or if you're running on a Haas minimill with mist coolant.


    Because you're gonna get suggestions for TSC drills, and people gotta know if you can actually use them.


    Assuming something like 4140 with HSS, I'd probably be in the 2500rpm territory, maybe 3000. .0015/.002" (.05mm) per rev, maybe a .060" (1.5mm) peck. Gibbscam tells me that'd take 35 seconds at 2" deep... I'd think more like 40 depending on your rapids.

    (at that depth I'd drill 3/4" deep with a shorter drill to keep it from walking too far, so maybe add some time for a tool change)


    You could go faster than that with cobalt. and even faster with carbide/carbide tipped w/ TSC...


    Post your parameters.

  11. #9
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,079
    Post Thanks / Like
    Likes (Given)
    3582
    Likes (Received)
    2366

    Default

    Quote Originally Posted by bobbybrown23 View Post
    3-4 min per hole.

    Material: Alloyed Steel

    Machine: VMC
    Ok, I realize you're new here. But you need to give us more information if you want actual help or else you'll get 1,000 different answers that may or may not help you.
    What machine?
    What is your maximum spindle speed?
    Do you have thru-spindle coolant?
    What material? .... alloyed steel isn't good enough, there are literally too many kinds of alloyed steel to give you any decent answer.
    And a word of advice, don't listen to dmftomb...all that guy does is ramble on and thinks his little quips of wisdom help everyone.

  12. #10
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,217
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2389

    Default

    Quote Originally Posted by bobbybrown23 View Post
    Application: Hole size Ø3mm, Length= >50mm.
    Currently using a HSS-E drill with pecking, but unfortunately the cycle time using this is very high.
    Can you guys suggest a more high-productive alternative to this?
    .
    as the length to diameter ratio of drill increases you often can get a random vibration resonance going 10x more than normal which breaks drill bits. that is often the rpm is limited not by heat level of the drill bit material but the vibration limit of the drill bits length to diameter ratio
    .
    feed also is limited by length to diameter ratio. push a long drill at too high a feed and it bends. if bend starts rotating vibration often increases 10x and drill breaks
    .
    when near limits often you get what appears to be a random drill bit breaking. bigger drills you can easily hear the increased vibration. little ones often cannot easily hear. just saying when records are kept often you see a pattern of sudden tool failures over months and years that go unnoticed when you are near the feed and speed limits. sudden tool failures rarely are 100% failure on every hole

  13. #11
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    2

    Default

    Sorry guys, but I'm pretty new to the whole machining scene..thanks for your replies!
    Material is similar to SAE 5120
    No TSC I'm afraid, max spindle speed is around 8K

  14. Likes Mtndew liked this post
  15. #12
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    2

    Default

    I'll get back with the parameters in a bit

  16. Likes Mtndew liked this post
  17. #13
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,079
    Post Thanks / Like
    Likes (Given)
    3582
    Likes (Received)
    2366

    Default

    Quote Originally Posted by bobbybrown23 View Post
    I'll get back with the parameters in a bit
    If you can, also tell us your current speeds,feeds and peck amount for the drill you're currently using.
    I assume it's just your everyday uncoated hss jobber drill? You never know, all you might need is a tweak here and there to get where you want to be.
    It won't be optimal of course since you don't have TSC.

  18. #14
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    3,190
    Post Thanks / Like
    Likes (Given)
    877
    Likes (Received)
    1767

    Default

    "HSS-E" is Cobalt

    Spot. (optional)
    Stub length.
    Jobber length.

    Flood coolant.
    2500 RPM
    .0036 per rev (.0018 per flute)
    .06" peck once you switch to Jobber length. .1" with stubby.

    That is about the maximum on the parameters, with what you have available.

    R

  19. Likes Mtndew, bobbybrown23 liked this post
  20. #15
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,217
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2389

    Default

    Quote Originally Posted by litlerob1 View Post
    "HSS-E" is Cobalt

    Spot. (optional)
    Stub length.
    Jobber length.

    Flood coolant.
    2500 RPM
    .0036 per rev (.0018 per flute)
    .06" peck once you switch to Jobber length. .1" with stubby.

    That is about the maximum on the parameters, with what you have available.

    R
    9 ipm feed with a 3mm drill drilling 50 mm deep ?? so drill sticking out of tool holder at least 60mm ? at 9 ipm feed ?

  21. #16
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    6,100
    Post Thanks / Like
    Likes (Given)
    293
    Likes (Received)
    2548

    Default

    You could also call Guhring tech support, they have a wide range of drills and are pretty knowledgeable and helpful. They can also direct you to someone who stocks what you need.

  22. Likes Mtndew liked this post
  23. #17
    Join Date
    Mar 2018
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    38
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    12

    Default

    I use Guhring parabolic drills for going deep for diameter plus use a short drill first to start hole straight.

  24. Likes Mtndew, bobbybrown23, michiganbuck liked this post
  25. #18
    Join Date
    Sep 2009
    Location
    barcelona, spain
    Posts
    2,286
    Post Thanks / Like
    Likes (Given)
    464
    Likes (Received)
    1273

    Default

    A high quality parabolic drill might speed it up.
    Perhaps over 50%.
    You might use a short drill to some depth, then another to finish the hole.

    As was said breakage and parts cost might be important, or not.

    S:
    Ask iscar to help and bring drills to try.
    Drill sample holes in one sacrificial part of same material to prove the process, with iscar present.

    As was said, don´t try for top speed.
    If 35 secs/part is achievable, 80 secs might be much more stable, and usually less tool wear.

    The HSS drill probably heats in the hole in 3 mins.
    This heats it, jamming it more.
    Exponential heat/friction occurs.

    S:
    Could you dam the part via say plastic walls, flooding it under coolant.
    This might allow pecks to keep the drill cool.

    S:
    Or perhaps full retracts on pecks vs short rapid pecks.
    This might allow evacuating chips better.
    A VMC can retract the drill really fast, and you wont lose time, but the hole gets evacuated and the drill tip gets cooled.

    S:
    Is the hole anywhere near straight uniform and cylindrical ?
    Gage pins or shop built gages can easily show you if it is somewhat straight.
    Or drill rod of 3 mm, and another of say 3.05 mm, -- 0.01 mm incremental for a no-go.

    3 mm is very flexible and can only take little push, and HSS is relatively limp spaghetti.

    I am pretty surprised and very impressed if the hole is anywhere near straight, uniform and cylindrical.
    Please let me know where do buy, what drills, if the holes are straight (ish).


    The stock answer is solid carbide drills.
    And perhaps bore the start by about 3-4 D or about 12 mm in this case after stub predrilling about 2.7 mm D.

    With a say 8 sec toolchange, you are maybe 8 drill + 8 + 8 bore + 8 + final drill == 30 secs, 62 secs total.
    The bore would support the drill and tend to reduce breakage.
    The start would be very straight and uniform.

    A bored start hole, or perhaps just solid carbide stub drill, might reduce breakage to near zero.

    My SWAG is around 90 secs, bit less, is somewhat easy to achieve with good reliability re: tool breakage.
    My SWAG is that somewhere under 60 secs is doable if you really tune and test the process and some breakage is acceptable.

    How will you detect broken drills with short cycle times ?
    Could you contact probe, perhaps independently, via the part and FH or stop or estop as needed via a relay.

    The O. post was about production, and these types of things tend to come up.
    Imho, imhe.
    Just throwing things out there, that might perhaps help.

    Weather you are doing pallets of 400 parts, or one at a time, and they need accurate fixturing, or not, and you have a Heller or top japanese machine, or a Johnford etc. may affect the best minimax.
    2000 / week or 4000 may be a major critical path issue.

    Since you did not mention it I expect hole accuracy is not an issue at this time.
    This is unusual and surprising with HSS at 17D deep drilling into alloy steel.

    If the hole is a clearance hole or assy hole of no particular accuracy ...
    .. and the part is not particularly expensive, so wastage is ok, ..
    fast drilling with solid carbide, maybe deep pecks to clear chips under coolant, might be the right route.

    If you are really doing production volumes, you can easily add through-tool coolant to the machine for a few thousand.
    This should reduce times by maybe 30-40 secs from 90 ish to 50 ish.
    So 2-3000 / week could become 5500 / week.
    But the hole alone may not be the bottleneck at 5k, or maybe it is.

    At 3 mins/hole, thats 200 parts max per day/11-12 hours, or 1000 ish/wk.
    At 90 secs, potentially 2000 /wk.
    At 35 secs, 5000 theoretical.

  26. Likes bobbybrown23 liked this post
  27. #19
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    634
    Post Thanks / Like
    Likes (Given)
    45
    Likes (Received)
    223

    Default

    I was about to turn off the computer for the night when I had a thought for the OP:

    I am assuming you are using G83 peck drilling cycle. You haven't mentioned your speeds/feeds and peck yet, but I am assuming you have a relatively short peck.

    my question to you is (and you probably don't know, so you'll have to do a bit of investigation into parameters and/or look at the position page when it does pecks) what is the "clearance" value for each peck?

    Peck drilling cycles peck a certain depth (Q for fanuc controls), retract (up to your rapid plane for G83), then go back down into the hole, usually a small amount above the last depth.

    If the clearance value is set pretty high, you're gonna have a much longer cycle than you really should

    Most of our older machines had default values of .100" (thats 2.5mm) clearance. Meaning it would cut .100" of air EVERY PECK. I'd say set it to .010" or so for your size drill (drilling things like Titanium/stainless with bigger drills, you'd want a bit larger of a value.

    Just something to look at if you're scratching your head wondering why it is taking too long....

  28. Likes bobbybrown23, Mtndew, aarongough liked this post
  29. #20
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    2

    Default

    Quote Originally Posted by bobbybrown23 View Post
    I'll get back with the parameters in a bit
    Speed= 1100 rpm
    feed= 50mm/rev
    peck amount= 1.5mm

    clearance value for each peck = 1mm


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
  •  
2