Help with a hole - High productive solution - Page 2
Close
Login to Your Account
Page 2 of 4 FirstFirst 1234 LastLast
Results 21 to 40 of 73
  1. #21
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    3,190
    Post Thanks / Like
    Likes (Given)
    877
    Likes (Received)
    1766

    Default

    Quote Originally Posted by bobbybrown23 View Post
    Speed= 1100 rpm
    feed= 50mm/rev
    peck amount= 1.5mm

    clearance value for each peck = 1mm
    Please revise 50mm per revolution.
    1100RPM is too slow it's 34 SFM
    I'm assuming "clearance" means how far out of the hole after each peck. Not clearance from Rapid to start feeding.


    You could double your chip time just by spindle speed. I wouldn't go over 75 SFM though. So 3.82x75/.118=2427RPM

    You're probably programming in IPM for the Feed, so keep in mind you need to change that, to reflect chipload per revolution, once you get that part figured out.

    R

  2. #22
    Join Date
    May 2008
    Country
    SOUTH AFRICA
    Posts
    1,476
    Post Thanks / Like
    Likes (Given)
    1058
    Likes (Received)
    607

    Default

    I agree with Rob on this one, your RPM is way low. As a rule of thumb in general mild steel I run 30M/min on HSS drills. That puts you in about the 3000 RPM range. I also don't understand your 50mm/rev, maybe it is 50mm/min? That is also a bit on the low side (0.05) but just for interest sake use the same chip load and bump the RPM up. So 3000 RPM and 135 mm/min. You might land up with chip wrapping at the lower feed but you are pecking at crazy small amounts so maybe not.

    I would personally spot drill, then push in a short 3mm drill, and then finish with your longer drill. If the longer drill didn't look too scary I would try it by just spotting and then going for it. Also I would not use a canned cycle. It is wasting your time. Write a sub program and make your own cycle. Start the hole off at a lower feedrate, to let it find the centre, and then go in about 10mm, peck but stay in the hole, then slowly start reducing your depth per peck and start fully retracting out the hole. If there are loads of holes to do this will save you a shitload of time.

    The drill that Teach put a link up to is probably your best bet at really getting that hole done quicker but without TSC you are probably going to struggle with that as well.

  3. Likes bobbybrown23 liked this post
  4. #23
    Join Date
    Mar 2011
    Country
    SWITZERLAND
    Posts
    924
    Post Thanks / Like
    Likes (Given)
    110
    Likes (Received)
    360

    Default

    Water jet takes about a second. A little circling added and you have a 3 mm through bore within tolerance.

    Waterjet Cutting Services in Florida (FL) on ThomasNet.com

  5. #24
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    413
    Post Thanks / Like
    Likes (Given)
    57
    Likes (Received)
    119

    Default

    Quote Originally Posted by TeachMePlease View Post
    Use the right drill. Like this one: CrazyDrill Cool XL 2 x d
    these drills are legit, ive also used the flat bottom ones to drill at a 30 deg angle thru titanium in the corner of a bore, paid for itself first run

  6. #25
    Join Date
    Dec 2004
    Location
    uk
    Posts
    13,171
    Post Thanks / Like
    Likes (Given)
    3853
    Likes (Received)
    6042

    Default

    Im a big believer these days in coatings in steel, if you compare a coated and uncoated drill the swaf is just ejected so much cleaner than with a bright or blued drill bit. You can see it on the flute side of the swaf, it has a lovely shine too it, this lessens heat generated through friction and lets you bump a little more speed. Speed can help with drilling as it throws the swaf at the side of the holes harder, which helps it climb up the flutes better.

    1100rpm is kinda too slow unless that metals dang hard, assuming your lower 30HRC or under 2k or more would be the first step. Bump it up and look at the swaf colour for true down hole temps as the guide. Yellow swarf is fine, a little blue on break through is also livable with, go much beyond a little blue and drill life really suffers.

    For that depth i would be going spot stub or jober length, then a long enough bit to get through, i probably would push the jobber or stub drill a lot harder than i would the longer one. Theres a lot of time to be saved in getting anal about the pecking and such if this is a long reoccurring run and the additional hand code work can really pay off in time saveings if this is a high quantity feature.

  7. Likes bobbybrown23 liked this post
  8. #26
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    2

    Default

    I'll try pushing in a short 3mm drill & then finishing off with a longer one. Kinda intrigued with parabolic drills, how effective are they? Do they need to peck?

    Also my shop-floor guy is saying that we're pushing the drill to the max regarding the feed & speed of 50mm/min & 1100 rpm.

  9. #27
    Join Date
    Dec 2004
    Location
    uk
    Posts
    13,171
    Post Thanks / Like
    Likes (Given)
    3853
    Likes (Received)
    6042

    Default

    Lots of people rate parabolic drills, maybe its me, but they have never impressed me, seam great in theory, just don't seam to deliver in practice for me at least in the gummy steel and aluminum i tried them in - normally get to cut. I bought a bunch of diffrent ones for a not overly deep 8mm hole and could never get as good a feed and speeds out of them as i could a nicely coated cobalt jobber drill.

    Look at the swaf thats coming out the hole, its the best guide as to how its really doing and if your any were near max. Way too many people seam to just base things on sound, the cuttings seam to get overlooked.

    One thing TomB is right about though, theres playing it safe and finding the limits, if you want to find the limits, the only way is to exceed them then back back off them. That means broken bits and possibly a few stuffed parts, for most of us, the savings can be more than great enough to cover those costs, if the parts your making are irreplaceable, its a different story. Here any hole going more than 5D deep i do expect to lose the odd part (5d less than 1% but im not crying when it happens) - bit, going your 16D deep, especially that small i would certainly want some kinda scrap allowance (in a hundred holes odds are getting prety good your going to have something fail especially dialing things in), especially if the goal is to dial things in for max production. certainly on the parts im doing it makes way more sense to chuck 3 in the bin in a hundred than it does to take twice as long doing them, your parts just like tomb's may be different and removing broken small drills deep down is a significant time and cost sink.

  10. #28
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    3,190
    Post Thanks / Like
    Likes (Given)
    877
    Likes (Received)
    1766

    Default

    Quote Originally Posted by bobbybrown23 View Post
    Also my shop-floor guy is saying that we're pushing the drill to the max regarding the feed & speed of 50mm/min & 1100 rpm.
    Show me the calculator that gives you 50mm per minute with a 3mm Drill going 1100 RPM!! There is nothing correct about that. IT isn't a guess. 1100 RPM with a 3mm Drill is 10 Meters per Minute (34 Inches per) you want to go 20 Meters per Minute (68 Inches), so double right?

    Sounds like your shop floor guy doesn't know what he is talking about, or there is some communication error. Until you get that fixed, I can't help.

    R

  11. Likes bobbybrown23 liked this post
  12. #29
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,775
    Post Thanks / Like
    Likes (Given)
    109
    Likes (Received)
    1234

    Default

    Quote Originally Posted by Mechanola View Post
    Water jet takes about a second. A little circling added and you have a 3 mm through bore within tolerance.

    Waterjet Cutting Services in Florida (FL) on ThomasNet.com
    50mm deep in steel? 1 second? That would be amazing.

    Regards.

    Mike

  13. #30
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,215
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2389

    Default

    1) very small dia drill bits usually do not do well at regular sfpm. for example if you normally use a certain sfpm then small dia drill bits usually use 20% less cause their small. sensitive to vibration, clogged chips, hardness variations, runout, etc
    .
    2) long length to dia ratio 20x or 30x usually back off feed another 20-50% cause long drill bits bend easy. vibrate easy. coolant has trouble reaching bottom of hole. long length to dia drill bits often need a sfpm/rpm reduction cause of random vibration resonance. not unusual to reduce rpm/sfpm to 50% of normal for vibration free drilling on 30x length to dia drill bits
    .
    3) using shorter pilot drill. got to watch that. if long drill is even .001" dia bigger than the short drill. the long drill will often random vibrate and break. many drill bits have a back taper and as they get resharpened the dia gets smaller. long drill bits make bad reamers
    .
    4) i record cutting tool parameters and record every sudden tool failure. if drill 10000003 is used i can look up last time i broke it at a certain feed and speed and what material being machined. like broke 1/16/2015, broke 5/26/2017, broke 6/12/2018..... i can easily scroll down down to a different feed and speed and see where no sudden tool failures occurred........ i find often 90% of sudden tool failures occur cause older cnc operator knows from experience to run say 80%rpm/50% feed for some tools and the new guy running 100/100% is breaking multiple tools cause he didnt notice the programmer who wrote program. 99.999% the guy running 100% breaking tools is taking longer dealing with the broken tools than the old guy going slower not breaking tools
    .
    literally some programmers you see their name and automatically got to check the whole program for obvious apprentice stuff or unrealistic expectations. personal experience is that experienced cnc operators always look at who wrote the program. you want to be like the maytag repairman everything working no problems got nothing to do but wait. i have often spend 2 to 10 hours dealing with a broken drill bits. unless you making cheap <$100. parts it cost a lot of money dealing with broken tooling.

  14. #31
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    3,190
    Post Thanks / Like
    Likes (Given)
    877
    Likes (Received)
    1766

    Default

    Tom, I'm tired of trying to help you understand, so I won't.

    BUT those values apply to you, in your shop, according to your spreadsheet. They aren't Universal truths for every man in every shop, every time with every Tool.

  15. Likes Mtndew liked this post
  16. #32
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    460
    Post Thanks / Like
    Likes (Given)
    359
    Likes (Received)
    245

    Default

    Quote Originally Posted by DMF_TomB View Post
    3) using shorter pilot drill. got to watch that. if long drill is even .001" dia bigger than the short drill. the long drill will often random vibrate and break.
    .001" is a huge variance on a drill diameter. You using drills from China or something? Use a quality carbide pilot and a quality carbide deep hole drill and it works wonderfully every time. I do it frequently and never had a problem. That is, buy the way, the cutter manufacturer's recommendation.

  17. #33
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,077
    Post Thanks / Like
    Likes (Given)
    3582
    Likes (Received)
    2366

    Default

    Quote Originally Posted by DMF_TomB View Post
    i have often spend 2 to 10 hours dealing with a broken drill bits.
    Then you clearly don't refer to your super duper spreadsheet data on drilling.
    Personally I can't recall EVER spending 10 hours on a fucking broken drill.
    But feel free to ramble on again and never once address the original question as usual.

  18. #34
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,215
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2389

    Default

    Quote Originally Posted by mhajicek View Post
    .001" is a huge variance on a drill diameter. You using drills from China or something? Use a quality carbide pilot and a quality carbide deep hole drill and it works wonderfully every time. I do it frequently and never had a problem. That is, buy the way, the cutter manufacturer's recommendation.
    .
    many carbide drill bits have a back taper or are smaller toward the shank. i have seen carbide drill bits .020" smaller at the shank before. so when drill bit resharpened the drill tip was .001" smaller diameter.
    .
    the carbide drills are often made with the back taper so they drill a smoother more precise hole at faster feeds, often 10x faster feeds. the higher quality (they were German made)and more expensive drill bits often has this back taper far more back taper than cheaper drill bits. sure many apprentices might not realize drill bits often have back taper, some types have a lot of back taper
    .
    i have often seen pilot hole made 4" deep and the 18" long flute drill that followed vibrate badly in the .001" small pilot hole. no feed or speed change will help with the vibration usually. got many records of different settings tried. record shows drilled pilot hole redrilled .001" bigger dia and often the longer drill can go at 200% faster feed.
    .
    also deeper holes drilled often hole made not straight its curved at it meets hardness variations. any experienced lathe or mill guy will tell you deep holes not always perfectly centered at the bottom. a long length to dia ratio drill bit in a curved hole can experience a random vibration resonance. that is 9 holes drilled no problem and 10th hole has problems cause hole curved, drill starts vibrating.
    .
    if you got a record of over 10,000 cutting tool parameters and every day you record any differences or problems you basically can learn from previous experiences rather than randomly repeat mistakes of the past.
    .
    like i said i can look up tool 10000003 and see the record of sudden tool failures , multiple sudden tool failures generally indicates not the best feeds and speeds. everyday i look up tool history and add to tool history. usually better to learn from past experiences rather than repeat the same problems. problems that happened over a year ago are often forgotten. records can show problems going back decades and the last 1000 times the tool was used

  19. #35
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,215
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2389

    Default

    Quote Originally Posted by Mtndew View Post
    Then you clearly don't refer to your super duper spreadsheet data on drilling.
    Personally I can't recall EVER spending 10 hours on a fucking broken drill.
    But feel free to ramble on again and never once address the original question as usual.
    .
    $10,000 part if it got a broken drill bit in it you get it out even if it takes 10 hours. obviously many parts that are scrapped can take even 10 hours to remake. most parts i make are in the $1000 to $50,000 range or at least the last 5000 parts i have made are in that price range. most parts have 10 to over 100 labor hours to make many parts
    .
    about once a year i have to deal with broken drill bits. last time i spent 2 hours getting a broke carbide drill out of a part. obviously its in the work log for that particular part and i could look up the date and time of day it happened. along with the reason it broke and the corrective action taken to prevent it happening again of course

  20. #36
    Join Date
    Dec 2004
    Location
    uk
    Posts
    13,171
    Post Thanks / Like
    Likes (Given)
    3853
    Likes (Received)
    6042

    Default

    Quote Originally Posted by mhajicek View Post
    .001" is a huge variance on a drill diameter. You using drills from China or something? Use a quality carbide pilot and a quality carbide deep hole drill and it works wonderfully every time. I do it frequently and never had a problem. That is, buy the way, the cutter manufacturer's recommendation.
    Yes, but if you look at most manufacturers websites, you will see they only allow downloading thoes kinda cutting parameters as PDF's not XLS files, so they can not be right.

    Dont forget, Photos of bad Crashes his post number 6, after that you too would probaly think long drills are out to get you!

  21. #37
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    460
    Post Thanks / Like
    Likes (Given)
    359
    Likes (Received)
    245

    Default

    Quote Originally Posted by DMF_TomB View Post
    .
    many carbide drill bits have a back taper or are smaller toward the shank. i have seen carbide drill bits .020" smaller at the shank before. so when drill bit resharpened the drill tip was .001" smaller diameter.
    Then you're using an out of spec tool. If your resharpened drill is undersized it's no good, it's now the next smaller size drill and is the WRONG TOOL even if it has the same part number in your tooling inventory system or spread sheet.

    If you resharpen a 5/8" endmill several times until it's 1/2", do you expect it to perform the same job as a new 5/8" endmill? I had a boss several years ago that did that very thing, and he's out of business.

  22. #38
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,077
    Post Thanks / Like
    Likes (Given)
    3582
    Likes (Received)
    2366

    Default

    Quote Originally Posted by DMF_TomB View Post
    .
    $10,000 part if it got a broken drill bit in it you get it out even if it takes 10 hours. obviously many parts that are scrapped can take even 10 hours to remake. most parts i make are in the $1000 to $50,000 range or at least the last 5000 parts i have made are in that price range. most parts have 10 to over 100 labor hours to make many parts
    .
    about once a year i have to deal with broken drill bits. last time i spent 2 hours getting a broke carbide drill out of a part. obviously its in the work log for that particular part and i could look up the date and time of day it happened. along with the reason it broke and the corrective action taken to prevent it happening again of course
    You STILL don't get it do ya?
    With all of your spreadsheet data, why are you even breaking drills? I mean you are the one who knows everything.

  23. #39
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    6,732
    Post Thanks / Like
    Likes (Given)
    290
    Likes (Received)
    5495

    Default

    Quote Originally Posted by DMF_TomB View Post
    .
    the carbide drills are often made with the back taper so they drill a smoother more precise hole at faster feeds, often 10x faster feeds. the higher quality (they were German made)and more expensive drill bits often has this back taper far more back taper than cheaper drill bits. sure many apprentices might not realize drill bits often have back taper, some types have a lot of back taper
    .
    All drills HSS and carbide are circle ground with a backtaper.
    And you do this on centerless but need you a straight shank portion. Figure this one out.
    Bob

  24. #40
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    3,190
    Post Thanks / Like
    Likes (Given)
    877
    Likes (Received)
    1766

    Default

    Quote Originally Posted by CarbideBob View Post
    All drills HSS and carbide are circle ground with a backtaper.
    And you do this on centerless but need you a straight shank portion. Figure this one out.
    Bob
    I can't figure that out, that's why we have you

    Just curious Bob, what is the accepted Ratio for back taper on Drills? I'm sure it changes with type, length, material, or other things, but is there a way to quantify what to expect?

    Also your opinion on Parabolic Drills. I'm with Adama, I've never had great luck with them, the web/core seems too flimsy for deep holes.

    R


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