584,866 active members*
5,132 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking > MetalWork Discussion > Trying to drill many #8 holes.
Results 1 to 16 of 16
  1. #1
    Join Date
    Aug 2005
    Posts
    300

    Trying to drill many #8 holes.

    Hi,

    I am trying to drill many holes through .500 thick 12L14 with a #8 drill using a Tormach PCNC1100 milling machine. I am running the spindle 1800 RPM's amd feeding 4.5 IPM. The holes are larger at the top (drill entry side). What am I doing wrong?

    Thanks,

    ErnieD

  2. #2
    Join Date
    Jan 2007
    Posts
    1389
    are you spot drilling them first? if you are then you have a bad drill.
    if your peck drilling your drill has run out, is not centered or you have a bad drill.

    how much bigger whats your tolorance? 12L14 cuts like butter

  3. #3
    Join Date
    Apr 2008
    Posts
    3

    many # 8 holes

    Hi my name is Jerry and I am new to this forum. I am just starting my apprenticeship in the field and dont know much. But I would say that your bit is brobably dull, causing slow feed and It may be walking toward the top of the hole causing it to be bigger. Have you tried putting a split point on the bit?

  4. #4
    Join Date
    Dec 2007
    Posts
    617
    Hi: Rule of thumb: anything deeper than 3D of drill is considered to be a deep hole... you could center drill with a #0 center drill, then drill peck your way through with a high quality, yes high quality drill. the split point is only an advantage if you choose to ignore center drilling.Small drill, high speed, low feed...no frr lunch in the universe for precision.
    The rule of 3D rears it's ugly head a number of times in the trade.
    No worries C12 is the easiest material to drill aside from your finger.

    regards
    ----------------
    Can't Fix Stupid

  5. #5
    Join Date
    Mar 2007
    Posts
    32
    Quote Originally Posted by cam1 View Post
    the split point is only an advantage if you choose to ignore center drilling.
    They take a lot less pressure to push through.

  6. #6
    Join Date
    Dec 2007
    Posts
    617
    Good point, I stand corrected.

    regards
    ----------------
    Can't Fix Stupid

  7. #7
    Join Date
    Apr 2006
    Posts
    82
    Do you do center hole before drilling ?? If not, your drill MUST have a web thin if you don't want to have a hole diameter to large at the top.

  8. #8
    Join Date
    Apr 2008
    Posts
    3

    learning a lot guys thanks

    Hey I'm learning alot from you guys but I do have a few questions. What is frr and 3D mean. Please excuse my ignorance.

  9. #9
    Join Date
    Dec 2006
    Posts
    242
    No one asked a couple of really important questions. Are you using a screw machine length drill? This makes all the difference. It will still have plenty of flute depth for 1/2" material, but there would be no need for a center drill and the loss of time. A jobber length drill will wander around without a center, which explains the larger top side of the hole. Also, using a split point is important too for not having to center drill. I would raise the feed rate to atleast 9 inches per minute. That is only .005" fpt, which I use in 1018 CRS. Your material is nearly twice as easy to cut. Are you using flood coolant? I would probably drop the revs down to 1500 and not even peck drill. Also, make sure your runout is under .003" at the end of the drill if you can. McMaster.com has a split point cobalt #8 drill for $2.87 and you could do several thousand holes on one drill if you flood with soluble oil. The part number is 28765A58. Their UPS ground shipping is really reasonable, starting at $4.25 for Michigan. The guy who gets paid big bucks for making a couple holes perfectly thinks a lot differently than the guy who gets paid a little per hole for many holes. I happen to be both guys. LOL.

    Good luck,
    Dave

  10. #10
    holes that are larger at the top are due to one of a few factors , no spot , dull drill , drill has been ground improperly and is offset , crap built up on the drill due to poor chip extraction and rubbing the edges of the hole wearing the top of the hole open ,drill is too long as was pointed out already , pushing the drill too hard , cheapo drills made from inferior materials


    change the drill and try again
    A poet knows no boundary yet he is bound to the boundaries of ones own mind !! ........

  11. #11
    Join Date
    May 2007
    Posts
    1003
    Quote Originally Posted by egyptandjustice View Post
    Hey I'm learning alot from you guys but I do have a few questions. What is frr and 3D mean. Please excuse my ignorance.
    Based on the context, frr is misspell 'free'. As in no free lunch. 3D means 3 times the diameter. Thus a #8 drill's first peck would be .597 deep.

    Apparently I am doing something wrong, as I find this rule to be true only with smaller drills. Try going 1.5 inches deep in 316 SS with a 1/2 inch drill in one peck. Doesn't work for me! Nor will it work with 52100. If anyone knows how it is done, please enlighten me. I would love to know how.

  12. #12
    Join Date
    Dec 2007
    Posts
    617
    The rule of 3D basically states that any hole deeper than 3 X the diameter of the drill, should be treated as a deep hole. It does not imply the depth of the first peck.
    I usually go in at least 1.5D on the "first peck" to avoid chatter, as the drill generally pilots itself on it's diameter at 1.5D. After that, I usually reduce the peck depth. The depth of peck is a variable that's workpiece and tool geometry dependant ie don't peck into work hardening materilas, and softer materials like aluminium tend to get long stringy chips on too deep a peck....

    regards

    regards
    ----------------
    Can't Fix Stupid

  13. #13
    Join Date
    Apr 2006
    Posts
    82
    Quote Originally Posted by cam1 View Post
    The rule of 3D basically states that any hole deeper than 3 X the diameter of the drill, should be treated as a deep hole. It does not imply the depth of the first peck.
    I usually go in at least 1.5D on the "first peck" to avoid chatter, as the drill generally pilots itself on it's diameter at 1.5D. After that, I usually reduce the peck depth. The depth of peck is a variable that's workpiece and tool geometry dependant ie don't peck into work hardening materilas, and softer materials like aluminium tend to get long stringy chips on too deep a peck....

    regards

    regards
    UNfortunately, there is no rules for pecking cycle. It depends of diameter, kind of chip (short, long), lubricant, machinability of material

    If you have favourable conditions:

    - Material, which produce short chip (brass, carbon steel, grey cast iron)
    - Cutting oil
    The pecking cycle can be from 3-6xD.

    If you have undevaforable conditions
    - Stainless steel (304-316l), electrolytic copper
    - Emulsion oil

    The pecking cycle should be lower than 0.3xD

    1) Look at the chip form (short, long)
    2) Look if there is adhesion on your drill

    If yes, reduce the pecking cycle.

    Of course the best thing is to have internal coolant. You can drill without pecking cycle

  14. #14
    Join Date
    May 2008
    Posts
    14
    Quote Originally Posted by ErnieD View Post
    Hi,

    I am trying to drill many holes through .500 thick 12L14 with a #8 drill using a Tormach PCNC1100 milling machine. I am running the spindle 1800 RPM's amd feeding 4.5 IPM. The holes are larger at the top (drill entry side). What am I doing wrong?

    Thanks,

    ErnieD

    Ernie,

    I looked at the tormach and I think it is a bench type mill only. I think that your feedrate might need to be reduced since the machine can not handle the load and you are probably bending the drill a bit while drilling which cause the top part to be a little bigger on the top. The servo can drive it down but the hp is important too. 1.5hp I think. You can increase the rpm so that you get the same productivity.

    i don't know how many parts you are doing but if you will be doing a lot of drilling for production, you should get yourself a bigger machine to do the job in half the time. You can use flood coolant and remove the peck cycle since 12L14 chips are good. Make sure you have enough coolant though to drive the chips away. you can also use mist coolants so that you don't have oil dripping everywhere. Noga mist coolant are nice to use.

    If you are doing too many parts, consider a machine with enough torque to handle the job.

    If the feedrate reduction and the split point recommendation doesn't solve the problem, look into the machine structure. Do you have backlash? Old machines might need to be adjusted to keep the tolerances.

    Centerdrills are good for accurate positioning but it won't do anything to correct your large on top holes. Check your drill chuck also, your chuck might have a large run off.

    Good luck.

  15. #15
    Join Date
    Aug 2005
    Posts
    300

    Drilling #8 holes

    To all that have replied,

    I have solved the problem of holes larger at the top. I did away with the parabolic flute screw machine drills and went with a regular screw machine length drill with a 135 degree split point. I now get a nice straight hole. I made a fixture that holds ten parts. I load and unload parts during the cycle. The machine never stops and I am running about 170 pieces per hour. So far I am getting approximately 800 holes per drill. I have not reground any drills yet but I can see it coming. I have drilled, maybe 3-4 thousand parts so far. There are supposed to be ten thousand parts total and I am sharing them with the guy that I am getting the work from. Whew, 10000 parts, 20000 holes; that is a lot of holes.

    Thanks for all the replies and suggestions,

    ErnieD

  16. #16
    Join Date
    May 2008
    Posts
    14
    Quote Originally Posted by ErnieD View Post
    To all that have replied,

    I have solved the problem of holes larger at the top. I did away with the parabolic flute screw machine drills and went with a regular screw machine length drill with a 135 degree split point. I now get a nice straight hole. I made a fixture that holds ten parts. I load and unload parts during the cycle. The machine never stops and I am running about 170 pieces per hour. So far I am getting approximately 800 holes per drill. I have not reground any drills yet but I can see it coming. I have drilled, maybe 3-4 thousand parts so far. There are supposed to be ten thousand parts total and I am sharing them with the guy that I am getting the work from. Whew, 10000 parts, 20000 holes; that is a lot of holes.

    Thanks for all the replies and suggestions,

    ErnieD
    Ernie,

    You should consider Carbide drills. I think you will reduce your cycle time more since carbide can run at higher rpm's. you can double your production and thereby reducing your cost. I just don't know if your machine can take the load. If it can't, then try OSG gold drills. Go with the same lengths as you have now but you can increase feed and rpm with this. Follow the chart and it can reduce your cycle time considerably. If not, then the drill regrinding will be reduced.

    I'm have a S20C or AISI 1020 product with 5mm and 6.3mm holes. 40,000 pieces a month each size. We run OSG gold drills since we increased our feedrate and rpm by 20%. We do about 175 pieces per hour on our machine for both sizes already, our depth is 20mm or near 0.78 inch. We have used Sandvik Solid Carbide and reduced the time by 200%. We used 3R quick change dies. (about 6 seconds max change over) then run about 70 pieces per run. If we only have one size drill, we run 350 pieces per hour.

    Hope this helps.

    John
    www.nitoseiki.com

Similar Threads

  1. Q: Drill diameter for reamed holes.
    By Deviant in forum MetalWork Discussion
    Replies: 21
    Last Post: 01-11-2019, 10:30 PM
  2. Drill Multiple Holes - Newbie Question
    By NetStorm in forum BobCad-Cam
    Replies: 5
    Last Post: 06-20-2007, 01:59 PM
  3. Drill holes with end mill or twist drill ?
    By Argofanatic in forum MetalWork Discussion
    Replies: 15
    Last Post: 12-30-2006, 05:05 AM
  4. drill dwell between holes
    By EVERFABCHAD in forum Mazak, Mitsubishi, Mazatrol
    Replies: 0
    Last Post: 08-11-2006, 01:15 PM
  5. Drill holes for flat cap screw
    By starCNC in forum Uncategorised MetalWorking Machines
    Replies: 7
    Last Post: 09-09-2004, 03:47 PM

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •