to bore or to drill?
Close
Login to Your Account
Page 1 of 3 123 LastLast
Results 1 to 20 of 52
  1. #1
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    422
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    92

    Default to bore or to drill?

    I've had a few jobs at work where the part needed roughly a 5" diameter hole and 5" deep. The material started out as a solid round, one was 1045 (couldn't get the right size seamless fast enough). In both cases my boss told me to to drill up to 2-5/16" then bore. Went from 1/4" to 1" then 2-5/16 then bore.

    It seem like it would have been faster to drill to 1" then bore. Drilling a 2-5/16 takes for ever. Or, maybe drill in smaller increments. I was wondering what you guys think would be faster.

    Thanks,
    Andy

    Here's what the parts looked like finished. Thought it might help to see what I was doing.





  2. #2
    Join Date
    Jan 2013
    Location
    canada
    Posts
    861
    Post Thanks / Like
    Likes (Given)
    299
    Likes (Received)
    423

    Default

    Drill then bore is the way I would do it.

  3. #3
    Join Date
    Feb 2012
    Location
    Iowa, USA
    Posts
    673
    Post Thanks / Like
    Likes (Given)
    2137
    Likes (Received)
    458

    Default

    I'm guessing you were using the engine lathe in the photos, probably no turret.

    I would have skipped over the 1/4" and went with a 1/2" or whatever smallest dia. would allow clearance for the web. Blow through with that, then straight to the 2-5/16". I don't think your arm would be any more tired in the end doing it that way vs. running an extra drill through.

    Either way, cranking on a tailstock is going to be slow.

    If you have the h.p., the holding ability, and a decent sized carbide bar and can roll .5"+ off in a pass then go ahead and bore from a drill size just big enough to get a start for the bar. 350-400 sfm, .012"-.018" feed would make pretty quick work roughing that out.

    Again, ya need the horsepower to do it fast.

  4. Likes Mike C., Atomkinder liked this post
  5. #4
    Join Date
    Jul 2010
    Location
    Eastern Washington, USA
    Posts
    678
    Post Thanks / Like
    Likes (Given)
    580
    Likes (Received)
    526

    Default

    Mount an indexable drill in your QC toolpost, go from Zero to 1.500"+ in one pass half the depth, flip the part, core out the opp. side to meet in the middle, then bore the rest of the way. BTW, make sure the face each side before coring out with the indexable drill. If your lathe has a threading stop on the carriage, use it to set the C/L position for the indexable drill. Oh, & make sure to plumb the drill with coolant.

    Standard Helical Flute Drilling Holders | Travers.com

  6. Likes Philabuster liked this post
  7. #5
    Join Date
    Nov 2009
    Country
    UNITED STATES
    State/Province
    California
    Posts
    70
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    11

    Default

    Quote Originally Posted by stonehaven View Post
    Drill then bore is the way I would do it.
    Water jet or oxyfuel cutting for stock removal?
    ---Joe

  8. #6
    Join Date
    Jul 2013
    Location
    Victoria, Australia
    Posts
    33
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    6

    Default

    We make replacement wheels for William crushers at work, 500 OD 200 ID, 250 bearing seats, they're laid out to centre, spotted then, 12mm pilot, then drilled 80 straight through in a radial drill, then bored.

  9. Likes TedinNorfolk, Matt_Maguire, adama liked this post
  10. #7
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,309
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2670

    Default drill or bore

    Quote Originally Posted by Andy221 View Post
    I've had a few jobs at work where the part needed roughly a 5" diameter hole and 5" deep. The material started out as a solid round, one was 1045 (couldn't get the right size seamless fast enough). In both cases my boss told me to to drill up to 2-5/16" then bore. Went from 1/4" to 1" then 2-5/16 then bore.

    It seem like it would have been faster to drill to 1" then bore. Drilling a 2-5/16 takes for ever. Or, maybe drill in smaller increments. I was wondering what you guys think would be faster.

    Thanks,
    Andy

    Here's what the parts looked like finished. Thought it might help to see what I was doing.




    .
    1) i would do as the boss says to do
    .
    2) you have to hold the part and if it slips in the chuck you might scrap the part
    .
    3) hp needed might be more than your machine has and as hp used increases cutting force goes higher.
    .
    4) chips coming off. a drill you can peck drill to break chips, you can vary feed when boring but if feed is maintained and you get long chips forming a mess you have to stop to clear the mess of stringy chips
    .
    5) tooling cost, depending on drill type it might be cheaper to use a drill than expensive carbide inserts.

  11. #8
    Join Date
    Dec 2000
    Location
    Bremerton WA USA
    Posts
    10,710
    Post Thanks / Like
    Likes (Given)
    41
    Likes (Received)
    4371

    Default

    Drilling is generally more efficient for stock removal than boring with an HSS tool but if you're willing to max cuts using carbide insert bars you can generally beat converntional twist drilling drilling especially for loger bores. Feeding a 2 5/16 drill is no easy matter even if you have a 2 speed tailstock. Your wrists swell up like grabpefruit. after a day of hand feeding honking big drills in an engin lathe.

    I've found drilling in as few steps possible saved far more time than a series of interrmediate steps. 2/3 of the drilling thrust comes from forcing the chisel edge into the work. I usually eyeballed the web and picked a pre-drill about 10% larger then the web size. Drill through with the pre-drill followed by the hogging drill. If you're seeking better concentricity, drill a half diameter deep with a drill 1/16 smaller than the hogging drill then bore to the drill size.

    This "pre-bore" guides the hogging drill resulting in a straighter drilled hole and, if the hole is deep, a LOT of PITA boring the hole straighter. I've drilled 3/8" holes 20" deep to meet a cross drill back in the day. The material was cast copper nickel and the hole was to pass filtered water to a water lubed outboard bearing of a main injection by-pass pump. Giving the drilled hole a good start in the right direction pays big dividends in straight holes.

  12. #9
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    422
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    92

    Default

    Thanks for the reply's. The lathe has pretty good power, its a 10hp I believe. I was using a 1-1/4 boring bar carbide if i remember correctly .250 was the max material I could take off at .020 and about 350 sfm. Once boring, it went pretty quick. Maybe if I slow the feed down I could have taken .500 off.

    Another thing I need to learn or get better at determining is, at what point does slowing the feed and/or sfm down to remove more material become quicker than higher speeds and feeds and less material?


    Here's another pic for your viewing pleasure


  13. #10
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,309
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2670

    Default feed

    Quote Originally Posted by Andy221 View Post
    Thanks for the reply's. The lathe has pretty good power, its a 10hp I believe. I was using a 1-1/4 boring bar carbide if i remember correctly .250 was the max material I could take off at .020 and about 350 sfm. Once boring, it went pretty quick. Maybe if I slow the feed down I could have taken .500 off.

    One thing I need to learn is, at what point does slowing the feed and/or sfm down to remove more material become quicker than higher speeds and feeds and less material.


    Here's another pic for your viewing pleasure

    .
    carbide inserts are made for certain feed ranges or inch per tooth. when they stop making short chips and you get long stringy chips it can be a problem. carbide inserts when you reach a certain feed rate the corners break down from too much cutting force. also too much cutting force the boring bar will vibrate which also damages insert
    .
    also 0.250 depth of cut at .020 feed at 350 sfpm at 2" diameter is about
    13.4 inch per min feed and removes 21 cubic inches per minute and with 1018 steel thats about 26 hp and 2475 lbs of cutting force
    ..... my guess is you were not at .020" feed

  14. #11
    Join Date
    Jun 2009
    Location
    Near:Louisville, KY
    Posts
    1,729
    Post Thanks / Like
    Likes (Given)
    193
    Likes (Received)
    386

    Default

    Coolant thru Spade drill as large as HP allows then Bore.

  15. Likes redlee, RC Mech liked this post
  16. #12
    Join Date
    Aug 2005
    Location
    Toronto
    Posts
    5,082
    Post Thanks / Like
    Likes (Given)
    3427
    Likes (Received)
    3958

    Default

    drilling will always be the fastest way to remove material, but gawd who wants to crank the tailstock quill for days.

    Build a carriage power drilling attachments like this smart folks and Dean Smith and Grace do. Bolts to the carriage dovetail with a stop for centre. It take straight shank MT adapters so you don't have machine the MT and could have it up to 5 or 6 MT if you like. I've big chunk of cast iron waiting to be made into one....#673 on the TDL


  17. Likes rustdreamer liked this post
  18. #13
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    422
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    92

    Default

    Quote Originally Posted by DMF_TomB View Post
    .
    carbide inserts are made for certain feed ranges or inch per tooth. when they stop making short chips and you get long stringy chips it can be a problem. carbide inserts when you reach a certain feed rate the corners break down from too much cutting force. also too much cutting force the boring bar will vibrate which also damages insert
    .
    also 0.250 depth of cut at .020 feed at 350 sfpm at 2" diameter is about
    13.4 inch per min feed and removes 21 cubic inches per minute and with 1018 steel thats about 26 hp and 2475 lbs of cutting force
    ..... my guess is you were not at .020" feed
    The material removed was .250 not depth of cut. Doc was .125. I should have said depth of cut instead of material removed originally.

  19. #14
    Join Date
    Nov 2004
    Location
    Birmingham, AL
    Posts
    13,230
    Post Thanks / Like
    Likes (Given)
    6617
    Likes (Received)
    2564

    Default

    If you had some threads in there, it looks like a gland nut for a hydraulic cyl. I make them all the time.

    From the chips in that pic, you aren't laying on that tailstock quill very hard. Unless the lathe stalls, you can't crank that tailstock too fast with that drill. You want those curls 1" wide and the spiral to be big around as your thumb. Upping the feed rate actually keeps the drill cooler and makes the edge last longer, since it is buried in cold metal instead of rubbing.

    As for the 1/4, 1/2 and then 2 5/16... forget that. If you sharpen the drill with a split point, you can eliminate the pilot drill altogether. A coolmist sprayer pointing down the hole will help, too. Get the hole drilled fast as you can.

    Now, on the speed vs depth of cut, I always go with depth of cut. Reason being, you can take a big cut at a lower speed and usually get the chip to break instead of having to fight long snarling curls. Not only are those aggravating, they are extremely dangerous. If you can double depth of cut and double feed rate, you can cut the spindle speed in half and still work twice as fast.

    Get the bar up close to the toolpost as possible, while still being able to reach all the way through (I mean leaving 1/4" or less to spare). Set spindle speed to get 200ft/min for mild steel. I'd try to take at least .200 per pass. If the bar squeals, drop the speed to the next available notch and try again. If you can get the squeal eliminated then deal with the chips using feed. Jack up the feed until the chips break short. If the chips just won't break, back the speed down another notch. Last resort, back the depth of cut down and work it out again. Once you get it working, make a mental or literal note of your depth of cut, speed and feed combo so you can go with it next time.

    You may have to back speed down as the bore progresses, due to the surface speed increasing as the diameter increases.

  20. #15
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    19,642
    Post Thanks / Like
    Likes (Given)
    15079
    Likes (Received)
    15248

    Default

    Quote Originally Posted by Mike C. View Post
    If you had some threads in there, it looks like a gland nut for a hydraulic cyl. I make them all the time.

    From the chips in that pic, you aren't laying on that tailstock quill very hard. Unless the lathe stalls, you can't crank that tailstock too fast with that drill. You want those curls 1" wide and the spiral to be big around as your thumb. Upping the feed rate actually keeps the drill cooler and makes the edge last longer, since it is buried in cold metal instead of rubbing.

    As for the 1/4, 1/2 and then 2 5/16... forget that. If you sharpen the drill with a split point, you can eliminate the pilot drill altogether. A coolmist sprayer pointing down the hole will help, too. Get the hole drilled fast as you can.

    Now, on the speed vs depth of cut, I always go with depth of cut. Reason being, you can take a big cut at a lower speed and usually get the chip to break instead of having to fight long snarling curls. Not only are those aggravating, they are extremely dangerous. If you can double depth of cut and double feed rate, you can cut the spindle speed in half and still work twice as fast.

    Get the bar up close to the toolpost as possible, while still being able to reach all the way through (I mean leaving 1/4" or less to spare). Set spindle speed to get 200ft/min for mild steel. I'd try to take at least .200 per pass. If the bar squeals, drop the speed to the next available notch and try again. If you can get the squeal eliminated then deal with the chips using feed. Jack up the feed until the chips break short. If the chips just won't break, back the speed down another notch. Last resort, back the depth of cut down and work it out again. Once you get it working, make a mental or literal note of your depth of cut, speed and feed combo so you can go with it next time.

    You may have to back speed down as the bore progresses, due to the surface speed increasing as the diameter increases.
    Listen to the man - Mike C knows what he's talking about, and has put it in to words much better than I could.

    Keep to the ''old school'' rules, they still apply today, minimum over hangs, sharp tools with correct angles and clearances, making tools work instead of rub - etc etc etc, will get the job done quickly and with minimal problems and messing about.

  21. #16
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    422
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    92

    Default

    Thanks Mike and sami,

    the biggest thing holding me back was the drill bit spinning, if I really cranked on it. I used a dog against a 1" piece of square stock in the tool holder to help hold it.

    I put a wrench on the nut that holds the tailstock handle on. I slowly put more pressure on the drill and the dog eventually twisted on the drill bit and slipped off the 1" stock. It was loud!


    DMF_TomB, are you using unit power or power constant values for your formula?

  22. #17
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,309
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2670

    Default machinability rating

    Quote Originally Posted by Andy221 View Post
    Thanks Mike and sami,

    the biggest thing holding me back was the drill bit spinning, if I really cranked on it. I used a dog against a 1" piece of square stock in the tool holder to help hold it.

    I put a wrench on the nut that holds the tailstock handle on. I slowly put more pressure on the drill and the dog eventually twisted on the drill bit and slipped off the 1" stock. It was loud!


    DMF_TomB, are you using unit power or power constant values for your formula?
    .
    if 21 cubic inches removed of 1018 steel per minute and using a machinability rating of 0.8 cubic inches per minute per hp thats 26hp. some inserts are more efficient and can remove up to 1.6 cubic inches per hp per minute at higher feed rates so thats 13 hp
    depth of cut perhaps not the best term
    .
    2" dia shaft 0.250 depth of cut is on lathe 0.125 all the way around so 0.25 x 0.020 x 4200 (surface inch per minute or 350 sfpm)= 21 cubic inches per minute
    ...... my guess is you were not at 13.4 ipm feed as you would have bored hole in about 30 seconds

  23. #18
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    422
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    92

    Default

    There is something else I wanted to say.

    Not knowing the proper forum etiquette I did not introduce myself when I first joined.

    I've been and electrician since 2002 with a little break in there when I joined the Air Force for 6 years. I got out in 2012 and went back to electrical work. In the mean time I bought a little south bend to do a little gunsmithing, chambering is all really. Through this and some other little projects I really started to enjoy machining.

    In January I was able to talk a local machine shop into letting me work part time. By the middle of march I decided machining is what I wanted to do. Electrical work wasn't to bad but, it was more of a means to an end then anything. And in march I decided to work full time at the machine shop.

    What I mainly wanted to say is that, I've been having a blast! Its been great learning and getting to do something I enjoy. I also have to add that I'm thankful my boss was willing to take me in and teach me and allow me to learn on his time.

    I've been told I'm crazy for giving up electrical work but, I'd rather be happy and enjoy what I'm doing.

    The shop I work in is old and little dirty but, I think it is awesome. It was built in the 60's which I think adds to it. We have older machinery and nothing fancy but, we it get done.

    On one side is the machine shop and on the other is where all the welders, press, and balancer is. We mainly do repair work or make a new part of something that was broken. I did have to make six bearing housings and a couple other small multi part orders though.

  24. Likes Mike C., TeachMePlease liked this post
  25. #19
    Join Date
    Nov 2004
    Location
    Birmingham, AL
    Posts
    13,230
    Post Thanks / Like
    Likes (Given)
    6617
    Likes (Received)
    2564

    Default

    "the biggest thing holding me back was the drill bit spinning, if I really cranked on it."

    Ah! Most good big lathes have MT sockets that also have tang sockets like a radial drill to keep the drill fro spinning. The dog was the proper approach. The last place I worked had a little Leblond that somebody had modified by putting a couple of setscrews in the tailstock quill to grab the MT tang on the drill. Worked extremely well and was one of those things I took note of.

    The pilot hole may actually be working against you in this department, as well. The pilot drill is to reduce thrust on the drill by letting the chisel point (web) pass. By not drilling the pilot hole, or at least using a smaller one, you will increase the thrust on the drill, which will push it harder into the tailstock socket, making the MT less likely to slip. I have to use this technique on the little Enco 12" machine at work when drilling over about 1/2". Drilling a pilot hole causes the drill to want to self feed and makes it nearly impossible to keep the drill chuck from spinning. Try it without the pilot and see if it isn't less likely to spin.

    You aren't really trying to get a precise hole in this part (another part of the reason for pilot drilling). You just want as large a start hole as possible to proceed with the boring bar. Use a center drill to get a start for the point and then just let her rip.

  26. Likes tdmidget liked this post
  27. #20
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    422
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    92

    Default

    DMF_TomB so, I'm not sure I understand you correctly. if I move my tool .125 into the material that is not depth of cut? Just looking for some clarification.

    Either way, maybe I have my info mixed up, this job was two months ago. If I was in front of my lathe looking at the dials I would be able to recall.


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
  •