No announcement yet.

Drilling the correct hole, the first time

  • Filter
  • Time
  • Show
Clear All
new posts

  • Drilling the correct hole, the first time

    I recently had the "pleasure" of making several blind tapped holes M3-0.5, and took it as the opportunity to try out a roll (form) tap. The thing with this kind of tapping is that it is very sensitive to the hole size, especially for fine threads. Thus my question is on how to consistently drill on-size holes.

    The first time I did it, I just peck drilled with the final size that I wanted. This turned out to be a big mistake. I ran the drill at 5k rpm on the CNC (which is still below the recommended SFM for aluminum) and it made a bunch of little chips. I think the chips would occasionally get caught, because the holes were inconsistently oversize and often bell-mouthed.

    As an aside, what I think is happening is that even if you have the same feed per rotation, at high SFM, the chip curls more and thus breaks inside the flutes of the drill. When I drill waaaaay below the recommended SFM, like on a lathe below 1000 rpm, I can get the chips to flow out as two continuous strings.

    When I drill on the manual mill at a lower rpm, like 1-2k, I can get continuous chips (or short but at least curly chips). Doing it this way, I can get a somewhat consistent hole, where I can stick the shank of the drill back in the hole and it is a snug fit.

    More recently, I used the technique where you pre-drill a few sizes down, and then drill with the final drill. In this case, I purposely ran the final drilling step with a slower speed and higher feed, much as you would do with a reamer. This allows the final drilling step to trim away only a small sliver of a chip. I would say this worked well, because I could not even fit the shank of the drill back into the hole. I guess the hole is either undersize or on size?

    OK, after all this blah blah, I am interested in knowing if there is a way to drill the correct hole in one pass only.

  • #2
    Hole size

    No. Not that I've found. If the hole really has to be good you will have to do a rough and finish just like on most other things. Normally if you just drill a hole it will be tornado shaped - kind of big right at the top, then slightly funnel shaped getting smaller as it goes down, as the drill gets more stabilized by the surrounding material. Drilling a small hole then an on size hole is essentially the same as drilling and reaming, though a reamer will generally give a better quality of finished hole.
    Kansas City area


    • #3

      Ain't no absolutes in this world. But this is what often works for me.

      First properly sharpened drills with best angles for cutting and clearance. 115 and 135 degrees are fine starting points, but aren't always the best choice when you need to be fussy. So modifying the point angles can help depending on the material and conditions. Don't be afraid to experiment.

      Tool holding. Toss that drill chuck away. I don't who made your drill chuck, even a cheap China made ER collet will do better day in day out. Or at least a Morse taper if the drills are large enough.

      If HSS drills are giving you fits, consider switching to solid carbide drills. They are stiffer and less likely to flex under load.

      When I see bell-mouthing of CNC drilled holes, I first think the drill is flexing under load. So my first reaction is to lighten the feed rate and use a shorter peck depth, but keep the rpms up. I don't ever do full retraction on drill cycles and I would consider using just a straight dwell to break chips rather than any retraction. And make sure coolant is getting into the bottom of the hole as you drill. I don't know the size or depth of holes you are drilling, but just because you are flooding the hole at the top, doesn't mean it's getting to the business end. Sometimes it's a real bugger to get coolant to where you want it short of thru-the-tool methods.

      Also think about your fixturing method. I've had what I though was good fixturing cause me grief. Vises aren't always all that and other methods work better.

      Finally, sometimes there ain't no way around it, multiple tools to make one stinking hole are the only way you can get the results you need.

      If you think you understand what is going on, you haven't been paying attention.


      • #4
        In aluminum I get the most consistent and "on size" holes by spot drilling for a short depth just to locate the hole, only deep enough to start a straight wall, then driving the final drill down fast and hard to final depth in one go. I also use WD40 to lube everything first. I find if you dwell too long it opens up the hole.


        • #5
          Moltrecht has a sensible discussion of hole drilling.


          • #6
            Just a follow up question to this thread:

            If you use the technique of first drilling undersize and then drilling on size, how much undersize should you initially drill? I'm thinking that the second drill probably needs at least some kind of chip load to cut well - sort of how even reamers kind of have a minimum chip load, i.e. don't drill the initial hole too close to the reamer size.


            • #7
              I like to use 2 or 3 sizes under depending on the diameter of the finish size. Bigger that 1/2" gets 3 sizes under.
              It's only ink and paper


              • #8
                ok, thanks. Do you also treat the second drill like a reamer, i.e. half the speed, twice the feed?


                • #9
                  Originally posted by Carld
                  I like to use 2 or 3 sizes under depending on the diameter of the finish size. Bigger that 1/2" gets 3 sizes under.
                  Or more...... if the hole is too close in size, the drill wants to catch and "screw into" the hole instead of drilling cleanly.

                  of course you COULD just bite the bullet and drill plus ream.... a reamer is a lot better than a drill at reaming...... And you won't need very many reamers, just ones to go with your taps.

                  A properly sharpened drill is also better at drilling than a badly sharpened drill.... All drills drill oversize, but the more even the sharpening job, the closer to true size they drill.

                  Keep eye on ball.
                  Hashim Khan


                  • #10
                    For multi drills I first use a drill bit the size of the final drill bits center webbing.


                    • #11
                      Originally posted by Carld
                      I like to use 2 or 3 sizes under depending on the diameter of the finish size. Bigger that 1/2" gets 3 sizes under.
                      I've been using just enough to clear the big 'ol blunt nose on the final drill size, but that probably starts getting iffy once you get into smaller drills in the 1/4" range. I definately learned that I want a good bit of material for the drill to work with. Otherwise my results were worse than just doing it in one shot with no pilot.

                      For something that seems so straight-forward (put round hole here with rotating cutting tool) it sure can become a rabbit-hole as the requirements tighten down.

                      As for being on-position and on-size in one pass.... I never have come up with anything. Best I can guess is maybe a stub-length bit, ER collet, maybe lower speed heavier feed, and fresh edge so it's cutting and not skipping around and has less flex to wander around the axis?