The drill bit has two "points", the outer edge of the cutting flutes, that try to rattle around in the bore that it is starting. Very frequently, you will get 3-lobed or 5-lobed shapes in thin sheets. As the drill progresses into thicker material, the twisting of the flutes gives it more secure support around the circumference, and the chattering of the point is reduced. But, in a thin sheet, the drill has gone all the way through before this can happen. The point angle and rake to the cutting flutes have some bearing on this, and there are a bunch of drill point designs that reduce the problem (split-point, brad point and many others). These can all be optimized for specific workpiece materials.
A very stiff mounting of the workpiece and a short drill bit, such as a lathe center drill will greatly reduce this problem. The Jobber's length drill bits are quite flexible, as you can see when you start these bits, the point will start to bounce around.
The reamer follows the centroid of the hole, which has no guarantee of being anywhere near where you wanted the hole. So, better drilling techniques will also give you a better final hole size. For almost any job where I want a hole to line up with something, I use a milling machine, clamp the work in a vise or to the table, and start the hole with a center drill first. Once the center drill has made a pretty good starting hole, the twist drill will follow with a lot less of this shuddering, and the final hole will be both more round and closer to where I started it. I usually get hole locations within a few thousandth of an inch of intended position this way. Using a center punch and then drilling directly with a jobber's length drill, the hole position can drift 25 thousandths of an inch, or even more.
How much of a hole do you drill with the center? I've been following Harold's recommendation to touch the work to make a mark and check the location before doing further damage - two fewer pieces of scrap and counting. If where I intended, I enlarge the mark, but my gut sense reading the above is that I should be doing more??
Congratulations on practicing one of the best tricks in the trade. You have obviously already reaped your reward, which is the reason those of us that use the same trick, use it!
Yes, you should be doing more-----if the hole size is critical, or you just want to turn out better work.
As you experiment with hole drilling, you'll come to realize that the depth and size of the center drill (which I always use, I don't use spotting drills) has a profound affect on how the drill starts out. I've never really concluded anything concrete-----sometimes a quite large starter hole is needed, other times a small one seems to work well enough. I use center drills from an #00 size up through #5, depending on the work at hand. Only experience, which you'll get by trying various combinations, will teach you what works best for your circumstances.
One of the things you often encounter is if your center drill is too large, the drill chatters like hell getting started. Controlling drill speed and feed rate will generally overcome any problems inherent with that scenario. Again, the circumstances of the job at hand may dictate the necessity of the large starting hole, so you have to learn to deal with the problems.
Make sure your drills are properly sharpened----and don't use one that has a dull edge, especially if it's only on one flute. That's a sure recipe for an oversized hole.
When hole size is critical, or you just plain want things to work out as if you're a skilled craftsman, start your hole with a center drill, drill undersized, then open the hole to the desired size. When drilling with fractional drills, you usually use a drill that is 1/164" under the desired size to drill the hole, which should allow enough for the hole to clean up. If it doesn't, there's something wrong with your process, usually the drill. You don't want to leave too much in the hole, otherwise the cutting forces can overcome the margins of the drill (which are circular ground and have no relief angle) and still yield an oversized hole.
When drilling with number drills, pick a drill that is maybe .010"/.005" or so undersized for the starter hole, then open to size. The smaller the hole, the smaller should be the difference between the two drill sizes. Don't leave too much for the second drill, but make sure there's enough left for the drill to open the hole to size.
Drills rarely provide a straight, round hole, but by double drilling as suggested you can usually get a decent hole that will be within a couple thou of nominal size, and will be as round and straight enough to be acceptable for most applications.
Drills that are sharpened off center will generally wing, creating an oversized hole at the mouth, but slowly moving towards center as the margin of the drill is forced towards center. You get a bell-mouthed hole.
If you're not adept at hand sharpening drill bits, it's not a bad idea to have a drill pointer of sorts to help keep your drills in good working order. Sharpening by hand is very good, but generally requires considerable experience before your efforts are acceptable. A careful hand can even split points.
Keep your drill shanks free from burrs. Hit them with a file if you raise one, so the drill is held concentrically in the chuck. Remember, drill shanks are not hardened, so they burr easily.
Do you find you have issues with drills being pulled into the work when double drilling? Working in a tool shop, we have no need for holes within a thou or two (either rough drilled or reamed only) so I don't have to do it very often at all. When I do, I find the drill frequently pulls into the hole making for a broken drill bit, spun part, or both. We have gear feeds on our radials at work so it's not necessarily an issue for us, but HSM's rarely have that luxury.
On a project where I had approx 80 holes (laid out by hand), I found this to work reasonably well. Properly pointed and sharp punches should be used.
Lightly prick punch doing your best to hold punch square to the work, and doing your best to tap the punch dead on so as not to move the punch when struck. Check against layout lines. Slight corrections can be made by holding punch at an angle (pointing in direction you want to move) and hitting again.
When satisfied with location, use a center punch to deepen the indentation, again keeping everything square and striking the punch dead on.
Since my drill press is el cheapo and has quite a bit of wobble, I used a small drill (.030 inch or so) to drill to a depth of approx. 1/16 inch. A drill this small will 'bend' slightly and go into your center punched indent. If the center drill you're going to be using is relatively small, might want to follow with a second drill, slightly smaller than the center drill pilot. Center drills have a nasty habit of clogging with chips and breaking.
I followed this with a center drill, going deep enough so as the countersunk portion was slightly larger (+ .020 dia.) than my finished hole size. The countersink allows the final drill to have only a small amount of material to remove before reaching actual size and consequently helps hold location.
Then drill to final size if your machine, setup, etc. are up to the task. A twist drill, like any cutting tool, performs best when operating at proper sfm and feed. For example, in mild steel, a
1/8 dia. twist drill should run about 3200 rpm. My drill press doesn't go that fast, so 'lighter' feed is used in order not to force the drill. Note that even 'perfect' drilled holes will probably drill oversize to some extent.
Probably most critical to maintaining location and drilling a 'straight' hole is having a properly sharpened twist drill. A properly sharpened drill should produce chips the same thickness and width from both cutting edges. Most job shops try to ensure this by starting with NEW high quality cutting tools. Keep in mind that if the workpiece is clamped in such a way that your carefully located hole is not central to the spindle axis, your location may be lost and you may end up with the hole not being 'straight'.
Rigid machine spindles, sufficient horsepower, controlled feed rates, flood coolant, etc. allow one to skip the small pre-drilling, etc. and are an ideal situation for spotting drills as opposed to centerdrills.
A definite yes to your question. In fact, when doing such an operation, it is almost a 'given'. I personally prefer to round off the corners of the drill slightly which will help prevent the drill from drilling oversize and also improves finish.
Of course, it's good for only a few holes, and the drill requires resharpening afterwards. Also want to have a good hold on the work.
"Robin S." wrote in news:pOatf.2274$ firstname.lastname@example.org:
IMHO and experience, you only want the undersized hole to be about 1/2 or less of the dia of the finish drill. What is important for the hole size is that the pilot hole is just slightly larger than the web wedge on the following drill. The wedge is where you get in trouble with drilling. Since the wedge displaces metal instead of cutting it, any variations in the microstructure of the drilled material (clumps of alloys or other materials) will pull the drill off-center. Yes, I said pull, since physics plays a role here, the drill (or any cutting tool, for that matter) is going to 'walk' along the path of least resistance. When you center drill, you are not only centering the drill with the cone, you are relieving the area under the wedge, so the drill will not walk.
The only thing I would add to the existing posts is this: When you center punch, you make a little volcano, not just a hole. It is helpful to file off the "hump" so the drill bit doesn't catch on it and begin its wanderings before you even get to the bottom of the punch mark.
John Emm> Why do holes made by normal twist bits almost always end up being out of
Not in drilling most anything but brass. Keep in mind that I drill this way routinely, so I probably subconsciously approach if from the position of already knowing of the problems you speak of, which are very real. Fact is, I should have made mention of them, but it didn't come to mind.
I rarely, if ever, use a drill press. I drill with my Bridgeport, almost never without using the vise or clamping my parts to the table directly. The control of the quill is superior to that of a drill press (radial drill excepted), so I can feel what's happening far better. It's quite easy to avoid hogging.
You raised some good points that should be of concern for those that use the double drilling system, for which they should be grateful. It yields better results, but has its own problems, as you've pointed out.
When I was trained (missile facility), hole size was routinely inspected, and parts scrapped when oversized holes were created, so I was instructed to work such that size was more or less guaranteed. I can see that where one trains can be instrumental in what method is preferred.
That isn't very effective when you're trying to achieve proper hole size, but it's a good way to reduce drilling pressure.
The reason for leaving a minimum of material in the hole for the second drill is to avoid the possibility of the cutting edges winging. It's virtually impossible for that to happen when there's only a few thou in the hole, even if the drill is sharpened improperly.
A drill sharpened with one edge longer than the other will compromise between running on the cutting edge and pressing against the opposite margin, trying to center the drill. This happens because the drill is flexible enough for the pressure of the cut to force the drill off center, balancing the forces. The result is a hole that is bell mouthed. The hole gradually forces the drill to center, but the result can be a scrapped part, depending on the nature of the work at hand. Tapped holes, for instance, won't tolerate that condition.