Drilling holes (was Re: Dumb question on the drilling of holes

Hi all,

Thought I'd add my 2 cents here.

Drilling holes is probably more than 60-70% of machining, and we all do
it all the time. Trouble it that it is so easy we may have started on
drilling without getting the basics.

As you know, there are 4 common drill lengths, jobbers, taping, screw
machine and long drills. In addition, there are specialty drills,
center drills and spotting drill fit into that category. Long drill
are aircraft or long flute. Aircraft have a long un-ground shank and
standard jobbers length flute. Long flute have a flute that is more
than half the overall length, often 3/4 or more. Soa 1/8 drill in
aircraft might be 12 inches long with a 1 1/8 flute length or in a long
flute, it might be 9 inces of flute. The latter is better for chip
removal in deep holes or when in use with drill busihings of long
length.

As was mentioned, common jobbers drills tend to wander as they start a
hole. A center punch allows one to locate a hole more precisely. Even
a drill press will allow a drill to wander from center as the
rotational forces and axial forces interplay. A tight spindle and
short drill will greatly reduce this movement. Once a hole is off, it
is hard to get back to center without some real work.

Drills have two flutes connected by a web in the center. The center
web cannot cut, so it just pushes the metal until it can be removed by
a flute. When drilling by hand, a center punch allows a small hole to
be drilled, removing the center material from the hole. Then the next
size drill can do it's work much easier as the material under the web
is not there and the energy is in cutting not pushing metal.

Here is where a person can make some mistakes. A large drill used to
'clean up' a hole is cutting with very small sections of the bit and
can dig into the work easily. We all have experienced the drill
getting sucked into the part and the part spinning or the spindle
stalling at one time or another. Drilling a 3/4 hole with a 1/4 pilot
hole is actually easier than drilling a 3/4 hole in a 11/16 hole.

This is easily found when the drill punches thru the metal. The hole
naturally opens and the drill may pull in and leave little bits of
metal. The drill would actually screw itself in at that point. If
using a hand drill the whole thing screws into the part rapidly.

When starting a hole by hand, a center punch works well, when starting
on flat metal, a center drill offers a small web and a large starter
hole. Split point drills offer the best of both. They start cutting
in the relief under the web. Spotting drills are split points for that
reason.

When on a very rough surface or on an angle, it is really hard to get
not only a start, but also the get the hole to drill dead center. The
reason is that the drill can bend and will follow the path of least
resistance. On an angle, the up side of the part will allow the drill
to contact and push the drill off axis and the hole will be off center.
This can happen on very rough castings or if there are soft and hard
spots on the part.

How a drill actually cuts is another problem. If the two flutes were
perfectly ground, the drill would start, drill, then as the depth of
the hole allows the sides of the drill to engage, the drill would seize
in the hole ruining the drill. Drill bits must be ground off axis or
they will burn themselves up quickly. Most grinders do not have the
capability for perfect symmetry, and most people don't have the
patience to make that happen anyway.

IF you want to try this, grind your drill bit in your drill grinder
until it is close, then with little hand pressure just touch up the
flutes until there are little or no sparkes. If you put much hand
pressure, it will be uneven from flute to flute, so a very delecate
touch is needed. A 1/2 drill in a 1" steel plate will work, and
remember, no coolant for the test. After the sies of the drill get
ruined, try it again with coolant. It will last a little longer, but
not much.

None of the drill manufacturers list this factet of drill making, or
how they incorporate the different angles or different grinds.

A drill cuts with the flutes, and the center web holds the flutes in
position. If one flute is at a slightly different angle, or if one is
ground a little deeper than the other, the angles will evenly contact
the bottom of the hole and the drill will bend to allow this. Since
one flute is slightly different, one flute will cut the hole a little
wider, and the other will cut a little deeper, but not cut the full
radius. You can see this on larger holes and of drills sharpened by
hand.

This allows the inner flute to not rub the wall of the hole, and the
outer flute to deflect from the wall and not be forced to rub it.

Not knowing this, most of us have experienced drilling a hole with a
drill and finding that the hole is oversized. So we use a small drill
to get the hole on center and the final hole is closer to the drill
size. Then we drill just under and use the final drill to clean up the
hole and get closer to size.

Also, knowing this, you can grind one flute a little, use a tiny thru
hole and get an oversized hole, say for bolt clearance or something.

The triangle holes mentioned are from one flute digging in, the shaft
bending, then the next flute swinging out of axis and digging in. This
is caused by no center support of the drill web and too little material
on the flutes to let the drill get centered, and too shallow a hole.
You will find this in sheet metal or holes that are shallower than the
length of the distance between point and drill side. Using a 132
degree will reduce that distance. Putting a backing plate or
sacrificial plate under the part will also help. Also the relief angle
will have some part in the hole. Too much clearance and the drill digs
too easily. Grind the drill with almost no relief when drilling on
thin metals or plastics, or brass and copper. This allows the edge to
cut, but also limits the depth of cut.

Lastly, when a drill cuts, the drill flute digs into the part and wants
to twist. If you allowed the twist to occur the drill would open and
the drill might be twice the drill diameter. To counter this, the web
holds the flutes in position. As the flutes cut, they spread slightly.
The thicker the web, the less the spread, but also the less room for
chip removal and the more forces is needed to push the metal under the
non-cutting web. This movement is small, but it exists. The duller
the drill, the greater force to create this spread, and the more
machine force to move the drill thru the metal

If you need exact diameter holes, ream.
If you need exactly located holes, bore
If you need exactly located holes, and speed, spotting drill, then
drill as needed. The more rigid the machine the better the locations
will be.
Machine grind your drills or buy in lot quantities for low prices.

If you need located hole, on a budget, make an adapter on your drill
press to hold a drill bushing. Then use an XY table to move the part.
This is similar to a jig-bore machine and remove sloppy spindles and
poor bearings from the equasion. at least on a budgetary scale.


Dave

--- In CAD_CAM_EDM_DRO@y..., Marv Frankel <dcdziner@p...> wrote:
> Guys,
> I'm following this subject with great interest. One of the reasons I
> subscribe to this group, is to learn enough to convert my mill to CNC. I
> have been fabricating some parts on a mill, using the DRO, and have run into
> problems drilling holes. Using certain drill bits, many of the holes have
> come out oversize, and some completely out-of-round. Changing bits has
> helped, especially if I use a shorter length bit, but I'm going to
> investigate using the 135 degree, or other similar drills. I'm looking
> forward to a CNC conversion, when I intend to center drill the holes before
> using the correct drill bit.
>
> Marv Frankel
> Los Angeles
>
<snip> ( you're welcome)