Drill Drift

Awl --
How does a drill drift in x,y, with drill depth?
I would like to drill four 5/16 holes through a series of 1/4" alum plates
(actually wide 6061 or 6063 bar), where the holes must line up later (within .001-.005), and wonder how deep I can stack these plates and stay out of trouble. The hole is a clearance hole for 5/16 threads, but a semi-tight clearance hole.
I am hoping 8 plates would be OK, with a "regular" drill, either 118 or 135 deg. If not 8 plates, about how many?
How does drift vary with speed, feed, pecks, drill point geometry, etc? Best drill? I will of course spot the hole. On a fadal, altho I have considered a P-pushing fixture on a drill press or BP to do this, as well.
On the fadal, I suppose I could come back with a long 5/16 em, which would increase the clearance a bit, but would improve alignment. But I'm hoping to not have to do this.
--

Mr. PV'd

Mae West (yer fav CongressShill) to the Gangster (yer fav Lobbyist):
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Proctologically Violated wrote:

PV, I'd use a 5/16 parabolic flute, split point drill. I wouldn't think you would have problems. I drill a 5/32 hole in a 10.00" long alum piece 5.20" deep from both ends using a parabolic flute drill. The worst mismatch is around .010 I would guess.
I use a Titex drill for this, none of those Costco Worksmith drills!
Best, Steve
--


Regards,
Steve Saling
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Don't worry -- the only thing parabolic on those Costco drills is their wobble.
--

Mr. PV'd

Mae West (yer fav CongressShill) to the Gangster (yer fav Lobbyist):
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Your drift is going to be mostly a factor of the quality of your drill bits and the tightness of your drill spindle. An import special drill bit in a $69 Harbor Freight 5 speed drill press is going to be all over the map. Same operation in a high speed CNC spindle with stub length drill might be 10x tighter tolerance.
Proctologically Violated wrote:

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Proctologically Violated wrote:

<putting on my teacher's hat and firing up the verbositizer...>
Drills drift with depth when the axial thrust is large enough to:
A. Cause the drill to flex B. Defy correction by the balance between the opposed radial forces from the cutting edges. C. Both of the above
Try this for a test. Put a small jobbers length drill (1/8 diameter or less) in a drill press. One of your Costco specials will work just fine. Start it cutting on something sorta tough, probably not aluminum. After it gets started, gradually feed it harder and harder, and watch it carefully. As the feed pressure increases, the drill will flex, taking on the shape of a vertical jump rope. If you could freeze it in that state and examine it carefully, you'd see that the jump rope curve extends all the way to the point of the drill. This means that the point is no longer pointing along the same centerline as your drill press spindle. It's now pointed into the work at an angle, which is determined by the severity of the jump rope effect.
For a while, a drill in this state will scrape and claw and drill an oversize, bell-mouthed hole. After a few revs, though, being that it's a drill, it'll figure out how to start drilling like it (sorta) should - exept that it's still pointed into the work at an angle. So, it'll drill at an angle. Often, it'll drill at an angle that continues to increase as it goes deeper into the work. That's because, once it finds a way to start drilling, the jump-rope effect gets compounded by the new angle of attack. Things just get worse and worse. I've seen small drills cut sideways by as much as a whole diameter, when drilling only a few diameters deep, even though they were held in decent spindles, and didn't have any serious runout problems till they were flexed by excessive infeed pressure.
Normally, a good grind on the drill will keep the radial forces balanced, and will try to correct for most of the above. But the possible correction is limited, and is easily overwhelmed by infeed pressure and drill flexibility.
There are two possible solutions. One, use a drill with a properly split point. This will have cutting edges that go almost all the way to center, and will have very little chissel point. It's the chisel that requires a lot of axial thrust, since it's just squishing and squeezing metal out of its way, and can't really cut like a real cutting edge. Cutting edges themselves need torque; but very little infeed force, unless they're really dull. Get rid of the chisel, and you get rid of the thrust problem. You can feed faster with a split point, and still not flex the drill. Which means you'll have an easier time drilling straight holes instead of crooked or curved ones.
Second solution should be obvious. Use carbide. It's much more rigid, and won't flex like HSS. Simple.
Apply both of the above solutions at once, and you should get straight holes easy.
With regard to stacking plates, there can be some problems. When you start drilling a hole, you've got the point of the drill, center only, pushing on the work. It's the center that does the most pushing, even on split point drills. As the drill goes deeper, you're using both the point and the cutting edges, creating maximum push. Whatever force it takes to drill well will try to deflect the workpiece, unless the work itself is very rigid or very well supported.
Suppose, just for the sake of argument, that the aluminum plates you're drilling are able to flex a little bit - maybe just .005" when the drill is pushing to the max. So you start drilling, with a nicely chosen feedrate of, say, .010 per rev. And the work deflects a bit, and then resists, and drill goes fine - right up until the point breaks through the other side of the plate. Then, all of a sudden, the biggest part of all the pushing force is gone, and all that's left in the plate are the drill's cutting edges, which don't push all that hard. In fact, they can actually pull at the work instead of pushing it, just because of the way they're shaped. So, at the instant the point breaks through, your plate goes instantly from being deflected .005 away from the drill to being back at flat and normal, or maybe even being pulled toward the drill a little bit. What started out as a nice neat .010 per rev feedrate suddenly becomes .015 per rev, or more. Bad news. The drill bites too hard, probably pulls the plate even farther toward the spindle, which increases the feedrate even more, and so on, until you either break the drill, or decide to turn down your feedrates so they're way less than optimal during most of the cut, just to be tolerable when the drill breaks through.
Now, take all of that and stack the plates 4 or 6 deep, so the total possible deflection is much bigger, and the drill has to do 4 or 6 breakthroughs during every cycle. It gets real messy in a big hurry.
If you want to test this, just go back to the drill press you used earlier, put a decent size drill in the chuck, and drill through a test plate. When you get to where the drill is just about to break through, you'll probably instinctively back off the feed pressure and grab tighter with the hand that's holding the work. That's because you know that the work is going to jump, and buck, and try to screw itself right up the drill bit, if you're not real careful. Same thing happens in a CNC machine, even if the clamping and smooth infeed help reduce it a bit.
So, you'll need to support your plates underneath. Don't bridge them across blocks or parallels, but support them everywhere with a sacrificial plate underneath. That prevents downward deflection. Then, find a good way to clamp everywhere over the tops of the plates, so they can't bow upward when the drill's edges tug at them. A sacrificial plate on top, with pre-drilled holes, works best, as long as it's substantial and rigid enough to truly hold the plates down and keep them flat.
If you support the plates properly, and pin them down adequately, then drilling a stack of plates shouldn't be any different than drilling through a thick piece of solid. If you don't contain them well, and use the right kind of drill, you're gonna need a lot of drills, and probably some good drugs or alchohol to get you through the day.
<verbositizer to idle, teacher's hat back on the hatrack...>
KG
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Holy Shit, I'll be expecting a Tuition Bill in the mail! :)
Good show, tho.
Seems like as long as chips are being cleared (ribbons spiraling out, etc), pecking doesn't seem to be a big issue -- unless part of the purpose to pecking is to let more coolant into the hole??
Is pecking one of those things that absolutely should not be scrimped on, or just let the chips be the guide?
--

Mr. PV'd

Mae West (yer fav CongressShill) to the Gangster (yer fav Lobbyist):
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

That was a very interesting read. Since I just fix the machines and you program and run them, you send in the tuition check. I'll just thank Kirk for the lesson ;)
Wes
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
On Jul 5, 10:24am, "Proctologically Violated"

have you considered one of those insert type drills ? they had them at my last place and they went nice and fast into tool steel, and dead accurate too. when the insert wore, replace and keep on going. highly recommeneded.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

You need to be using a quality drill with a good point and relief, but I have found the most important point is starting each hole with a center drill. If a jobber length drill drifts off even a couple of thousandths, you are no longer in line with the spindle and will be forcing the error to multiply as you drill.
I have drilled 5/16" holes through aluminum castings as much as three inches with no more than .002 drift.
Of course, having your spindle perfectly square with the work piece is usually very important as well, depending on the required accuracy with the outside edges of the work piece.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here. All logos and trade names are the property of their respective owners.