PDA

View Full Version : Deep hole (for me)



Seastar
05-28-2013, 11:32 AM
I have a 10 inch long round bar of 2023 T3 AL that I need to drill or bore a ,250 hole al the way through.
What's the best way to keep the hole centered?
I need it within about .010 all the way through.
A hole that small and deep would require a long and flexable boring bar so I think that method is out?
I ordered a long enough drill but I am afraid the drill will wander or flex.
How would you do this?

What cutting lube is best for a hole like this?
Bill

Rich Carlstedt
05-28-2013, 11:59 AM
Read the sticky deep Hole drilling 101
http://bbs.homeshopmachinist.net/threads/43432-Deep-Hole-Drilling-101

Make sure your tailstock is on the same C/L as the spindle
Start with a new Ball End Mill, not a center-drill --very important and make sure the mill depth goes at least 51 % of the drill spiral flute pitch.
This will give your drill 100 % centering support on the flutes
Rich

Paul Alciatore
05-28-2013, 02:18 PM
Cutting Lube: I would think that any good cutting fluid would be OK. Just do use one.

Tooling and technique: A gun drill or D bit would probably be best. If you could stand a slight irregularity in the middle, I would start from both ends and meet in the middle.

In any case, I would withdraw the drill frequently to remove chips from the hole so they do not push the drill sideways or scratch the finish of the hole. And add more coolant/lubrication on each peck.

Do do this in the lathe with the stock rotating. Alignment will be a lot easier that way.

As for the topic that Rich refers to above, it appears to be a good, if somewhat confusing, discussion of deep hole drilling. I must say that I am on the side of that discussion that says that there is no difference in the SFM of the two flutes when a drill is deflected off center. I think the key factor in that discussion is that you must look at the off center drill point as actually rotating around it's own center in a local sense. This is the essence of beanbag's analysis and Barrington's animated sketch in that discussion. And this local analysis is key to seeing that the two flutes are cutting at the same SFM velocity.

But one thing not mentioned there, that I personally think is very important in preventing the drill from wandering, is the amount of "land area" on the outside diameter of the drill. Standard twist drills have relatively small lands on the OD. They are deliberately reduced from the full width of the area between the flutes to cut down on the friction when drilling a hole. For smaller holes this is a good thing and it allows the drills to be operated at faster speeds for shorter total times when drilling holes. However, this is not always the case. A hole saw has a small diameter drill that is used to produce a pilot hole and the OD of these small drills have full width lands to help increase the bearing area so the drill can serve as a pilot for cutting the full diameter with the circular saw element of the tool. A standard twist drill can be forced to "cut" sideways. I have often widened holes in soft material, like aluminum or wood, by tilting a twist drill in a hole. Not the best technique, but it does work. So these small lands are not the best for preventing sideways motion of the drill.

I think that the primary factor in drilling a straighter hole with a gun drill is the very large land on the OD. It is almost impossible for the drill to wander due to the opposing action of this large land on half to 3/4s of the circumference of the drill. It is like trying to cut with a lathe tool that has zero clearance. You may be able to force it, but it will fight you all the way. And there will be smoke.

I doubt that a gun drill used in a home shop or even in many small commercial shops will be run with high pressure coolant being fed down a central hole. Neither mills or lathes in these small shops have any provision for any such coolant feed, much less a very high pressure one. You are most likely going to use a solid drill that is either HSS or some other tool steel for most of it's length and possibly with a carbide tip.

So, when drilling a deep hole, in a small/home shop environment the best thing you can do is use a drill with a large land area on the OD. Hence, use a gun drill or a shop made D bit. Avoid the standard twist drill. And, since you will not be using a coolant/lubricant feed through the drill, withdraw the drill frequently to clear the chips out AND add more coolant/lubricant to the tip of the drill. I add the "lubricant" to coolant because in this case the lubricating qualities are more important than the cooling ones. You will be drilling at a slow speed and with pecking, there will be little tendency for heat to build up. But lubricating the land areas of the drill is perhaps more important than anything that is happening at the point where the cutting is actually taking place.

jimsehr
05-28-2013, 02:27 PM
It might be a good idea to start with oversize stock , then if you have to you can turn the od using the 1/4 inch hole to center stock to make od true to id.
jimsehr

Jaakko Fagerlund
05-28-2013, 03:49 PM
Gun drill and pressurised air or coolant through it at about 20-100 bar.

Evan
05-28-2013, 04:10 PM
It is essential that the cutting edges and the flutes be as close to identical as possible. If they are at all measurably different return the drill and try another. Cheap won't do in this case. You do have the benefit of working with good material. The 2000 series aluminum machines very nicely.

Rustybolt
05-28-2013, 09:16 PM
It's aluminum so you can run it pretty fast. First center drill. The drill will follow center if you do everything right. Next, like Evan said, select a properly ground drill. Good quality new drills are a good bet. DON"T CROWD THE DRILL. Let it cut. TAKE YOUR TIME.A good rule of thumb is 3 times the drill diameter for the first pass. 2 times for the second and one times for each pullout after that. If you have flood coolant use it. if not use a spray bottle and dose the bore frequently.

Rich Carlstedt
05-28-2013, 09:16 PM
......In any case, I would withdraw the drill frequently to remove chips from the hole..........
.
Excellent suggestion Paul !


............
As for the topic that Rich refers to above, it appears to be a good, if somewhat confusing, discussion of deep hole drilling. I must say that I am on the side of that discussion that says that there is no difference in the SFM of the two flutes when a drill is deflected off center. I think the key factor in that discussion is that you must look at the off center drill point as actually rotating around it's own center in a local sense. This is the essence of beanbag's analysis and Barrington's animated sketch in that discussion. And this local analysis is key to seeing that the two flutes are cutting at the same SFM velocity..

The confusion was created by Beanbag. If you believe the image he projected, so be it.
Let me say that his argument flies in the face of real world facts and over 20 years of real life experiences.
I emphasize the importance of a good starting hole, with every message posted ( including this thread) . If someone wants to create another perspective based on imaginary conditions, and disregard the start of the hole (!), let them post it on another thread. It will mislead folks.
The intent I had was to help those who wish to drill deep and with some better than average success.
Your comment about flute support is important, as well as Evan's point on balanced flutes and good drills. Very important !
I have built deep hole drilling units and high pressure pumps ( 3,000 PSI @ 25 GPM ie), and was involved with many thousands of deep holes ( to 48") and hoped to share some of that experience




.......................But one thing not mentioned there, that I personally think is very important in preventing the drill from wandering, is the amount of "land area" on the outside diameter of the drill. Standard twist drills have relatively small lands on the OD. They are deliberately reduced from the full width of the area between the flutes to cut down on the friction when drilling a hole. .

Absolutely right, so when you use such a drill, the pilot hole must not only be to the same size as the drill, but the starting depth should allow the hole to guide the flutes with 360 degree restraint. Thus my comment, as every drill has a different flute angle.
Another help is to use Aircraft drills as you get shorter flutes and more rigidity

One final word, a good gun-driller can hold .0001 " run-out per inch of travel
If the same drill is revolved and the work held stationary, that becomes .0015" per inch

Rich

Black_Moons
05-28-2013, 09:52 PM
It might be a good idea to start with oversize stock , then if you have to you can turn the od using the 1/4 inch hole to center stock to make od true to id.
jimsehr

++ On this idea. Although the hole might still not be 'straight' but could be curved. But then, that may not matter, it may just need to be accurately located on each end.

Of course, if thats true, drilling from both ends works great too.

Paul Alciatore
05-29-2013, 12:29 AM
Rich,

I would be the last one to argue with 20 years of experience, which I do readily admit that I do not have on this subject and, if you read my comment carefully, I did not so argue. I only disagree with your explanation of WHY it works. If it works, then IT WORKS and it should be done that way. I just do not buy the idea that one of the flutes is going faster relative to the material it is cutting just because it happens to be further from the center of the workpiece. In this situation, it is the center of the drill bit that counts for calculating the linear velocity of the edges of the flutes across the work and both flutes are at about the same distance from that center at all times. And this will be the case BOTH with the drill revolving and with the work revolving.

My conclusion is that there is, there must be, some other reason why rotating the work helps to keep the hole centered. Perhaps it is in some other detail of how the lathe functions as opposed to a vertical milling machine or drill press. I do not know what it may be, but if I were going to try to bore a deep hole I would try to set it up on the lathe with the work rotating and the drill fixed, either in the tailstock or in a tool holder on the carriage/compound. I would do it this way because it does work, for whatever reason. This is art and experience vs. science or theory. And I would pay a lot of attention to aligning the drill with the rotational axis of the work (of the lathe).

Perhaps you, I, or someone else will come up with a better reason why it works. I eagerly await that.



...<snip>...

The confusion was created by Beanbag. If you believe the image he projected, so be it.
Let me say that his argument flies in the face of real world facts and over 20 years of real life experiences.
I emphasize the importance of a good starting hole, with every message posted ( including this thread) . If someone wants to create another perspective based on imaginary conditions, and disregard the start of the hole (!), let them post it on another thread. It will mislead folks.
The intent I had was to help those who wish to drill deep and with some better than average success.
Your comment about flute support is important, as well as Evan's point on balanced flutes and good drills. Very important !
I have built deep hole drilling units and high pressure pumps ( 3,000 PSI @ 25 GPM ie), and was involved with many thousands of deep holes ( to 48") and hoped to share some of that experience

...<snip>...

Rich

PixMan
05-29-2013, 12:30 AM
I've done a similar job using a Titex A1622-1/4IN parabolic flute split point drill. It has 5.91" of flute length, and when I drilled a .25" diameter 6061 x 8.5" long hole (about halfway from each end) in the 1.25" diameter stock, the holes matched up near perfect. Lots of pecking once I got more than 2.5" deep though. I spotted with a 90 3/8" drill I have, NOT a center drill.

Those drills list for about $33.90 each, well worth the money.

Jaakko Fagerlund
05-29-2013, 04:00 AM
And please, use a spotting drill and not a center drill. Center drill is made for drilling center holes, not starting points. Center drills are most often 60 degree included angle, while drills usually are 118 degrees. This means that the drills cutting edges start from the edge of the workpiece, meaning from the largest diameter that the center drill produced. Do it often enough and your drills cutting flutes will get severe damage at that point. Also the dril has a tendency to grab.

Good 120 degree spotting drill makes such a hole that the drill contacts at the very center of it, thus providing that it will go exactly where the spotting is.

Sure center holes work as starting points, but they are not meant for it.

dian
05-29-2013, 04:17 AM
if you predrill with a center drill, you would not use the 60 angle, just the tip, that seems to be 118. i bought cnc spotting drills, but i never use them, as the chisel edge is huge and i dont believe they would center properly. the center drill is much shorter and much more rigid in proportion to the tiny chisel.

what i wonder about: if the "d-bit" drills are so good, why are they not widely used? i have never seen one.

beanbag
05-29-2013, 04:36 AM
If you step drill (e.g. drill a hole 1/3 the diameter first), will this make the final hole more or less straight? On one hand, the thinner drill is more likely to deflect. When the bigger drill goes thru, does it tend to follow the pilot hole and also deflect, or is it actually more likely to drill straight because you don't have to push so hard to make the web cut?

EVguru
05-29-2013, 04:54 AM
what i wonder about: if the "d-bit" drills are so good, why are they not widely used? i have never seen one.

Because they have no means whatsoever to clear swarf.

Before quality HSS twist drills became so easily available and affordable, a D-bit was an easily made and cheap solution. They still have their place as a useful tool in the workshop.

They can be thought of as a fixed size boring head that is guided by its own hole.

Rustybolt
05-29-2013, 07:30 AM
jaako
If he takes his time and proceeds slowly he'll do fine, even using a center drill.

vincemulhollon
05-29-2013, 08:27 AM
If you step drill... will this make the final hole more or less straight?

Less, but still probably straight enough. Step drilling is for hand drills where you don't have the HP to do it all in one cut. It works REALLY well for that. Its not for precision.

I've found that when I "must" step drill I get better results when the drills are razor sharp. That lowers the HP which was the whole point, but also means it prefers to cut rather than grab so it turns out straighter. Since you're doin' it wrong by step drilling, its important to at least try to do everything else about the task right, like a really good sharpening job. Its good practice since the step drilling will destroy the bigger drill at the contact point but not the center which does nothing, so you'll have to sharpen after the job anyway.

The worst clamping problems I've had have been step drilling when it inevitably grabs. I'd rather drill sheet metal than step drill, and sheet metal drilling sucks.

I've also managed to snap larger drills when step drilling. A little 1/8th in an small "80s" hand drill can happily chew a curvy path for a 1/2 that a 1/2 cannot survive. This is worst in wood when you hit/bounce off a knot or whatever rather than metal. Also aside from cutting curved holes you can simply drill a non-perpendicular hole that a 1/8th can handle the bend without snapping but a 1/2 will snap right off when it tries to follow the 80 degree entrance angle or whatever. Step drilling is kind of like tapping, you know you can easily drill a tap hole that the tap drill will be perfectly happy with, but the tap itself will snap in.

Evan
05-29-2013, 04:14 PM
Step drilling isn't going to help with a bit that diameter ratio to hole depth. It does work well when the ratio of the hole diameter is a larger fraction of the hole depth. I used step drilling in repeated sequence to drill this spindle hole in stainless steel for the lathe I built some time ago and it came out within a few thou of on centre. In this case the bits were large enough to be relatively rigid over the entire hole depth. Not the case with a .25" bit over ten inches.

http://ixian.ca/pics10/lathepart1c.jpg

http://ixian.ca/pics10/lathepart1d.jpg

andywander
06-03-2013, 09:34 PM
.... I just do not buy the idea that one of the flutes is going faster relative to the material it is cutting just because it happens to be further from the center of the workpiece. In this situation, it is the center of the drill bit that counts for calculating the linear velocity of the edges of the flutes across the work and both flutes are at about the same distance from that center at all times. And this will be the case BOTH with the drill revolving and with the work revolving. ....

Paul, look at it this way. If the work is revolving, and the drill is way off-center, by it's radius, for instance a 1" drill is off center by 1/2", then one flute would be at the center of the revolving work, and so there would be no relative motion of that flute to the work. While the opposite flute would experience twice the speed relative to the work.

Now obviously, the drill would probably snap off in that situation, but it does illustrate the difference in cutting speeds as the drill goes off center.

J Tiers
06-03-2013, 10:33 PM
I have drilled a number of deep holes..... 0.236 through the length of an 8" piece, etc.

I have some things that have worked for me...

1) YES YES start the drill on-center, dead-on center. If that is messed up, everything else is a waste of time, you start with an error.

2) DO NOT USE A REGULAR DRILL. use an "aircraft" bit, with a long straight cylindrical shank, and flutes on the end for maybe an inch or so for 1/4" drill. A regular drill is nearly hopeless on deep holes unless you are very good at it. be sure the shank is not larger than the flutes (can be, usually isn't)

3) pull out and clear chips about every 1/2 the drill diameter. yes, it's a pain, too bad. chips drive the drill off center.

4) use a cutting oil. sulfured ones are good, I use pipe threading oil, the dark amber Harvey's.

5) don't mess around, drill to final size. Why would you think a smaller drill that is more flexible will go straighter? Right... it usually won't.

6) use a SHARP drill