Drilling large holes

I need to make two Ø1/2" holes in an aluminum block (38" × 10" × 1"). My tool is a Ø1/2" × 18" drill bit so I have to drill the block from opposite faces. I have to be careful with the drill bit so it can not bend through the operation. The holes have to be straight.

Which type of point angle is best for this application? 118 or 135?

Thank you very much for your support.

???? Palafox - first, twice 18" is only 36", which would not be all the way through the 38" long dimension. But of course 18" is more than long enough to drill through the 10" or 1" dimensions. So that is a little confusing.

Second - this is a gun drill of some kind? A fancy OSG deep hole drill? 1/2" x 18 is 36 diamaters, and that will be more of an issue than the angle of the tip (or so I think.) Hopefully folks more expert than I will speak up.

Third - how straight? there is no such thing as perfectly straight. what is more, how much of a step is allowed where the two meet, assuming that's what is really going on.

Aside from the obvious problem mentioned above, it is extremely unlikely that you will be able to drill a straight hole with a drill that long. Especially if you plan on starting the hole with that drill and drilling the whole way with it. If you absolutely must do it this way, the hole should be started in a rigid machine with a short, stout drill, then changed out for a medium length drill, then the long drill. Your best option if you need the hole very straight is to get it gun drilled at a vendor who specializes in that type of work. Drilling from both ends as you plan to, the question becomes not "will the holes be straight," but "how crooked will they be?"

Yes, if possible, get it Gun drilled. If you try to drill 2 holes 18 inches deep using a twist drill, there is a good chance that they may not meet..

I think your best shot would be to start on one side like eKratz mentioned and then make an 3/8" or so extension on your drill Either by welding or threading I leave that up to you Perhaps even cut down the cilindrical part of your drill a bit so it has less friction in the hole Then do the rest of the hole with a handheld drilling machine And a lott of pecking The initial hole will guide your drill and with the handheld drilling machine pecking is much easier

Peter from holland

That hole is a prime candidate for a gun drill operation. Any shops near you with a machine that you could subcontract to? I see a lot of trouble with drill wander (never meeting up in the middle) and way too much time doing it with a twist drill.

Palafox said:

I need to make two Ø1/2" holes in an aluminum block (38" × 10" × 1"). My tool is a Ø1/2" × 18" drill bit so I have to drill the block from opposite faces. I have to be careful with the drill bit so it can not bend through the operation. The holes have to be straight.

Which type of point angle is best for this application? 118 or 135?

Thank you very much for your support.

Click to expand...

The obvious question is, why two 38" deep holes ? Can't imagine them being for bolts . What are they for?

Palafox said:

an aluminum block (38" × 10" × 1").

Click to expand...

Sorry. My mistake. It is a 30" × 10" × 1" aluminum block. Those holes are meant for lubrication purposes only so a perfectly aligned hole is not necessarily.

My first option was a gun drill but I have no one near with this tool. So, my plan was to make the operation with a smaller drill, then a medium drill (12" airplane drill) and finallly the larger drill bit.

I was also concerned about the point angle for this operation. Regularly we use a 118 degree split point angle and I was curious if a 135 degree split point would be the best option.

Thank you again for your help.

Some of the earlier replies have some good info. I would think that in general, the split point drill is a better choice, as it will require less pressure for the same amount of material removal, and may therefore help in a more accurate hole with less drillbit deflection.
You do not state what tool you will use to drive the drill bit. If I were doing this operation, the machine would be a critical choice, as well as the obvious issue of aligning the material to the spindle with some kind of fixturing. I would not dream of doing this with any sort of hand drill, but the length of the part presents some challenges as well for a choice of machine. Let us know how you plan to do it, or how it worked if it's already done.

I hope that you know better than to try to hand drill this item...from your postings so far it would seem that you do. Definitely use a split point drill, and in aluminum I think included angle will not make much of a difference. If I were to pick a machine I would prefer to drill this job on a horizontal boring mill with several staggered length drills since you have updated your original post "The holes have to be straight," to "A perfectly aligned hole isn't necessary."

Personaly i would stick the part in a lathe so it rotatets if at all possible. Drill wander will significantly decrease. Thats a long way to go. The depest i have done is something in the order of 14" on a 1/4" bit that was from one end though. Drilling from both ends if done in a lathe generaly comes out far better than most people think it would. Its slow going but i would have deffinatly said possible to do what you want. Just take it slow, peck befor the flutes get to full and keep it cool - lubricated.

30x10x1 in a lathe? Sounds like a little PITA. I'm with eKretz. The HBM would be ideal. It would be nice to have a coolant mister to help keep it from galling up.

I beg your pardon in advance but, I think the others have been too kind. Allow me, as a favor to you, to be a little blunt. 60:1? I think that you have no idea what you are getting into. So you drill from both sides, so what, that still only gets you to 30:1. Which is about where just plain SOB stops and Royal PITA begins. As others have said, you run a real good chance of the two holes not meeting in the center at all. You also have a real good chance of breaking an expensive drill and spoiling the work.

I would not use a undersize pilot hole. A smaller drill is just going to wander more. To clear chips and keep the friction down I would drill to 10" at the full diameter and then step down or use a reduced throat drill. Starting the hole with a stub drill as eKratz says. If you have a stiff machine and a carbide stub drill then your starter hole is going to be fairly straight. If not, then I would start a hole undersize and bore it straight.

And for the lathe-phobic among us, yes, you could line-bore this on a lathe.

sshhh,aint nothin!

A mold maker does this every day(almost).
first it aint a large hole,it is a deep hole.
,as hole gets deeper you can step dia. down a 1/64,for no side grap/ rub.
we usta use shop made drills,standard drill welded onto stick of crs,alittle wobble did not hurt a thing,cutting oil,clear chips as needed.
a spindle stroke of 20 inchs helps also,
Iffin you end up making drill,watch for it wippin into a 90 bend at drill chuck at high rpms,be very careful!!!!
CNC will make it a gravey job iffin u know watt your doin,yep.
as said above you need to start with a jobbers lenght or a stub lenght if your scared.
done it a thousand times,9/16 was the most common,3/8s npt size,eh?
Gw

for the record, I didn't say you couldn't do it in the lathe. I was merely stating the obvious common sense factor that given the shape and envelope of the work, a lathe would be more difficult than an HBM. I used to use the lathe all the time for extra deep grease holes for Link-Belt cranes and excavators, but all of the parts were round.

I don't think there should be any problem with the holes meeting in the middle with a 1/2" drill in aluminum as long as you start with spot drill, jobber drill, then work up in length. You've just got to take it easy with the long drill.

GW, I never started with the shorter drills out of fear, I always figured it was just plain faster since you can't push the long drill.

Palafox - OK, the real summary and some suggested reading:

A. It's a deep hole, quite a deep hole. (It implies a machine with quite a long stroke and/or set up space => HBM. Unless you happen to have a VMC with 48" of Z height at hand. And I'd really like to see a picture of it.)

B. The advice has been about how to drill a deep hole. I suggest a book by lindsay publications called "deep hole drilling" which is entirely devoted to this topic.
http://www.lindsaybks.com/bks5/deep/index.html

C. The gist of these techniques has been described below, but I'll try to summarize:
1. Make a correct starting hole, which the longer drill will use as a guide.
2. Construct the drill so that it has rests or the like that can bear on the guide (which is just the recently drilled part of the hole.)
3. Remove the chips - by long pecks, by pumping fluid down the drill, etc.

Both AMEC and OSG make drills that may make this task easier.
http://www.alliedmachine.com/default.aspx
(I've seen the AMEC product at a trade show but can't find the particular catalog page now. But they make what amounts to a carbide insert tipped gun drill.)

http://www.osgtool.com/news.asp?id=85 - which I've seen but not used.
I'm sure there are others.

(I've never bought anything from AMEC, though I have a number of OSG products - but I neither endorse nor disparage either for this task, I just happen to remember these products.)

If you know how to make a "D" bit,they drill with great accuracy. I made a 9/16" D bit out of drill rod,and drilled a 16" deep flintlock pistol barrel out of very tough propeller shaft bronze in the lathe. It was only .002" off center where it emerged.

A D bit is a very old design,but it is still a good one. They bored cannon with them hundreds of years ago.

You need to start a carefully drilled,then single point bored hole that is 3 or 4 times the diameter of the D bit deep. The D bit should JUST be able to enter the hole. It must be frequently withdrawn to clear chips,as it hasn't much capacity to hold chips. If you start the bit carefully,and don't drill too aggressively,it will do the job.

Twist drills are often not real straight to begin with. Since they are made in the shape of a spiral,they are also not very rigid,like a coil spring. The D bit is made by taking a piece of drill rod the correct diameter,and milling it down to a few thousanths above half diameter for,say,1 1/2" for the size you want. Leave the uncut half of the D bit .252" thick. Harden just the last 1/2 inch of the bit,so as to not warp the drill. 01 would be safer than W1. Grind the end of the bit at a slight angle,so that the CUTTING SIDE is a little ahead of the trailing edge. Also,grind maybe 10 degrees of clearance angle below the cutting edge,or the drill will not cut. You may have to touch up the edge a few times for each hole,and keep the false edge from building up. The D bit can be left at full diameter for about 3",but you should reduce the diameter maybe 1/32" for the rest of the length of the drill rod. This reduced surface does not have to be precision. It just provides clearance for the body of the drill so it doesn't rub,overheat,and gall in the hole,becoming permanently stuck.

Others may ridicule this D bit,but I know from personal experience that it does work. The solid portion of the body,which bears against the hole, will not flex,or let the bit wander off course like a twist drill will.

A gun drill really operates on the same principle as a D bit,and with pressure fed coolant going through it,and a carbide tip,it is better as it flushes the chips away. If you don't have that option,a D bit would do the job. The bronze I drilled with mine was VERY tough. I also drilled a same length genuine wrought iron barrel with it. It still came out very accurately,as it did in the bronze.

Be sure to use plenty of kerosene lubricant.

"Mold makers do it all the time." +1

Sub plates and stripper plates have never given me an issue on a radial drill. Start with a nice spot, preferably on a VMC, and then go at it with the drill. Move the table up when the quill travel becomes excessive and continue drilling with a spray bottle of coolant and a good air line to remove chips from the flutes.

1/2" x 18" doesn't seem like anything terrible; I've done half that diameter @ 20"/side and the coolant lines have always met.

I'm surprised nobody has mentioned parabolic flute twist drills yet. They are much better at clearing chips, allowing you to make bigger pecks. If you have to use a twist drill, that would be the type I would use.

i once built a fixture to use my lathe as a horizontal boring mill. i was drilling 1/2 inch holes 18 inches deep from both sides in 4140. we put the drill in the lathe chuck and used the saddle to feed. lots of pecking and a very tired arm at teh end. we went with center drill, half inch end mill (to get the hole started straight), short drill, longer drill, longer drill, long drill. something like that, its been a while. ended up less than a 1/16 misaligned which was more than good enough.