Small holes - deep...

[skunkworks]

I am needing to drill some small holes (1/16) down the edge of thin material. approximately 4-5 inches. My question is - how thick does the material have to be (stainless or aluminum) on each side of the drilled hole? ie - how strait will the drill drill?

assuming i can spot / start / align the holes accurately (not a problem)

I am planning on doing it in at-least 2 steps. standard 1/16 drill - then switching to a longer drill to finish the job.

Thoughts? .01" each side? .02"? more?

sam

[John Stevenson]

1/16" drill 4 to 5" deep ???

Personally I'd run away as fast as I could from a job like this.
A drill bit is possibly the most inaccurate cutting tool available to man and if you got a couple of holes to work out OK chances are you only want one to break thru and wreck the job.

Can you not re-design the part so you are only putting token 1/16" holes into something that opens out ?

Failing that how about milling grooves in two sides of thinner plate and sandwiching them together ?

[Toolguy]

Read "Deep hole drilling 101" in the Favorite thread sticky at the top of the Forums. Lots of good information. You are looking at a tough challenge. Your best chance of success on that one is a spot drill, then a single flute gun drill with high pressure coolant coming out the tip. Next best would be spot drill, parabolic flute drill with lots of pecks and cutting oil. If you can do 1/2 the depth from each end of the hole, it will have a better chance of success. Best of luck.

[loose nut]

Can't say how much material thickness you would want but trying to drill 1/16" 4"+, with a twist drill, is bound to have considerable wander unless you are very skilled at drilling or just plain lucky. How straight do the holes have to be. I don't know if a D-bit that small would work very well, normally a gun drill is used for deep holes but lots of luck getting one that small that wouldn't cost..........................

[BCRider]

Even with a guide I would not be confident on doing such a thing. At the very least you will need to start with premium quality aircraft extension drill bits. No cutting corners here on this. The cutting lips need to match to a very close degree for angle and width to limit any wandering. And you'll want high speed and room to clear the chips frequently. You will only be able to drill about 1/16 at a time before you pull it out to clear the chips. Clearing this frequently or even more so will be a key element in reducing any wandering. The guide bushing will be essential to this for both alignment and drill bit operation because at the speeds you will need to be spinning the longer extension drill bit would lose it and bend out to the side in a blink if the end was not running through at least a short guide bushing.

You'll also want a collet or some super accurately centered method to hold the drill bit. A common chuck is almost never good enough for something critical. And then the setup will all need to be centered up really accurately.

Even with all these precautions and setting up I'm still not that confident that you'll stay within the thickness at that depth. I have no idea what you're making but clearly the engineer that came up with such an idea should be tarred and feathered. Or if this is your idea you need to go lay down until the feeling goes away and you come up with another plan that does not involve drilling such long and narrow holes.

The only other option to all this is gun drill bits. They make such things down to .177 so I would not be surprised if they make 1/16 versions. But here again this is highly specialized, expensive and would require a really accurate jig with integral guide bushing for the drill. Again I'd either tar and feather the designer or if it's you go have a wobbly pop and come up with a new method which won't be so demanding on tools and cost.

[fixerdave]

Never tried it... don't even think I'd want to (that's a whole lot of pecking going on there) but what about the previously mentioned concept of spinning the work instead of the drill to get straighter holes?

If you could get the block hole centered in a 4-jaw then you could drill with the tailstock.

Can't say as I fully understand the logic of spinning the work instead of the drill. But then I can't say I understand the logic of drilling a tiny hole that deep. Can't you mill away at least the underside of the middle and then just drill 2 shorter holes? Better yet, drill short holes and press-fit some pins in, or thread some short holes and use screws, or ...

I dunno... Personally I call the the 8" woodscrews I've got "bad design screws." I use them AFTER I've 'screwed' up the design. If you're still planning... maybe do some more.

David...

[skunkworks]

Wow - thanks for all the pointers... I would be the engineer and it is an experiment - one off.. (well 2..)

I have a access to some really nice equipment. Alignment and accuracy is not a problem.

drilling from each direction might be the best solution...

sam

[becksmachine]

My first suggestion is to shoot the engineer, and then have a beer and celebrate the end of the job.

Oh, he is you so if you do shoot the engineer then there would be nobody to drink the beer. Can't have beer going to waste.

Yes, it would be a challenge to your patience, but I did drill some long small holes just yesterday. These were in bronze, and a little bigger, 6/32 tap drill, but they were 4-5 inches long and probably 50-60 pecks per hole.

These holes were lubrication galleries in a long bronze nut on my horizontal boring mill. Wall thickness was also greater than you are talking about. .020" would be the minimum that I would contemplate. Would it be possible to drill the holes before subsequent machining was done? That would at least let you work with a thicker piece while drilling the holes to minimize any tendency for thermal effects to have an influence on straightness of the workpiece.

How many holes? A mist system might be best, if not, manual lubrication at withdrawal of each peck cycle would probably be mandatory.

Dave

[BCRider]

Without running out to buy anything new what about starting out with a bit of scrap and a stock jobber length drill bit? Start with a brand new bit and run up the speed to likely the top end that the press will provide. Use a little cutting lube in the hole. For aluminium WD40 is as good as anything. But something like Tapzall for alumium might prove better. And don't buy cheap asian bits. Buy a pack if you must of some higher quality drill bits so you know the ends are sharpened symmetrically. Otherwise you're starting with an impossible task before you even switch on the drill press.

I suspect that spotting off the hole with some form of spotting drill or a "D" shaped countersink shaped "engraving bit" would aid in getting a straighter start. If you don't start straight you have zero hope of finishing straight. Or you need a clamp on bushing/guide to ensure a good start.

Starting straight is where I think turning the work instead of the drill bit would come in handy. It aids in assuring an axial start. But there isn't a lathe made that can turn at the speed needed to PROPERLY drill with a 1/16 drill bit in aluminium. So that factor alone means you're pretty much stuck with a drill press.

If you find that there's no hope for a straight hole even with a good axial start then there's no hope of doing this with a long aircraft extension drill either. And little hope of having holes from each end meet in any way that gives you anything that can be used for passing a wire down.

This good axial start would involve not moving the part at all once you spot drill the starting point. You need to be able to remove the spotting drill and put in the 1/16 drill without any table movement at all. Only the quill can be moved.

Try it, I'd love to hear about the results.

[skunkworks]

it is probably a hundred or so.. The design is very fluid at the moment

the actual spotting/drilling would be done on a cnc...

sam

[BCRider]

Check this out;

http://media.guhring.com/catalogs/hbkbyevb0ee.pdf

It's a page about deep "gun drilling". It looks like the drill bits are categorized by being able to drill so many times the diameter. In your case 4 inchs at 1/16 is 48D. So it's within the range possible with the styles 5647 and 5648. No idea of cost or special jigging beyond finding that there's a product that looks like it might work for you.

There's another option that might be worth considering which could result in excellent accuracy and little or no risk of runout. EDM.....

[skunkworks]

I actually thought about edm... I don't know if I am there yet - we have a edm that is 'some assembly required' and with no experience yet - I would not want to start with that project.. maybe in the next revision

sam

[enginuity]

Can you drill it from both sides? How close do they have to meet up?

[Mcgyver]

The first question is, can you design something easier to make - ie larger hole with a couple of 1/16 bits loctited in each end, and so on.

If you absolutely positively have to do it as described, it is do-able but time consuming. I held a 1/8" hole to a couple of thou over 4" and more than once. 1/16 will be slower and a bit more of a challenge.....post 19 here tells you how http://bbs.homeshopmachinist.net/threads/43014

[LKeithR]

...Alignment and accuracy is not a problem...

The best equipment in the world isn't going to keep a 1/16" drill that long from wandering. The only place you need "alignment and accuracy" is when you're starting the hole...

My first suggestion is to shoot the engineer, and then have a beer and celebrate the end of the job...

Yes, your first step is to redesign your part so you don't need a hole that deep. Unless this is something you can sell for a lot of money in relatively small quantities you need to rethink it if it is to be a practical and viable product.

...the actual spotting/drilling would be done on a cnc...

CNC isn't a magic bullet that will overcome the difficulties this job will present. It'll just help you to make scrap parts more quickly...