Drilling Straight? Experienced Machinists Inquire Within

[Cartierusm]

Ok, I've been working with tools all my life and been a home based, advanced, cnc machinist for about 8 years. Whatever I know about drilling straight is just from experience, but now I'm at a point where I need a little REAL information about how to drill straight holes on my CNC Mill.

The reason I'm asking is I've got some up coming projects and I'll need lots of special size drill bits and the cost difference really adds up between types of drills and would like to have some information clarified.

Normally when drilling on my CNC Mill and the hole needs to be straight I use new or good condition 135 degree split point drill bits, high quality ones from my local machinist supply. Regular sizes are not expensive. I don't spot drill and I program it at 10 to 15 IPM and peck .03" down at a time. I machine lots of aluminum so this is what i've found to work perfectly. And in my time I've had to drill some very precise holes.

But now I'm getting into some gunsmithing areas and need lots of special sizes and if going Split Point it can get expensive.

So my question is can I get a straight hole from a regular good quality drill bit? If so what is the procedure, I figure I would still use 10 to 15 IPM, .03" Peck. Would I use use a spot drill to go down 1/16" to get it started or should I do that, then drill down with a smaller drill. And if so how deep and what kind of bit?

For example I'm going to be drilling 2" into Aluminum with a .154" drill bit. How should this be done? or drilling down 4" with a .093" drill?

Thanks in advance. If there are some articles out there already with this info please direct me to them. I've googled but didn't find anything.

[neutronics]

When drilling those deep holes, are you drilling through solid material or drilling through two bulkheads with a void in between? (As in take-down pin holes for an AR receiver.)

[Shane123]

i always use a keo center drill to spot my holes, even with carbide drill bits i go down .05 just to make sure when i plunge i dont start with any walking. with the keo #4 or #3, you could easily go down .150-.2" to help make sure you go in full corner depth of the flute before you add extra pressure to your drill tip.

[HuFlungDung]

I'd definitely recommend a spot drill with the same angle as the drill point to follow. A lathe center drill does not produce a stable conical depression to guide the drill point, and it is important to avoid that critical wobbling of the drill as it tries to get started on top of the hole. I'm talking about dead on accuracy, versus close. I've tried in the past to drill cross holes through round shafts, dead center and could not maintain position closer than +/-.001" with a center drilled hole. Switching to a spot drill solved the problem immediately.

It makes some sense that if the start of the hole is less than perfect, that it is not going to get any better, the farther the drill has to go in.

In a super critical situation, it might make some sense to drill a starter hole and bore it a little ways, to serve as a sort of guide bushing for the long drill.

Try using a parabolic drill for deep hole drilling. I find that the chips tend to travel much faster up the flutes, which can result in less chip packing. This might mean you can take two or three chip-breaking pecks before a complete retraction is necessary to clear the flutes. I like the Haas high speed peck drilling cycles, as they permit quite a variety of permutations to drill a hole nearly with the exact strategy that one would write out longhand.

BTW, I run my drills at a conservative feedrate around 6 to 8 ipm in aluminum, at 400 sfm (for a high speed drill). Although one could boost the feedrate higher, I think a higher feedrate increases the tendency of the drill to wander slightly. When you have an extra long drill in the spindle, you don't want it to bow under the feed pressure, because that creates another source of random error. But you want enough feedrate to ensure chip flow up the flutes of the drill. Too slow, and this won't happen, and you'll be restricted to tiny peck distances.

[Cruiser]

The key to a straight and true drilled hole is having the center point exactly dead on and the angles match exactly. I have found that brand new quality drills are not perfect. Because of this I purchased a drill doctor 750 and would dress my new drills slightly and was shocked as to how far off they could be, and, I did my own split points. Another point that can help is using a pilot hole to get things started. The pilot must be true and straight to start with tho. I have used an end mill and formed starter holes slightly under size and deep enough for the point of bit to enter fully before engaging material. If not using any pilot the bit might have a tendency to be just slightly out of position and from then on it is drilling at an angle and the error will be noticed at the exit on opposite side of part. I never trust a drill to center itself without a starting spot if it is small enough to be flexible, also, trusting a center punch spot for a precision hole is a no no as the punch spot can be off more than the machine and the bit can deflect at center spot and be at an angle all the way through.

[Cartierusm]

Great thanks for the help. I'll definitely get a REAL spot drill. So if I spot drill down a 1/16" and use regular drill bits and not split points I'll be all right?

[RICHARD ZASTROW]

You might also try this method: Start an undersized hole, BORE the hole larger to provide the equivalent of a drill bushing, then use above methods and drills to complete the hole length.

We used this method to drill 5/8" holes 26" deep to meet another cross-drilled hole on an injection mold. Hit it right on.

Dick Z

[Caprirs]

The parabolic drills are definitely helpful with deep holes. They will allow for more aggressive pecks and are better at evacuating chips. I agree with the others that creating a bore with an end mill can make an excellent guide for the drill bit.

Be sure the drill is running concentric in the spindle too. Fighting a drill chuck that wobbles excessively can drive you nuts, whether on the spot/center drill or the finish drill.

Also, do not underestimate the importance of having the spindle and head trammed and square to the table. If the head moves perfectly perpendicular to the table but the spindle is not square to the table, the difference in length between a stubby spot/centerdrill and long drill will result in the drill being off center when it makes contact with the workpiece and result in bad holes.

[Cartierusm]

Thanks for the great info. I appreciate it. As for tramming a few years ago I finally got one of those dual dial indicator tramming devices from ebay. Helped a Ton.

The drill bushing idea is great too. I often use endmills as drills in my work. I usually drill a regular hole .06 or more undersized, enough that the center is gone so the endmill doesn't work too much.

Neutronics, how did you know . I've never liked the way most people machine their AR15 lowers. I've been a machinist for a long time and the way most people go about machining an AR-15 lower is ridiculous. All these people machine the outside shape first, who cares how it looks as your machining it.

The way I designed it and wrote the g-code was I mill the block of Aluminum to exact size first, then go about each side milling and drilling so there are no fancy jigs to sandwich the part in between. Then I have one jig double sided, one flat with dowel pins and one side with the bumps to hold the part level once one side is surface machined also with dowel pins. This way I never need to use a weird jig and spend time locating the part on the mill. I have a vice stop that is X0 Y0, so I just slide the block in and everything is located for me. So after I machine front, back, top and bottom I lay it flat with parallels and machine the holes and slots on the right side. then put in the jig and slide the part on two 1/4" dowels and an 1/8" dowel in holes that are there naturally from the right side drilling op. Then I use one bolt to hold it down do my 3D machining. Flip the jig over put the part on and mill the Left side slots and 3D. The jig has angles machined into it so one side butts up against the vice stop and rests on the angle for the grip hole and then flip around and mill the hole by the threads for the buttstock detent. Very simple.

[BobWarfield]

Originally Posted by Cruiser The key to a straight and true drilled hole is having the center point exactly dead on and the angles match exactly. I have found that brand new quality drills are not perfect. Because of this I purchased a drill doctor 750 and would dress my new drills slightly and was shocked as to how far off they could be, and, I did my own split points.

+1 on Drill Doctoring. It is amazing how quickly bits get dull, how far off new bits are, and how much you didn't realize your bit was dull until you get in the habit of using newly sharpened bits. Once you see how it is supposed to cut, you know what to look for.

The Drill Doctor just makes it super quick and easy.

I'm also a big fan of screw machine length bits wherever possible and of putting the bits into ER32 collets if I'm really being picky about the hole.

Cheers,

BW

[Cmailco]

Typical procedure for deep hole drilling is to drill 2-3D deep with a pilot drill. Some companies make a "pilot drill", which is basically a drill/chamfer bit or you could just use a short carbide drill of the same diameter with an included point angle 2-5º GREATER than the drill used for the hole.

That said, you should always use a starter with a point angle greater than the drill's when drilling with carbide. HSS/cobalt drills will likely survive the entry just fine either way.

Same basic concept as Rich mentioned but much quicker, should you need to do this in a production setting.

Basic procedure:

Enter the hole at 100 sfm, feed to .020 from the pilot's finish depth at .010 in/rev, correct the spindle speed, turn on the thru-spindle coolant and feed to final depth - no pecks. Retract drill to feed start point (.020 from pilot's finish depth) at 120 in/min, lower speed to 100 sfm, exit the hole at .010 in/rev.

There are a whole slew of factors affecting hole straightness but 90% of the battle is in making a good start and keeping chips out of the way. TIR can be corrected with an adjustable hydraulic or "BullsEye" chuck. I guess the one thing you can't control are workpiece inclusions....

[MikeZee]

Home based, advanced cnc machinist, 8 years????? I been doing this for forty years and do not call myself " advanced ". Who cares how much a bit costs, that gets passed on to the customer, and if he's getting good product he won't care either. But I'll tell ya,
drilling .093 thru' 4" of anything is a tall order. It's a long procedure and I don't type that fast. Good luck.