1. ## Breaking Drill Bits

First off, I know about "Feeds and Speeds." I even know the formulas for calculating them; and for the most part they seem to work quite well for me.

It's when I use the really small drill bits that things tend to go crazy.

Here's an example:

If I use a 7/64" HSS Tin coated drill bit I can use either the mathematical formulas to calculate my Speeds and Feed or I can simply use the Speeds and Feeds Wizards. Either way, the numbers I come up with aren't too much different from each other.

Lately I've been having to use really small diameter drill bits. It's these small diameter drill bits that snap like glass rods; both the cheap ones and the expensive ones. From 7/64" on up I have little if any problems with breaking drill bits.

Anything smaller than that is an exercise in frustration.

I've ended up having to do all my small hole drilling with a hand-held cordless drill just to keep from breaking my tiny drill bits. (.064 range)

The only thing I haven't tried yet is setting my 770 on the lower speed pullys and drilling at the same RPMS as my cordless drill. The reason for this is that I've broken all my tiny drill bits.

What are the smallest drill bits you guys work with on your CNC mills and how do you avoid breakage?

MetalShavings

2. Make sure your head is tramed and z is traveling square to the table. That breaks small drills quite easy. Rpm, the more the better as well.

3. For small tools, drills/mills/whatever, the rules change some, because the tools are more fragile, and it is more difficult to evacuate the chips. So, you have to go more gently. Generally, I think the rules work OK for calculating appropriate RPMs, but you need to reduce the feed. For all but the most shallow holes, you also have to "peck drill", which means drill a short distance, then retract the drill to clear the chips. The deeper you go, the more difficult it becomes. Drilling really deep holes (like 5 diameters or more) can get very challenging. Coolant also helps a LOT.

Regards,
Ray L.

4. yeah, the feed will certainly get smaller with the delicate drill bits, but most important are using screw machine length bits for holes <2d and parabolic bits for deeper holes. If you are using standard jobber drill bits you will be ripping your hair out.

5. Oddly enough, I've done most of the things you guys have suggested, with the exception of the "screw machine length bits."

I can tell by the sound of the breaks that these little drill bits will go just so far then the tip will gum-up and catch.

I guess when they invented CNC mills they really didn't have these tiny little drill bits in mind.

I'll have to back my feed-rate down to next to nothing and twiddle my thumbs while I wait.

Thanks for the input everyone. In the back of my mind I was kind of hoping there was a trick to getting these little drill bits to perform like the larger bits.

MetalShavings

6. Do not make the drill to work too long, and not too high speed. When drilling deep holes, keep often to clean the drill bits, prevent drill chips blocked and the drill bit was broken. When drilling, to add some coolant, thus reducing the rapid wear of drill bits due to high temperatures , to extend the drill bits life.

7. If you have any backlash in the Z axis this could be getting you in trouble.. Other than that I tend to use a good oil instead of coolant in the lettle bits.

If you have to you could get you one of those sensitive drilling chucks. Let the CNC machine possition the bit, then use the sensitive drilling chuck by hand to drill the hole.

LittleMachineShop.com - Sensitive Drill Feed and 1/8" (3 mm) Keyless Drill Chuck

Jess

8. I have had the same problem (and still do) with 0.05in drills on aluminum. I got better at it but never found a perfect solution. What I do and lower my breakage rate is: make sure you have little runnout, use the short drill bit type, spot drill first, lower the feed, peck drill, put some w40 (I even have a special lubricant for aluminum forgot the name but it does not seem to help much more than w40) and rub the bit with a piece of wood when it is out and still spinning, before it goes drill another hole. That helps remove the chips. It seems to work ok with all of that combined but I cannot leave the operation unattended or it is certain I will break a bit before the 10 holes are drilled, usually after just three or four. The holes are 1/4 in deep by the way which is a lot for such a small drill bit. I also bought some expensive drill bits recommended for aluminum and it did not noticeably improve (I dont remember the brand). I tried running the spindle to up to 10000rpm but it seems to get worse so I stick with 5000rpm. I can't remember the feed but I think around 1ipm. That was not what was recommended to me but after experimenting a little that's what I ended up with.
I would be happy to hear from more experienced machinist what are their trick.

9. We do .002-.004 diam drills all the time. Hardly ever break one in the cnc. Spray mist, lots of rpm, lots of small pecks. 20k spindle though.

10. underthe tire,
What feed per rpm do you use? Even at 20K rpm that is still only about 10 fpm for .002" drill... nice and slow. Are the drills single flute or two flute?

11. My mill's max RPM is 10,000.

What gets me confused is the fact that when I use my cordless drill to drill with these same small bits, I get no breakage and I'm using no lubricant.

I've had to order some more bits so it will be a while till I can experiment some more. I'm thinking that at a certain diameter, traditional Speeds and Feeds don't seem to apply any more. In the field of photography, this type of phenomenon is referred to as the "Law Of Reciprocity."

On my next go-around I thought I'd try to set my RPM to match my cordless drill and apply over-exaggerated Retraction-Heights along with lubrications. That way every thing's moving slow enough where I can stand in front of my mill and manually remove any material build up that tends to gum up the tip of my drill bit.

On my last project I had to drill 15 holes at .0625 diameter. The depth of my holes was set at .621". None of my bits made it beyond .15-.20" before snapping; unless I used my cordless drill; then I have the problem of drilling non-vertical-non-symmetrical holes.

Like most of you who have experienced these types of setbacks, I'll keep plucking away at it till I find the method that gives me the best results with the least amount of breakage.

I was just hoping that one of you fellow CNCers had found the "Holy-Grail-Method" of using these tiny drill bits. It appears that there really is no such thing; with respect to very small diameter drill bits.

MetalShavings

12. At very low feed rates the Z-axis will move in discrete steps, it's a digital device. A cordless hand-drill is an analog device.

Phil

Page 1 of 2 12 Last