A drilling question

[Acmeaviator]

Is there a type of drill bit that is best suited for use in a router? Can I use the same bits I use in my drill press - assuming they can handle the 10k rpm minimum on the router?

[curtiss]

I have used small drills from time to time, mostly 1/8 and some 1/4 inch.

I believe a downcut for drilling can heat up and cause a blaze, especially if it cuts into the vac plenum.

Sometimes you can just use a small bit to mark out the holes and then use a regular drill to finish the job.

[ken_rychlik]

Depends on size. I use a 1/4 inch straight router bit all the time for drilling shelf pin holes.

[Coleman Becker]

i usually mark the center of the hole and the outside of the hole with a v-bit then drill it out by hand

[wberminio]

Brian

Are you drilling for shelf pins or large holes?

For shelf pins I use 5mm boring bits with carbide tipped brad point.

[erik_f]

I wouldn't use drill bits they normally aren't designed for that kind of RPM. I guess it depends on what size hole you are looking to drill also. Usually I just use the bit I am cutting with to do any drilling that needs to be done. Make sure you take a couple passes at it just like you would if you were drilling by hand.

[geneb]

I haven't tried it yet, but could an HSD 2.2hp spindle do an adequate job of drilling with the RPM set to say 1800-2000?

g.

[bleeth]

The small spindle will do a fine job.
There is crossed info below that needs a bit of clarifying. If you are talking about drilling standard substrates like mdf. pb or ply, for shelf pins or hing holes and therefore aren't going too deep then you normal cutting bit (down or mortise) will work fine. I use a mortise and a peck strategy retracting to "0" to clear some of the chips before I go to the bottom of the hole which is .4375 deep and leave my spindle running at 16-18K.

If you are talking about drilling all the way through the whole game changes!!! This is the way fires are started as the substrate can get really hot. You need to be careful there. Due to the danger and the limited attention span of some of my operators I stopped doing the divider panels between 2 drawers in one cabinet which we were drilling all the way through so both sets of drawer slides could be drilled as the cabinet. A slower spindle speed and careful pecking is critical when doing that with a down cutter and especially a mortise bit. Even with 4 pecks there was still noticable blackening of the hole (and smoke!!) with the spindle spinning at the same speed as for cutting when trying it with the 5mm mortise we standardly use for all our cab parts and no bit changing. The issue was not as bad for a downcutter but I get more clean parts out of a mortise bit between table surfacings.

[dlcw]

I use boring bits, which are designed for this application, in my 2.2hp spindle. I set spindle speed at 2500 RPM and have never had any problems.

[Acmeaviator]

Great feedback - I need to drill .5" to 1" holes centered in some large plywood gears. The holes need to be "perfect" - previously I have used my drill press but the gear diameters are to large for my press to work. I've got a router equipped BT48 so my slowest speed is 10k. I'm going to experiment with some different router bits and see what I get:D

[bleeth]

Brian:

For holes of that size I would use a 3/8" bit and an area clearance strategy in toolpath and not drill at all.

[Acmeaviator]

Dave should that be a straight 3/8 bit or a spiral bit?

[Brady Watson]

A spiral will evacuate the chips better than a straight. Use a helical ramp on an inside profile.

Regardless of what tool you choose for drilling, it MUST be center cutting - meaning, hold it in your hand and take a good look at it's center. If there isn't a cutting edge in the center, like that non-center cutting H-shaped 2-flute straight, then the material has no place to go & you'll be killing your spindle/router bearings and probably stall the Z motor.

I don't buy 2-flute 'upcut spiral' router bits anymore. They are more expensive as a router bit than a standard center cutting end mill, they are made from inferior carbide, they are lower tolerance and they are not truly center cutting - and the helix is identical to an upcut spiral router bit...

-B

[bleeth]

IMHO straight bits have no use in a cnc cutting wood of any kind. Use a down cutter or mortise. Brady is right about endmills generally being a better grade of carbide then many wood bits. That being said, since I refuse to consider the likes of Freud, Vermont American, Bosch, or Ridged bits suitable for CNC as well as many other companies router bits, I use only better quality solid carbide bits made for the purpose. Generally I use Centurians, Onsruds, and some Whitesides as well as a couple of manufacturers of specialty bits and those who only come through commercial distribution.

For a tooling strategy for holes like that I will use an area clearance and offset path style starting at the inside with a large (90-95%) stepover. That way the bit will start at the center of the hole and move outward so there is no "center plug" to go bouncing around when the hole is done.

I'm conservative about how deep I go in one pass so for 3/4 ply, etc I will use a couple passes with a 3/8 bit. They come out pretty darn clean on my bot but I am running a 5HP spindle and not a router. I use the same strategy to pocket for hinges like big Soss for jambs and it leaves a very sweet mortise. Although I cut more oblong slots of similar size than round holes this has worked for me for years.

[geneb]

At those hole sizes there's no reason you can't just pocket them out with a 1/4" cutter...

g.

[Acmeaviator]

Thanks for all the help gentlemen - dropping the feed speeds and using a pocket toolpath instead of a drilling one helped immensely. For most parts the drilling is no big deal, but the arbor holes in my clock wheels - especially the escapement wheel - need to be perfectly true. On the plus side I'm greatly enjoying watching the bot machine perfect wheels in minutes that I used to spend hours making on my scroll. Nothing ruins a beautiful day like notching the 119th tooth on a 120t wheel:eek: