# Drilling holes with a CNC Router



## MF2015 (Jul 14, 2015)

Hi all, I was hoping to get some input on how to drill holes with a CNC router. I need to drill 1/8" and 1/4" holes in 3/4" Baltic Birch. I did a setup using an 1/8" (and 1/4") end downcut plunge bit, and what happens is as the bit gets lower in the wood it generates smoke, my router will only go to 10,000 RPM. I use vcarve and mach3. 

Is there any advice on how to drill holes, either setup or bit to use? 

Thanks


----------



## Stick486 (Jan 4, 2013)

try an up cut...
a down cut won't clear the chips and that's what id burning...


----------



## 4DThinker (Feb 16, 2014)

If you have a 1/8" chuck then use a 1/8" drill bit rather than a router bit. Just don't use the drill bit for anything other than 1/8" holes.


----------



## tooler2 (Aug 11, 2012)

On a CNC milling machine you would use a canned drill program for each hole it involves pecking the bit.
Rob


----------



## SteveMI (May 29, 2011)

I make cribbage boards with 150 to 600 holes in each one with V-Carve and Mach3. As Rob pointed out, use the pecking feature of V-Carve. I have had good success with the RU1600 Whiteside 1/8" upcut. I'm sure other brands of 2 flute upcut will work.

All my cribbage boards are made with solid wood, primarily red oak and maple. 

Plywood can be a challenge with that diameter. My experience is that the 4' x 8' plywood sheets are made with an exterior glue that can be gummy with smaller diameter bits or endmills. The 5' x 5' sheet plywood is interior grade and uses a glue that is more friendly.

Steve.


----------



## MEBCWD (Jan 14, 2012)

Stick486 said:


> try an up cut...
> a down cut won't clear the chips and that's what id burning...





4DThinker said:


> If you have a 1/8" chuck then use a 1/8" drill bit rather than a router bit. Just don't use the drill bit for anything other than 1/8" holes.





tooler2 said:


> On a CNC milling machine you would use a canned drill program for each hole it involves pecking the bit.
> Rob


All of these suggestions hold true. 

First, generate your toolpath with the drilling toolpath in V-Carve, use the peck dill option in the program to clear the chips.

Second, don't use a down cut end mill, it will pack the hole full of chips and cause burning or worse it could cause the bit to be forced off line and drill an oversize or out of round hole. Use a drill bit or upcut end mill with the proper speed for the drill/mill and peck drill. 

Remember if you use a drill bit for the hole do not use it for other toolpaths. Drill bits are design to drill holes not to cut grooves.


----------



## MF2015 (Jul 14, 2015)

Thanks everyone, that's great feedback and I will try an upcut. I have been using peck but with a downcut. One question I have about using a drill bit is my router will only go to 10,000 rpm on the low end. Is that to fast for a regular drill bit?


----------



## 4DThinker (Feb 16, 2014)

I ran a 2x4 piece of BigBox cheap plywood for a student... 1/8" holes 3/4" on center over the whole panel. "Good" .125" drill bit in a router that also only went down to 10,000rpm. Seemed to work fine. Holes looked good. Took what seemed like forever with all that pecking. No problem packing the hole or the bit, but you might have better luck with an upcut spiral in hardwoods.

You can go deeper with a drill bit than most 1/8" end mills are long. Reason I tried the drill bit for holes in 3/4" plywood.


----------



## Ryan360 (Jun 22, 2015)

if you have your speeds right it shouldn't smoke. Unless maybe its dull. =)


----------



## fixtureman (Jul 5, 2012)

You could chuck a 1/8 upcut end mill and use the peck drill for the 1/8 holes then use a pocket tool path with the same 1/8 bit no need to change


----------

