Hi Everyone,
I’m testing out making a guitar body on the small CNC, which requires precise drilling of pilot holes to interface with another part that I’m making on the laser. I’ve done some research and the use of drill bits on a cnc machine for this application seems to be dependent on the machine itself being able to reach lower RPMs.
Would using a 1/16" drill bit on the small CNC be ill advised?
Thanks in advance!
Yes, you can use a 1/16" drill bit to drill holes. A carbide drill bit would be ideal.
Another option is to use a 120 degree spot drill to mark the hole locations. Then, take the part to a drill press and set the depth stop, drilling the holes manually. The drill bit will center in the pits, causing your holes to be in the perfect location every time.
If you buy a carbide drill bit, it makes only one diameter of hole, and it needs a rigid setup, so it’s not a very versatile tool. If you buy a carbide spot drill, you can use it to help you drill many different types of holes. (If you have a drill collection, you will also need a separate ER-20 spring collet for each shank diameter.)
If you drill, you will need to research the correct feeds and speeds.
Especially with larger diameter tools, helical boring is a better option. In your situation, drilling is fine.
I have never done it myself so cannot give any useful comment on the feasibility, but just wanted to provide a word of caution. I think it’s possible but it’s one of those things in the shop that’s more dangerous that it seems, and requires extra forethought. Forgive me if you know all of this already, but it bears repeating! 
A 1/16" drill bit in hardwood requires ~3,000rpm, whereas the CNC spindle by default provides ~21,000rpm, and its minimum is 6000rpm. Many of the issues and small fires we’ve seen related to the CNC are due to drilling toolpaths. People set up their cut incorrectly, and with poor chip clearing and high speeds on the spindle, it basically turns into a high-tech version of one of those rotating stick fire starters
Thankfully the only casualties so far have been some ruined spoil boards and ruined projects, but fires like that can be hard to notice and can grow quickly.
I think many times this is due to the user using an end mill rather than a drill bit, as drill bits are designed to clear chips better, but I’d be cautious either way.
The other important thing I think people forget is that the spindle speeds that you set in VCarve have no effect on our CNCs, so people will design their toolpaths and setup their cuts thinking they’re using a low RPM, but the spindle is actually spinning at 21,000rpm.
From the IQ manual, you must set the spindle speed on the VFD itself. 100hz/6000rpm is the lowest it should go, according to the manual. Perhaps 6000rpm would be slow enough to get decent results, not sure about that.
Please correct me if I’m wrong and you can set it in software, but this is what I remember from class a few years ago. @jamesfreeman or do you know @Rolo ?
Alternatively the way @aanne3 suggested is good too, just spot drill with a v-bit and move to the drill press
For reference, here’s the results of a time it happened in the past from drilling 5mm holes in maple plywood:
Here’s some advice @AlexSchoedler had when it happened then:
How deep is the hole? Are you using fusion or Vcarve? Does anyone know if Vcarve can do a peck drilling cycle? If your using fusion, you should definately use a peck drilling. This is where it will drill some, and then raise the bit to clear chips, and then drill some more.
I think the problem with a small bit like that is that it will load up quiuckly. If it cannot disperse the material, this is what will lead to burning, which is accelerated by the vacuum table.
My drill press at home goes up to 8000 (!). I just tried a 1/16 bit in some walnut, and it loaded up quite easily. If I peck drilled it, it seemed fine.
