Profile cut small holes

[tri4sale]

I have a design I need to put about 50 holes that are 5/16th in diameter in 3 different boards (so about 150 holes total). First time I've needed to cut something like this. Searched but didn't find a match but that maybe because my search skills are lacking

Cutting into rough sawn oak, about 1 inch thick.

I went with a profile tool path (Aspire said profile cut was going to be a lot faster than pocket cut for the holes) , using a Whiteside UD2101 bit (.25 diameter). I think RPM is at 13000 (not in front of machine, going from memory). My thought is profile cut the holes, won't be any waste cause the bit is not much smaller than the holes. Using that bit for the other cuts, so keeping tool changes down was my other goal.

Well, this didn't work, started burning, so quickly stopped the cut.

While a drill would be best solution, I don't have that option on my
machine (4x8 PRS Standard). If I used a smaller bit, I have a UD1600 which is a downcut 1/8" diameter bit, do you think I'd end up with same burning issue? Changing bits really isn't a big deal so I don't mind swapping out bits if I have to.

Or is there a better solution for cutting the holes? The wood is 1 inch thick, but the final product is 4 inches thick so I need the holes to line up which is why I wanted to do the holes on the bot. Open to suggestions and advice. Let me know if you need more info or if pics would help (can get those when on other computer later)

[srwtlc]

Try the same profile toolpath, but add a spiral ramp. Pass depth will dictate the number of spirals. If you saw burning before, check that the tool is still sharp. Dial down the RPM and maybe up the feedrate. Higher Z feedrate will help the spiral ramp. Is that number bit a compression bit? If you can deal with a bit of chipping on the surface, use an upcut instead. The up compression portion of your bit could be dull and then the downcut portion will push chips back into the hole, causing more heat.

[scottp55]

Scott is dead on, but just want to amp that changing X,Y feeds will do almost nothing to cool bit down, it's all Z plunge and RPM to keep bit cool.
Do test cuts in scrap until bit stays cool. 1/2Diameter passes works well, and is so quick you can barely tell it's spiraling.
scott

[Burkhardt]

To add to the previous recommendations...for the spiral step down set the feed rate and plunge rate to the same value, for your holes I would suggest something like 0.5-1 ips.
I know Vcarve has the funny habit of applying the lower speed of both values to spiral paths which can cause burns if plunge is set very slow. I suspect Aspire will do the same.

[tri4sale]

Went back this weekend and made some changes. Picked up a Freud up-cut bit, 75-102 (solid carbide, 2 flute upcut finishing bit, 1/4" Diam, 1" cutting length)

Setup a drilling profile for the bit in tool database, w/ spindle speed 10,000 RPM (thats as low as my router will go) and Feed / Plunge rates at 2 IPS, and 50% for pass depth and stepover.
Seupt the toolpath as a profile cut on the inside, with a spiral ramp.

Attached are screen shots of those settings.

I then ran a test cut on scrap wood, 50 holes going 1 inch deep. Here is link to youtube video showing cut (without dust collector so could watch the cut in case it started to burn): https://youtu.be/CjWS2uupWq4

Results were good, I don't see any burning, holes look good, will need to do a little cleaning up at hole entrances but nothing major.

I'll do a production run soon and see how it goes. Any other suggestions / tweaks?

[scottp55]

Looks about right Daniel....was bit still cool(or slightly warm)?

[tri4sale]

I forgot to touch bit to see if it was hot or not. I'll do that next time I run a cut, might use a temp laser to see what it says.

[Burkhardt]

If there is no burn and the hole diameter is correct no further recommendation. A conventional cut direction tends to create a hole that is a few 1/1000" bigger than when cutting climb direction. I sometimes have to experiment before committing to the real part.

For holes deeper than one diameter and if you have to use a downcut bit to avoid tearout I have had good success with a small air nozzle (20psi) strapped to the spindle and directed at the bit tip (about 2" distance). That will help clear out the dust while cutting and not have it compacted to a burnt cake at the bottom of the hole. Actually I use the same nozzle for any deep slot cut with a downcut bit.

[Ajcoholic]

I wonder how a single flute bit would perform VS a typical two flute? It would be interesting to try. I generally spin my 1/4" bits around 11,500 to 12,000 when I am "drilling" holes using a spiral tool path. I used to do a lot of shelf holes in solid wood before I bought a boring machine. Never tried one, as I had no burning issues either. But it seems in a deeper hole, the more room/clearance for waste in a single flute might help?

[Burkhardt]

I wonder how a single flute bit would perform VS a typical two flute? It would be interesting to try. I generally spin my 1/4" bits around 11,500 to 12,000 when I am "drilling" holes using a spiral tool path. I used to do a lot of shelf holes in solid wood before I bought a boring machine. Never tried one, as I had no burning issues either. But it seems in a deeper hole, the more room/clearance for waste in a single flute might help?

Good question. I never tried that as well, maybe because my single flute bits tend to short fluted and not usable for any deeper hole. But it may well help.

Forgot to mention...if the hole is really drilled at bit diameter or milled only slightly larger I found it helpful to peck drill in max. 1-diameter steps to prevent flute clogging. The profile cut in Vcarve does not have a peck option (I know of) but using a pocket path will retract after each layer automatically. Takes of course longer.