Drill Toolpath

[IslaWW]

Assuming you have the HP to push it you can pretty aggressive with the spiral profile method. Here is some drilling in Phenolic with a straight flute bit. 1/4" bit doing 5/16 holes in an aggressive fashion. The drilling is in the first 15 seconds

[ken whiklo]

The bit I was using was brand new. So not the bit.

The bit (end mill) may be sharp but the problems still could be with how that bit is used.

Adrian mentioned the first thing that came to my mind: if the bit is a down-spiral then even with a soft (Mohs scale soft) wood you'd get burning especially with the slow feed rate and rpm you were using.

We still have no confirmation about whether you were using a down- or up-sprial bit.

The second thing that came to mind is that the feed rate and rpm are excessively slow. The chip-load for your speeds is around 1/1000" for a single-flute bit. Charts I've seen suggest for hard wood that this be 9/1000" to 11/1000". Thus the very fine dust you are getting is given a chance to scorch the holes.

For a single-flute cutter at 1/4" I'd probably start with 75 inches/minute (my machine's max Z rate) at 8000 rpm. With rock maple i'd probably be conservative and use 1/8" to 3/16" pass depth with peck drilling retracting to 1/8" above the material surface.

Even with a 5HP spindle I don't really like running less than 10000 rpm.

I've never used a twist drill in the router as it is so difficult to get the rpms slow enough. Easy for a drill-press not so for a router spindle. Besides, single-flute end-mills work just fine for me in MDF, plywood, solid wood, HDPE, and anything else I've need to drill multiple holes in.

Adrian's spiral ramp trick works a treat too. I've used it recently to drill a number of 5/8" holes in 3/4" plywood with a 3/8" cutter in "one pass".

Steven

Thank you. I tried your settings and got the first holes I have been able to machine without burning.
I have said it before but it bears repeating. This forum and the experienced users who offer advice are just another benefit of using Vectric software. Thanks to all for chipping in.

[tomgardiner]

I done thousands of holes in solid and ply with carbide brad point bits and HSS twist bits. I have run a 1/4" bit at 6000 rpm and 200 in/min plunge. Peck drill only if you experience chips packing in the flutes