Hi. I’m looking for recommendations for drilling hardwood and peck drilling.
My guitar projects have a range of holes needed with 5/64"to 3/16" diameter at depths of .75" to 1.1875". I bought 2 flute 118 degree drill bits with enough reach for these depths (some still on order). These are rated about 1500rpm on average.
These aren’t extremely deep holes but I’ve only ever done this on a drill press with precision HSS brad points at much slower 1500rpm average. Manually pecking roughly the bit diameter each stroke until final depth. One set of holes actually needs to go through the full 1.75" thickness. Those I do half from either side meet in the middle with locating pins to avoid bit wandering in wood grain.
I’m using VCarve which has two Peck options for partial and full retract. I don’t think Motion supports the actual Peck G-code. The Shapeoko PP is creating simulated peck cycles in the G-code by repeated incremental G1Z down followed by G0 Z up retract actions. I’m a bit worried that hundreds of short rapid Z up / slow Z down moves over a batch of bodies will be hard on the machine (5 Pro). Also worried about breaking a bit in the material.
I’d like to hear anyone’s thoughts or experiences with this type of drilling and possible effect on the machine. Thanks…
A few thoughts:
1: your spindle is probably way too fast to be using drills that aren’t specifically rated for high speeds. Pretty sure the lower end of your spindle is ~8000rpm.
Even if they don’t fail catastrophically, I’d imagine they’ll be terribly unbalanced and wobble like crazy at high speeds. Probably not a great hole. (Get some rated for the top end of your spindle. Maybe 24,000rpm?)
Pecking is pecking regardless of which code generates it. The motion will essentially be the same (assuming create doesn’t do anything too terribly silly under the hood). If you’re comfortable with a regular pecking cycle, you’re probably going to be comfortable with whatever create pops out.
With your larger holes, you can probably get something like a long reach endmill and interpolate your holes to size. Might be useful if you have a hard time sourcing rated drill bits in the proper size
I wouldn’t be too worried about the repeated motion of the z axis. Generally speaking, these components are rated for far more than we tend to throw at them. If you do wear it out, you’ve likely made whatever that cost is back many times over
For your full depth holes, if they’re the larger holes I bet you can find a tool to do it from one side (assuming you have the z-height available for such a long tool). If they’re the smaller holes…I don’t have an idea for you, maybe somebody else will
I feel like chip evacuation is going to be a big part of clearing your holes without breaking a bit. I did a project recently with deep-ish ratio holes and an air blast was the difference between occasional snapped bits and an extremely reliable operation…it was only a 1mm hole and only a few mm deep but I feel like the lesson still applies scaled up.
Doesn’t answer all of your questions but hopefully more experienced folks will chime in to answer whatever remains (and correct whatever I got wrong )
Thanks I appreciate the info. I may be worrying about the rapid movments for no reason.
I’m running the 65mm spindle which has the low end rating of 8000rpm. I found 1/8" and 3/16" drills from Amana and IDC rated for CNC speeds. The through holes are 1/8" and IDC sells one with long reach marketed for wood cribbage boards.
At first, I thought as you said, for the odd sizes like 3/32 and 5/32" I’d use a 1/16" or 1/8" long reach endmill to do a micropocket rout in several passes. Well I drew that up and I saw the toolpaths with those tight circles and thought this seems like a step backward. It shouldn’t be more complicated to drill a hole with a CNC than it is without one. Almost all my manual drilling was done with drill bushing fixtures which prevent wobble - I definitely don’t want oversized holes.
I ordered a few collets from MariTool and saw they have a line of screw sized solid carbide “machine drills”. The small sizes were $8-12 I plan to test peck drilling with those on scrap unless folks here convince me its sheer folly - not going to work or safety hazard. If that doesn’t work out I’ll try the interpolation route.
The compressed air is a good suggestion. I’ve been making do with the coarse method of an outdoor leaf blower lol I need to get a proper setup. I’ll look into that. Thanks…
Hello…I have some real wold feedback I thought I’d share. It is interesting. There is a surprising dearth of information from technical sources about drilling in wood on a CNC. What little info there is varies widely from you can’t possibly run a spindle low enough for a drill bit to you should run it at 20K.
Drilling into 1.75" thick basswood a rather soft hardwood
1/8" holes .92" deep with IDC “Lightning” bit. Used vendors speeds of 17000rpm/60im plunge.
3/32" holes .86" deep with MariTool Carbide drill. No vendor spec with some trial and error landed on 15000rpm/40im plunge
3/16" holes 1.2" deep with Amana Carbide drill. No vendor spec used 14500rpm/55im
All 3 the pecks were bit diameter increments. I manually edited the retract to Z0 to run at the same speed as the plunge, not Rapid. The first test with the 3/32" bit I started with with Rapid up retracts, but once it got a few pecks in the rapid up move visibly grabs the workpiece and attached fixtures and pulls it up violently. Scary!
Otherwise no issues… With the retracts set to non-rapid I could see micro-chips flying out and sucked away by Sweepy. I will still look into the compressed air idea.
)