I’m trying to drill compact HPL with Shapeoko XL, equipped with Makita Router.
The HPL sheets are 4mm thick, and the holes are 4mm in diameter, I’m drilling them one at a time, not stacked.
Unfortunately, we’re experiencing extremely high tool wearing. After 200 holes, we have to change / resharp the drill bit. We tried changing the drill bit, by using some strenghtened with 4% Cobalt with no results, 240 holes later it’s done.
We also tried to slow down the descending phase to 100mm/min, actually we also splitted drilling in four phases, 1mm at a time, with no benefit.
Equipment used:
- Shapeoko XL
- Makita router
- Drill bit: 4mm diameter HSS strenghtened with 4% Cobalt Cutting Feed and Speeds:
- Feed : 100mm / min
- Spindle speed: 10000 r.p.m. (minimum Makita’s rotation, higher RPMs results in louder, higher pitched noises and even less drill bit’s durability) Material to cut: Compact HPL, 4mm thick Numbers of drills per sheet: 20, after which there is an unloading / loading time of the sheets to make the tool rest.
I was wondering, are my settings okay? What do you usually use for drilling?
A friend of mine told me that he usually use 500 r.p.m. to drill hard materials, just the same as we do with our drill press. Unfortunately, it seems that there is no compatible router with those low speeds, which are bad for milling.
I’m a newbie of CNC and this forum, please correct me if I’m doing something wrong!
Thanks and have a nice day!
I do a reasonable amount of drilling with the VFD spindle in my Shapeoko, I run carbide drills, not HSS or other softer materials to keep a sharp cutting face, I only use steel drills in woods like MDF and they blunt quickly in those abrasive materials.
Seems like your chipload is very small and your drill is doing more rubbing and burning than cutting in the hole which will wear it very quickly, especially in an abrasive material such as HPL.
Take a look at this thread
I run a feed per revolution of at least 0.04mm in Aluminium, 0.1mm in wood and more in plastics based on both recommendations and experience. The carbide drills I buy are not expensive
I’m sure there are similar suppliers where you are.
Check out the recommended feeds in FR-4 from Precisebits here too
For a 4mm drill they are suggesting 20kRPM and 60 in/min (1,524mm / min in proper units) feed rate to keep the feed per rev up at 0.08mm/rev
It’s also worth bearing in mind that each drill and material combo has an optimum range of surface speed which you should stay within, this gives a working RPM range for a given diameter of bit, from there you work out what feed rate you need to keep chips coming out and not burnt up dust.
I run between 2k and 8k on the VFD spindle for drills in the 2-8mm range, I run at the bottom of the surface speed range so that I can keep the feed rate down so machine rigidity doesn’t become the constraint. If your router only goes down to 10kRPM then that’s going to set the min feedrate, then the rigidity and torque set the max drill diameter you can usefully run in any given material.
So, I suggest trying some carbide drills and jack up the feedrate.
Thanks a lot, I’ve asked to my local drill seller to buy drills for drilling with CNC, but I don’t know if he had something made to rotate at 10,000 RPM.
I see it’s kinda pricey, but I’ll give this tools a try, if I can get them in Italy
Thank you sir, I will try to get them, they doesn’t seem so pricey, I will have a look for a re-seller in Italy with similar items.
I’ll try to get a faster descent with higher RPMs, let’s see what happens.
It’s pretty hard to get the nice feed and speeds with different materials. As I’ve read online, there must be some trials and errors to get it work right, when the material properties and the drill properties are unknown.
The challenge is to work within the plunge feedrate the machine can mechanically cope with as the mechanical forces pushing a drill into the work hard enough to get the feed per rev are surprisingly high. I’d suggest staying at your min RPM until you’re comfortable with that, the lower the RPM the lower the feedrate you need to get a proper chip size. If you stay at 10kRPM then that’s half the feedrate of 20kRPM for the same feed per rev.
If the router starts to stall then you may need to speed up.
Dependent upon how well the chips are clearing you may also wish to consider a peck drilling with partial retract toolpath to drill, say 2mm in, retract to clear chips, remaining distance.
