I have to drill 13 2.5mm diameter holes in a 3mm thick sheet of aluminium. I was thinking about just using a CNC drill bit and going slowly. Has anyone done any aluminium drilling with their Snapmaker?
John
Donāt think it has enough power to get through. What Iād probably do is use a smaller bit just enough to start and create a ādimpleā and then finish off with a hand drill or press.
That way you get the SM to place them perfectly.
-S
That vid was very enlightening. 300mm p/m and .20mm steps is pretty aggressive for this machine. When I resurfaced the bedplate, I only ran it at 100mm p/m with a stepdown of .05mm. Drilling should be different I would think. Hopefully someone has done some drilling. I just ordered a pack of bits. Iāll let you guys know how it goes.
Lots of pecs should be fine.
That vid the guy is using a 4 flute 6mm endmill, not at all ideal for plunging. Iāll be trying ally with single flute tools. Iād also be pocketing the slot with a smaller cutter and finishing the side with a 0.2mm finish pass.
Looking at the Z rail the tool head mounts to, there may be a way to add a linear guide top and bottom to increase rigidity.
Iām in the middle of a 2 day print but will be putting the CNC up soon and have a crack at it 
Pugs
2 Likes
Was going to say the SM has the speed for the drill bit or 2-flute endmill, and the ER11 sufficient gripping force, that as long as you add lots of Z-hops (to use a 3D printing term) to clear chips, it shouldnāt be a problem.
Then I realized, thatās basically what @pugs said :
Drilling really is one of the most forgiving operations so long as a) the holes arenāt deep, and b) the drill bit is forced to enter straight. Iād expect many, if not most, snapmaker owners to not own a drill press, meaning theyāll want to use their A?50 for this purpose. Might be worth whipping up a sort of drill-mode GCODE macro, something where you enter the X, Y, Z, and depth and bang the hole just happens. Iāll mull it over.
ditto. Actually at this point the delay is in CADing out something that requires CNC. Though non-snapmaker life intrudes quite a bit as well 
Quick note for the OP: Check out āhigh helix drillsā for the size of hole you are drilling. For such shallow holes (3mm) they probably wonāt make a difference, but if doing multiple holes via CNC they might clear the aluminum chips better.
G81 and G83 (and some others) are already defined for drilling cycles. Marlin does not implement them, however.
There is an implementation of them: Bugfix 2.0.x FNeo31 (G81, G82 and G83) by AJMartel Ā· Pull Request #42 Ā· AJMartel/Marlin Ā· GitHub
1 Like
Hi Guys,
The drill bits wonāt be here till Tuesday. Forgot about the Christmas delay.
I set it up in F360 but Iām wondering what a good/safe plunge rate might be. I plan on running the spindle at 7000 RPM as that was the speed with the least amount of harmonic vibration when I surfaced the bed plate. When drilling aluminium by hand at work I spin the bit at about 60 rpm but have a lot of ass behind it.
60 rpm seems very slow for aluminum. Unless the drill is like 3/4" or something.
According to Norseman (Iām travelling and did not lug Machineryās with me), your speed of 7000 RPM seems reasonable:
bash# units 2.5mm in
- 0.098425197
irb> 200 / (0.098425197 * 0.2618)
=> 7761.650102793583
From the same site, looks like .025 to .05 mm per revolution is ideal. Though that gives me 388mm per minute, which ā¦ well, it seems high, but it might be right. A minute is a long time when drilling.
My Engineers Black Book is suggesting the following.
8149rpm & 61 m/pm with a feed rate of 0.02 - 0.1mm feed per/rpm
Handy calculator here, values a bit different
https://littlemachineshop.com/mobile/speeds_feeds.php
9700rpm & 76m/pm with a feed rate of 0.04 - 0.111mm feed per/rpm
Pug
Gotta love UPS; the bits arrived this morning.
Iām going to stay in the conservative side of the spectrum because I donāt want to stall the spindle. Setting it up at 8000rpm with a plunge rate of 60 mm/min. Thatās 3 seconds for each hole. Times 13 holes. I should have an answer in about an hour.
Wish me luck!
John
Wow, that was way too slow. I did 2 holes and stopped it. Next try is 300mm/min in, 1200mm/min out. 8000RPM seems like a good speed. It falls right in between your recommendations.
BRB.
John
Way too fast. Broke the bit on the first full hole. Glad I bought the 10 pack of bits.
letās try 120mm/min.
1 Like
Broke another bit. Must be these cheap carbide bits as the spindle doesnāt seem to be having an issue. It did make it further into the plate this time. Gonna go back to 60mm/min and just suck it up.
Well, even at 60mm/min at 8000RPM the bit stopped turning. Just not enough umph in the spindle. Going to drop it to 40mm/min at 12000RPM one time.
Perfect. The spindle slowed some, but the holes drilled true all the way through.
So the final feed and speed of drilling with a 2.5mm drill bit is. 40mm/min in, 1200mm/min out, 12,000RPM.
Now I have to mill the outline of the part.
John
1 Like
I think itās not the cheap carbide thatās the problem. Carbide is intolerant of deflection and the tool head is deflecting enough to break the bits.
HSS bits would likely fair better here.
1 Like
Thanks for that. I was aware that carbide bits are brittle (Iāve broken so many of them). I didnāt know the HSS were less so. I will make sure to get HHS bits in the future.
Once I slowed it down to 60/8000 it stopped the spindle though. So I think Iāll stick with this slower plunge rate.
Did you program in pec[k]s?
Without swarf evacuation aluminium will stick to the drill flutes. a bit of kerosene will also help as a cutting fluid
Pug
Nope. the machine lives in the house so thereās no cutting fluid I can use. This machine really isnāt set up for liquid cooling anyways. I just drill them in without issue at the slower plunge rate. The whole operation took less than 10 minutes. The outline of the part is about 420mm total. Itās cutting now with a 2.5mm end mill at 100mm/min with .2mm step downs. itās about halfway done.
John
1 Like