I’m having a lot of trouble breaking bits, mostly 0.254 mm (0.010") and 0.381 mm (0.015"). These are square end mills, mostly 3 flute Kyocera. I’m cutting exotic hardwoods such as Indian Rosewood, Ebony, Wenge. (The Indian is not nearly as hard as Brazilian, FWIW.) Currently, I’m mostly trying to cut simple slots, up to 1 mm deep, in which to embed powdered stone inlay.
I think I’'m being conservative with parameters; my last trial with a 0.254 mm was:
DoC 0.050 mm
feed 80 mm/min
plunge 15 mm/min
RPM 500
The CC suggested RPM was about half that which seems really low. I’ve read a bit, eonough to understand values can be too low as well as too high. I don’t mind going slow, I’ve got time but some sources state this can result in insufficient chip clearing, overheating and other maladies.
I’m not sure in what part of the process breakage is happening. I may try to video the process, it’s too much to sit and watch carefully enugh for long enough.
(I’ve also had issued cutting mother of pearl but noticed, early on, most of the breakkage there was on the plunge. My thought there was to use high speeds, low plunge rates and a very small DoC. I got somewhat better results but still had some issues.)
Maybe not applicable, but since it sounds like you’re inlaying a liquid slurry, have you considered vcarving the pockets? A v bit would probably be beefier and still provide the correct line thickness if you used something like a 60 degree or 45? Just a thought.
@WillAdams No, the 500 was double the RPM that CC suggested! I know, as you have mentioned in other posts, CC is “conservative” so I generally up the speeds by a factor of 2 or so. I will try upping the speed substantially more. I have glanced at the PreciseBits page in the past, will pay it more attention.
@DanoInTx Indeed, I am experimenting with vee bits as well. One prospective issue there is that you want a certain depth to “anchor” the inlay. At the vee goes deeper, the line gets wider and, since most vee bits have a “tip-off” of 0.10 mm, this means a pretty shallow line. I am about to experiment with a “no tip-off” bit from 2L.
According to the PreciseBits tutorial, the second thing one should do, after measuring runout, is to “set the acceleration on each axis” using the controller interface. Is this possible with the Nomad and CM?
I’ve worked this a few times in g-wizard, and It’s telling me 10k rpm on nomad, with your 80mm feed rate and .050mm DOC - AND that deflection is really high (will break endmills)
With a 30mm feedrate, same other parameters, deflection looks ok.
I’m just wondering if you put a little air or alcohol mist on the mill if that would help with cooling. Alcohol might also lubricate the tooling. I’ve never tried it but it’s worth a shot I think.
I frequently use 0.0236", 0.0200", 0.0150" and 0.0120" end mills in padauk, wenge, katalox, pau ferro, chechen, maple and bamboo. I typically run the 0.0150" end mills at 22,000 RPM and 30 IPM with a DOC of only 0.040". The 0.0120" end mills I run at 24,000 RPM and 25 IPM with a DOC of 0.030". I run really conservatively though.
@MadHatter Thanks, nice mermaid! You are evidently working on something other than a Nomad whose max speed is 10k RPM. Are you ramping into the cuts or plunging?
I am was using a SO3 with a DeWalt DWP 611 router, SuperPID and the PreciseBits EP collets, with solid carbide end mills from drillman1. I do plunge cuts, because I use makercam.com for 95% of my gcode, and it only does plunge cuts.
I am in the sloooooow process of making room in my shed for my SO3 XXL, getting the base for the XXL built and installed, finishing up my dust collector setup, getting my 1.5KW spindle and speed controller setup.
The spindle has a top speed of 24,000 RPM so that is nice, and as of now, I only need the 1/8, 3/16 and 1/4 collets for the spindle since all of my end mills are only those diameters (so far, at least).
My SO3 has been brought into the house and re-purposed to diamond drag engraving next to my 3D printer since that is a quiet operation.
Damn! If you’re using a router then run-out imay not be as implicated in breakage as I feared, good news. I wonder if high speeds might somewhat negate the effects of run-out to some extent, allowing the bit to present itself as just a tad larger (just a hypothesis). I too have been careful about my collet choices. It appears drillman1 deals in, at least, Kyocera so I seem good there as compared to you. I will check out more of his wares.
Thanks for sharing specifics. I am quite encouraged, will step up the RPMs and do some more testing.
[Edit: Thanks for the drillman1 tip. Some of his prices are less than half Kyocera’s. Testing is now affordable! I thought my searching was pretty complete but I never found his excellent, searchable ebay store. Forums are good!]
Ouch! I can’t recommend my settings will work for acrylic. I’ve yet to work acrylic on my Nomad but I’ve done plenty work with it with a router and bandsaw. The issue there is melting so I’d guess the high speeds that worked for me in wood may not be appropriate.
I’d guess you should not use too slow a feed rate, that causes melting with router and bandsaw. I’d also thing lower number of flutes, say two versus three or four, would help. Try to discern when your bit is breaking, whether on the plunge or while feeding. I’m speculating here but if your cuts are relatively deep it might help to lubricate the chase with a bit of light weight oil to kee the bit from burning the already cut layers. By “burning” I also refer to the built up accumulation of plastic that might be creating a drag on the bit.
Since you asked, here’s what worked for me in wood (0.20 mm square end mill, 4 flute):
DOC 0.050 mm
feed 30 mm/min
plunge 10 mm/min
RPM 10000
I used a 3.45mm drill bit to rough out the interior of the pockets, leaving the corners to the single flute end mill. Even with this initial drill roughing, I broke about 7-8 end mills using the 3D pocket toolpath option in Autodesk Fusion 360. My first breakthrough came when I switched to an Adaptive toolpath. That helped the end mills survive about 20-30 holes, but I needed to mill around 600… My second breakthrough came when I changed the ‘Optimal Load’ parameter from 0.4mm (40% tool diameter) to 0.2mm (20% of diameter). That effectively doubled the total milling time to around 6 hours, but considering how many tools I’d broken up to that point, I was happy to compromise. It’s possible 0.3mm would have worked, but I didn’t have time to keep fiddling with it.
One of the reasons my parameters are different than yours, besides the wood, is that there is a world of difference between a 1.0 mm bit and a 0.2 mm bit. Even with 0.794 mm (1/32") bits I am far more cavalier than the specs I posted here.
