Hi everybody,
we’re getting a lot of use out of our CNC router but we’re struggling with tool longevity. we’ve been using SpeTool 1-flute carbide end mills, using MQL and quite a bit of air, cutting something like 2 thou per tooth, 1000 fpm, and they survive about 30 minutes in 6061.
I would expect a quality carbide tool to last 100 hours, so something is wrong here.
folks who use their routers a lot, what tooling do you use? how long does it last?
We cut aluminum on a haas not a router, but we do use mist coolant and 1/4" bits as our primary endmills so it our experience should be helpful. First of all, are your bits getting and aluminum stuck to them? if you’re getting aluminum smeared on the bits thats a bad sign and might need a change to your tool coating or possibly your coolant setup. Next I wouldn’t recommend O-flutes for 1/4" bits cutting aluminum, O-flutes are for clearing chips which shouldn’t be an issue with such large bits and aluminum. We use 3-flutes with a titanium nitride coating. Do not use any coatings that contain aluminum. If changing bits doesn’t help or isn’t possible, reduce your material removal rate. It may also be helpful to check the runout on your spindle and bits, even a small amount of runout can kill bits. Then there is the question of the rigidity of the machine, if you’re machine isn’t very rigid (as is likely with a router) you’ll need to run slower to avoid chatter and premature tool wear.
I’ve had tools last all season. We cut mainly 5052. 1/8" endmills from thrifty bot
.08"-.125" Sheets, 30ipm, 24k RPM
We use a good amount of WD40 as cutting fluid
Is this accurate? The fastest we run anything is 400ipm and that with a 1/2" 2 flute in wood. What’s your depth of cut?
I highly recommend the DLC end mills from thrifty bot (4 or 6mm QTY 2 - 4mm Carbide Single Flute Endmill).
We run 24k rpm spindle, 60ipm federate, 0.5mm ramp DOC in 6061 with no problems. Just make sure that the tool is lightly misted with coolant to keep wear to a minimum and prevent chip buildup. We aim for about 0.001" of chip load.
We also use these endmills for polycarbonate with the following settings, 24k rpm, 90ipm, 2mm doc ramp. We aim for around 0.002" of chip load.
These settings were run on a typical omio so it’s likely your machine is capable of similar
Our tools are able to last a couple weeks with these feeds and speeds. I hope this helps!
*Side tip: for small aluminum holes, less than 4mm diameter, I highly recommend switching bits to a dedicated stub-drill with 0.02" pecking-full-retract drilling operations. You’re life will be so much better.
I’m very happy with our 3-flutes, we buy through a contact at a tool and die shop so i don’t know the brand, but I’m assuming you’re response aimed at the OP not me.
Yeah I clicked the wrong reply 
.
We use Carbide 1/4in single flutes from Amana Tool. We’ve been cutting at about 18-20k rpm and 50ipm in 6061 with a .25in DOC, and 12k rpm at 100ipm in Polycarbonate with a .125in DOC.
In aluminum we’ve used WD-40 as “coolant/lubricant” but we are about to switch to 99% IPA.
We’ve only lost 2 endmills due to overheating but other than that they have lasted almost a year.
what is the failure mode? is it getting gunked up with aluminum? or ? we use the thrifty bot 4mm as well and it lasts months in wood, polycarb and 6061
the failure mode is just that the tip gets dull. it stays clean until it’s really dull. in “dull” mode it does what dull cutters do: eject very hot chips that tend to stick to themselves, filling deep slots. make burrs.
it sounds like our feeds and speeds aren’t that far off what other folks are using.
surface feet per minute, i.e. cutting edge in the work. so, 30 ipm or so.
because you are running 1/4" bit, you may actually be running too slow… we run 40ipm on a 4mm bit, I think with a 0.03 DOC, 12000rpm (lowest setting on dewalt 611 router)
We have a moderately stiff router, running 24k rpm | 1000mm/min|1.35mm DOC in 6061 using These 6mm single flutes. We have run up to 2mm DOC with machine rigidity bieng the limiting factor and we plunge when we do tabs.
With these feeds we have lasted multiple seasons on one endmill- they have survived various accidental rapid plunges, loose islands and the z axis falling off with the spindle at 24k rpm💀
Would recommend!
That makes much more sense, so roughly 15000rpm 30ipm, I don’t know what’s optimal for a O-flute but that seems like it shouldn’t be the problem.
We use the ttb 4mm bits for everything. At 100 ipm 1/16 doc in 6061 they last a good while. I can’t remember the last time they’ve worn out, they usually break from a student running them into the bed or the tube jig
With much respect, I recall learning 35+ years ago that TiN coatings was not ideal or even intended for Aluminum because the cutting edge was not “sharp” enough. …yeah, relative phrase.
Over time, I learned that the TiN coating could also smear the Al (due to the “dull” edge) and thus buildup Al on the cutting tool (endmill, insert, drill bit, etc). (Highly) polished cutters or other more modern coatings are much better for Al.
-It’s understood that TiN coated cutters are cheap compared to other coatings. …It’s been around a long time. Heck, I’ve seen all kinds of TiN coated tools (screwdrivers!!) and it’s used for marketing.
Yes, we have many TiN coated cutters and use them on Al all the time. …We use what we have, but I discourage its use in high speed spindles and/or (even low quantity) production.
…I love 3 flute endmills in high speed spindles!!
Fair enough, I guess its mostly just important not to use aluminum based coatings.
For cutting Al, agree 100%!
With our router I’d run the spindle at full chooch (20k rpm) with a 1/4” or 1/8” (for smaller geometry) single flute uncoated endmill. Uncoated generally works fine for aluminum, at least for 6061. 120IPM and ~0.03” radial engagement for 1/4” endmill and ~0.015” for 1/8”. This was for 1/8” DOC on bellypans.
The most important thing is to ensure proper chip evacuation. I kept a compressed air line blasting straight at the tool the entirety of some 6+ hour bellypan jobs. You don’t need coolant, really, just get the chips out. If you start recutting chips, that’s where the problems start.
Love our new single flutes. Parts have come out cleaner than I’ve ever seen for us. We recently got a new motor for our spindle on our flat router, and we’ve also been able to run it up to some very fast speeds, up to 90 IPM on aluminum with 0.02” depth, and even 150 on polycarbonate. Haven’t broken a bit… yet. I think some mentors and I want to run the machine until it breaks one of the bits and then go slightly down from there and have that be our standard. OP if you have any specific questions about our router feel free to ask and I’ll get back when I’m in the lab next