Hi guys, I have an exact replica of an Avid CNC 4896. I’ve been practicing as a beginner for a month now. I have a NEMA 34 motor and a 3kW spindle. My question, if you can help me, is that I’ve been using Chinese Spetool router bits on ash wood, and today while cutting a contour, the bit was making a very high-pitched noise and I think it’s no longer cutting. I should also mention that it’s an 8mm bit, which is the one I use most often, and I’ve done some epoxy resin recesses in a few small areas. I imagine these Chinese router bits don’t last very long. I’m thinking of buying a CMT bit here in Europe, Spain. I look forward to your advice; I’m a complete beginner. Also, what feed rates do you recommend for ash and a higher-quality router bit with an Avid 4896? Thank you very much, greetings from Spain, and please excuse my English.
One thing that I found out more recently in the last two three months was to use roughing bits they dig out wood faster but have less of a finish look then bring in your finishing bit to do the final passes which reduces the wear and tear on your finishing bits
Please keep in mind that in the CNC world, router bits are not investments - they’re consumables. Even top brand bits will need to be replaced regularly. Keep spares on hand and replace them when they stop cutting nicely.
Like @JeffsDesign said, use roughing bits. That could be as simple has having two 8mm bits, one new and one old, and use the older one for roughing and the new one just to clean up the edges. When the new one gets too dull for finish work, it becomes the new “old” one and you get a new “new” one.
Does it make sense to use the old cutters for roughing and the new ones for finishing, rotating them, and what about the feed rate? For milling, I’m using 2000 m/s and 18000 rpm. I know I’m being conservative, but I don’t know if it’s better to increase it so the cutters work better and suffer less wear. Thanks.
If you are too “conservative” (high RPM but low feed rate) you are actually creating a low chip load which generates heat and that dulls the cutter. The best way to be “conservative” is to take a shallow depth of cut once you find the correct chip load.
One thing I’ve started doing, in addition to asking advice just like you, is to enter all my machine specs in an AI engine (chat gpt, grok, etc…) and get some recommendations that way. Then I compare that with the feedback from my own research to establish a starting point. Wood is very forgiving compared to aluminum or steel…
2000 m/s As in 2000 meters/second? I think something was lost in translation.
Two flute cutters?
Mm/min jaja si la tradición falló,fresa de dos filos de 8 mm CMT tools
I think your feed rate us too slow for the 18K rpm spindle speed. I would start with a feed per tooth of .127mm (.005”) which would put you at a feed rate of 4572mm/min. (180 ipm) I find that if the cutter us screaming then the feed rate is to slow or RPM is to high and the screaming is the cutter rubbing and not cutting. I also look at the chips. If they are dust then I take a bigger feed/tooth, which means slow the spindle or increase the feed rate. Learn to calculate spindle RPM based on the cutting speed (Surface feet /minute or Meters /minute) of the material being cut and the cutter material (HSS vs Carbide) and the formula for feed rate .
Feed (mm/min)=RPM×Flutes×Chipload (mm/tooth)
Example:
RPM = 12,000
2 flutes
- Chipload = 0.13 mm/tooth
Feed=12,000×2×0.13=3,120 mm/min
Gracias Loren, si tengo que empezar a entender mejor los calculos de velocidades según esta formula.
The WORST thing you can do with a router bit or any type of cutter, is not cut enough. You end up rubbing the wood instead of slicing it, and abrading away (or burning up) both the wood and the bit. You REALLY need to move fast enough, or cut slower, so that each flute takes of a minimum amount of wood - and it’s usually in the 0.001” - 0.010” ( 0.025 - 0.25 mm) range. At 18000 RPM with a 2-flute cutter, that means a minimum of (does math) 36 in/min (900 mm/min) but closer to 7x that for most bits (252 in/min, 6300 mm/min). I run my roughing passes at around 150 in/min, and finish around 40-60.
Example: Freud 1/4” bits in hardwood, they recommend 0.008-0.011” cut per flute (“chip load”). That’s 288-393 in/min (7300-10000 mm/min). See https://www.freudtools.com/public/assets/freud/downloadables/freudtools-router-bit-feed-and-speed-for-cnc-20170822.pdf
So based on that, I’d say you’re being overly conservative but not terribly so, and could afford to go much faster if you wanted. If you think your machine isn’t powerful enough to cut that fast, use shallower passes.
I just started using a Spetool bit and so far so good. I got QTY:5 1/4” compression bits for less than the price I usually pay for one Amana or Whiteside bit. I’m cutting 9mm baltic birch at 18000 RPM and 200 IPM with .360” DOC using “Conventional” cutting profiles. Still on the first bit and have run through well over 100 sheets of machining. The bit is a little discolored but still sharp and cuts as well as on the first sheet. So so far so good. My experience with Amana coated bits is that they usually break on me after a couple hundred runs and the Whitesides (non coated) get dull around about the same. I guess results on this 1 SpeTool bit isn’t a statistically reliable data set and I’ll be interested to see how the remaining 4 bits do, and in how long it takes for me to need to start using the next one. At any rate, the 5 bits just have to last for me longer than about 200 sheets to make them a good buy. 
Great, so far the Spetools I have have been pretty good, at least the smaller ones, but this 8mm one in particular, it’s also true that I use it quite a lot and I had to do a hollowing out of ash wood + epoxy resin, it lasted me 100% for two and a half months, it’s not dead yet but it doesn’t cut half as well as it used to.