What bits to use for cnc and what speeds and feeds to run at

I was wondering what cutters outher teams use on their cnc routers and what feeds and speeds you run them at

Out team is a fan of Amana Tool’s router bits. We have had good luck cutting lots of aluminum, wood, polycarbonate, and even stainless steel. We have their 52 bit set, so we have the option to cut quite a few materials (see link below). As for feed rates/speeds, they post a document with their recommendations on all their bits. We usually start on the slow side of their recommended ranges.


This Amana endmill is pretty cheap: https://www.routerbitworld.com/Amana-HSS1621-HSS-1FL-3-16-x1-4-x2-7-8-UPCUT-p/amana%20hss1621.htm

Amana says it can do up to 18k rpm anda .004 to .006 chipload.

So if you ran it at 10k rpm and .004 IPT, yo can move it at 40ipm. 40ipm, slotting, with a low depth of cut (maybe 1/16") is a good place to start.

I’ve run this endmill before as well. It works well at 42IPM and .07" depth of cut, but doesn’t last long. I throw them away once per sheet.

I’m a fan of Onsrud bits.

We use a 63-620 at 8k RPM to through-cut aluminum sheet at around 20-25 IPM without coolant. It does not work well if cutting only partially through the material: Punch through then cut. A 63-618 can be used at the same rate for smaller (3/16") areas, but we almost never need it.

When cutting aluminum sheet, after laying everything out we create a bunch of strategic 1/8" holes (1/8" cobalt drill bit in 1/8" collet) and run screws through them into the MDF table. This not only holds the material in place, but manages the cut-off bits that, if they move, can break the bit. We used to use tabs for this, but removing tabs in aluminum is a pain. After everything is crewed down we run the cutting path.

For Polycarb we use an Onsrud 63-768 (3/16") or 63-760 (1/8) at 16k RPM and 50 IPM, through-cutting at with aluminum.

As with any machine, start around these numbers and experiment, changing RPM and feed a bit at a time to find the best performance, then keep it there.
We use a Freud 75-102 for wood and foam. I can cut 1/2" plywood single-pass at 80 IPM without trouble.

We have been also using the Onsrud 63-620 for the last 4 build season with great success.

Feeds/Speeds for our setup
60-70 IPM
0.050 DOC


This sounds like advice for a mill, not a router.

Apart from running a little slow at 8k rpm, what do you mean?

Slotting with a 1/4’’ endmill at 8k rpm with 1/8’’ DOC sounds like it wouldn’t work at all on most routers.

That sounds like advice for a mill, not a router
Nope, router on almost its slowest speed.

Yes, I’d have thought that as well, until I tried it. The bit cuts SO much better full-through than part-way. Part way through (as in 0.050 DOC) really needs coolant, as the end of the bit gets warm. Going completely though is far easier on the bit (empirically). Note that Onsrud recommends a 1x DOC (that is, 1/4" for a 1/4" bit) at something like 90 IPM :ahh:

We have upped the speed for testing, but 8k was the sweet spot. We don’t really have the HP to double the speed (which would allow double the feed), but we have cut 1/16" sheet at 50+IPM. We use MDF as the table and cut maybe 0.050 into it.

I did measure the thickness of the chips with a micrometer and we’re getting something like 0.002 - less than recommended but it works.

As I stated: YMMV, start conservatively and up speed and feed (easy in MACH3) until you get a sweet spot, then cut there for everything. OK, you might need to waste a few square feet of metal to dial it in, but we cut several hundred feet last year with only one bit breaking.

What type of spindle do you have? Most that I am familiar with don’t have a ton of torque down in that speed range.

From what I’ve read, 8k rpm is still in the “good” range for router spindles, even if low. I’ve seen people go that low to atke light cuts in steel before. Also, cutting 1/4" thick aluminum with a 1/4" endmill at 20ipm should only be a ~0.4HP cut, so even if horsepower scales down linearly with speed and you’re using a 2.2kw spindle, it’s still a safe cut. That being said, doing that same cut with an air-cooled versus a water-cooled spindle may work better on the latter due to the better cooling.
Clearly it works for one member, but maybe some more specs of the machine (such as spindle HP) would be useful.

We run a fogbuster coolant setup when we are cutting on our router. Totally worth the money, previously we ran a cold air gun.


As for our spindle its a porter cable 3.25 HP router.

We have been using the 4mm option from WCP and absolutely love it. Started off with Onsrud (I believe the 63-620), but made the switch for cost reasons and have been very satisfied.
I don’t have our feeds and speeds off hand, but we typically run a bit “conservative” DOC,

The best cutters you can buy for FRC are from ebay. They come from a seller called rogue systems inc:
They sell cheap, uncoated, US made carbide endmills. I find their 1/8" 3 flute “AlumaCut” endmills to work very well at a reasonable price. Tey also sell a 90 degree spot drill/chamfer end mill that is extremely useful. I run slotting at 15 IPM and 0.02" - 0.03" DOC. For pocketing I run at 40 IPM, 0.06" DOC and .025" WOC. A cheap coolant mister is good to use also, you can go faster if you use coolant. I have this one:

I run a 50% rubbing alcohol and 50% water solution through the mister. I have a very fine mist coming out. I also have a dust boot that is designed to have a coolant mist spraying onto the cutter at the same time as the vacuum is running. My worry with the alcohol is that the vacuum will suck up alcohol vapor and ignite it but that has not been an issue so far. You really do not need coated end mills for most applications but find ZrN coated tools for aluminium and TiN for steel if you want coated end mills. TiN will work for aluminum but ZrN will work better. Never use ZrN in steel. Generally, for CNC routers, coated end mills only work better because most of them are a higher quality tool that cuts better. The low MRR that routers run at makes coatings essentially useless.

What RPM are those IPM numbers at? I run much more aggressive feeds on the $1.50 endmills I get from China, but they may not last as long as the ones you use. Typically I run at 42IPM and a .07" DOC slot at 18k rpm on the single-flute Huhao 4mm endmills, and a slightly lower DOC at 30IPM on generic 1/8" endmills.

You need to move to single flutes. That MRR is not great.

That it true, it is not great but I am running a shapeoko 3, a much lighter duty machine than most and these speed are specifically for cutting into 1/4" thick stock. With such deep slots and small pockets, chips tend to gather in the bottom and jam up the cutter if I go much faster. Other issue when going faster include excessive machine deflection as the shapoko 3 was not really design for metal (but it can do it). I am still constantly experimenting to improve my feeds and speed. I do not believe that the 3 flute tools are the issue but I will look into 1 flute tools.

I like to run at about 17,000 - 18,000 RPM for 1/8" cutters. The biggest issues I face come from my machine (shapoko 3) that isn’t rigid and a wooden bed that causes me to not be able to use very much coolant (if at all). As for the life time of my tools, it is at least 6 months (the longest I have lasted without snapping a cutter with aggressive feeds) of cutting at least a part of week, generally more. What machine do you run those feeds on and what do you have for coolant/chip clearing?

Ah, the Shapeoko explains it. I run those feeds on a Laguna 4x4 with no coolant, although there is a vacuum and dust shoe to help suck away chips. On routers, mist or other compressed air cooling is the best way to handle it (or somebody spraying copious amounts of WD-40 on the work).
Still, even on a Shapeoko, single-flute endmills will do better than 3-flute endmills because you can maintain more consistent and larger chipload.