1/64 endmill in brass

Hello, I’m trying to machine some brass stamps. I have been having no problem until I needed a 1/64 square end mill. I’m breaking them like they are free. I even bought g-wizard to see if that would help. On that attempt this morning it broke about five seconds in. So I cut the values in half to see what would happen with my last one. Made it about a minute and done. Is this possible? In g-wizard it doesn’t like the 10000 rpm limit but says it should work. Thanks, Duane


What are your feeds and speeds?

To add to @JosephSeth’s question…

Which brass alloy? 353 is easiest, 260 work hardens and is quite difficult.

Endmill geometry?

What toolpath settings in which CAD/CAM tool?

1 Like

@WillAdams @JosephSeth @Duane How many flutes? I ask because at that level of micro tooling, there is little room for chip evacuation. Also, halving the diameter of an endmill reduces stiffness by a factor of roughly 7. You use GWizard. CNCCookbook has a nice article on their blog this week about optimizing tool paths to reduce stress on tooling in corners etc. I find his blog most useful. Jerry



As someone who’s been doing some micro-engraving, a potato-quality proof-pic and then a few thoughts:

First, specific tips regarding not breaking tiny tools:

You need to cut with the correct chip-load on the cutter for the sake of longevity, rather than maximum material removal rates, within the limitations of the Nomad/Shapeoko, so you have to set your feeds & speeds based on the diameter of the tool, and the number of flutes.

The guidelines for this are:

Start with feed-per-tooth values of tool diameter x 0.005, so on a 1/64th tool that’s ~0.00008in, rounding up. That means at 10krpm your feedrate is: 0.00008 x 10,000 (spindle speed) x 2 (flute count) = 1.6 IPM
Yes, I know that seems silly slow. So only use the teeny weeny tool where you absolutely need to.

If you’re feeling ballsy, you could increase your multiplier to 0.8% instead of 0.5% of tool diameter, and in ideal milling conditions I’ve seen recommendations going as high as 2% for aluminum, so test at your own discretion.

Depth of cut on tiny tools should be no more than 100% of the diameter of the tool when adaptive cutting, and 50% when slotting at the given above calculated feed-rate.

If you want to cut things faster, you’re going to need a higher-speed spindle. If wishes were spindles, I’d have an NSK 3060 series with quick-change tool-holders that can run at 60krpm…

Now general suggestions:

  1. Use Fusion360 & the integrated cam and use adaptive clearing path strategies as much as possible. You really want to be careful not to put too much lateral force on the tool (because snap). If you do this and have lateral engagement of 30-40% of tool diameter you’ll be prolonging tool-life. Pay attention to chip-thinning though—if you use a lesser step-over, you can increase your feed per tooth to keep chip size consistent. Harvey Tool has a good blog post about chip thinning worth a read.

  2. Machine in C360 brass if your application allows it—it’s a leaded alloy, which sometimes does and sometimes doesn’t matter. It’s often called “free machining” brass, because it cuts well.

  3. A little coolant helps a lot to preserve tool life. For brass you can use soy-based oils.

  4. I’d recommend using 3-flute cutters as you’re spindle-speed limited and at that size of cutter and 2 flutes will take 50% longer, meaning you’ve got to run the machine at that size that much longer. I wouldn’t recommend higher flute-counts due to evacuation and chip-thinning issues in tight pockets.

  5. I assume you’re only using the 1/64th tool for finishing passes, and doing the bulk of the work with other tools, right? this piece I was working on went through 4 tools in the end on my Shapeoko3: 1/8th 2-flute, 1/16th 3-flute, 1/32 2-flute, and then a 90° v-engrave taking a few passes to get down to proper engraving depth.

Good luck!


The last one I tried I slowed it WAY down to see what would happen. Feed 1 ipm plunge .5 ipm. Step over .0010 and depth of cut .0010. It lasted about thirty seconds. I have some pulsating noise coming from the spindle. It sounds like a bearing. I wonder if that could have something to do with it.

This is a really great set of recommendations, thanks for putting these all together in one spot!

As a general rule, plunge should be 25% of lateral feed, therefore your plunge is a bit aggressive by my observation. Spindle noise also is no bueno, definitely get that checked out.

Also, I’d recommend using Fusion360 if you can, and use a helical plunge rather than a straight plunge—easier on the tool, and helps evacuate chips to prevent jams & snaps.

It’s also possible to be taking too small of a step—then you’re burnishing(rubbing) and you’re heating your tool, and heat is the primary contributor to tool failure, outside of an outright break (due to chatter/deflection)

Your step-over & DOC are conservative for adaptive clearing, but you’d be taking a VERY thin/light chip, so you were likely over-babying the tool.

If the tool snapped off on an inside corner, that’d be because of a sudden change in tool load, which is yet again why you want to use adaptive clearing path strategies. If it snapped along a straight move, I’m guessing the spindle is likely to blame. Good luck!


The smallest diameter square end mill I use is 1/32
My settings for that are: .250mm DPP, .200 step, 300mm feed, 100mm plunge, and .040 OAD.

The 10k rpm limit makes running smaller end mills unacceptable.

For smaller details, I use a 20 degree tapered end mill, with a .004 tip. MeshCam thrives when I’m running these small details.

Tool settings: .127mm DPP, .020mm Step, 200mm feed, 100mm plunge, .050 OAD.

I should note that I only use carbide for brass. HSS heats up too quickly, and wears out too fast. I’m up to 5 or 6 dies with my tiny tapered endmills before they get dull and the tip breaks off.

I run all my tools at 10,000 rpm. That is technically too slow for my smallest tools, but I make do by adjusting the feed and stepover.