Spindle stalling during drilling operation in brass

I’m having trouble drilling a 3 mm diameter by 1mm deep hole in brass. My nomad keeps stalling halfway through. I’m using a high speed steel 2 flute drill bit. I’ve used the speeds and feeds recommend by fusion 360 (rpm 1460, surface speed 45 feet per second, plunger 8 1.7 in per minute, .001 feed per revolution.)

I bumped the rpm up 5000 based on this calculater (Goodcalculators.com/speeds-feeds-calculator) but get the same results. I’m probably doing something very basic and very stupid but I’m not entirely sure where it is messing up.

3mm is a large drill for the nomad. In many types of wood and plastic, the Nomad will do it, but I doubt you will make it in brass.

Many brasses don’t drill well with a standard bit, and require the cutting edges be reground to avoid grabbing, or the use of a slow helix bit. To do this, you grind the cutting edge to zero rake. See the video from Clickspring for an example: https://www.youtube.com/watch?v=pAngKHIZgyA


That calculator assumes excess power is available, which is not often the case with the nomad, it’s only ~50 watts. Try cutting the plunge by 50%, and “brass” the drill (see the clickspring video above). It’ll only be efficient on brass after that, but it’ll work much better in soft material like brass.

To add to this: for a 1mm deep 3mm hole in a more difficult material, I would bore it with a 1.5mm or 2mm endmill. Fast, and no power issues. For, say, 2.5mm and above (no hard line here), I generally mill rather than drill on the Nomad, depth permitting, unless the material is very amenable.

If the depth is greater than I can mill, I will pilot with a small drill bit, mill as deep as I can, and use that to guide drilling on a press after the CNC work is done.


Out of curiosity, how do you bore with an end mill? Those only cut from the side?

Center cutting endmills aside (which really arn’t meant for drilling, in general), there are a number of ways, but they all essentially involve a helical tool path.

Some tools have this as a basic operation (Fusion360, Autodesk HSM or whatever it is called now, etc), and in other tools, you can fake it with other operations, such as predrill a small hole, maybe 1mm, then model a round pocket and machine that. Some tools will do fine just treating the hole as a pocket.

1 Like

That solved my problem and it’s even faster than the workflow with a drill, more so without a tool change.


Brass is awful to work in. I can get a good hole now but when I get to the 2d contour operation I keep breaking end mills. It will ramp in just fine untill .5mm then snap even with 30 reduced feed rate.

Whether brass is difficult to cut or no depends on the specific alloy — 360 free machining brass is considered the standard for being easy to machine — please post the specifics of your difficulty and we’ll do our best to help.

1 Like

I unfortunately can’t seem to find any 360 brass sheet in 1 mm thickness. I’m using 260 with a 1.5mm 4f carbide end mill running 5000 rpm taking a 0.001" cut.

We have a brief note on that at: https://wiki.shapeoko.com/index.php/Materials#260

Online metals has 353 engraver’s brass which is almost as easy to machine as 360 (and lower lead content):


Try it?

Have you seen @wmoy’s two videos on brass? #MaterialMonday on YouTube

Well I don’t have any of that on hand and need to finish this part before it could get here. I’ll definitely order it next time but it doesn’t really help me now. I actually started with those numbers from wmoy but that broke an end mill too. :frowning: I’m clearly doing something wrong. I get that special brass is easier to machine but I feel like I should be able to also machine regular brass they doing something with the numbers.

I do pretty okay on aluminum brass isn’t that much harder.

I’m pretty sure it’s the specific alloy 260 is noted as being difficult to machine, gummy — have you tried coolant?

Wd40 and air that’s all I have.

Better than nothing. Could also try alcohol - I’ve found that works surprisingly well.

Gotta ask - your 2D contour is setup such that you are slotting the brass all the way through? If you are getting good results on the helical boring with an end mill a switch to adaptive to avoid slotting might help (if you have the space for an adaptive toolpath)

1 Like

Not a bad idea, not sure how to do it though. I’m cutting out parts from a sheet metal, most of the features are within 3 mm of each other. Never even occurred to me to a try it adaptive. I suppose I would have to set up touch no touch rules or constraint in some way?

1 Like

Not exactly sure what your toolpathing requirements are, but I have used adaptive with additional offset to create adaptive loops where normally one would just see a straight contour. Not sure if that helps!


This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.