Nomad and 0.396mm (1/64") endmill

(Ross) #1


I’m trying to mill fine detail on 6082 grade aluminium with a 1/64 (0.396mm) 2 flute solid carbide endmill and having problems with the bit breaking. The larger bits I use for previous passes are working without problems.

I’m using the settings Carbide Create automatically generates for the tool which are the following

Depth per pass = 0.052mm
Stepover = 0.178mm
Spindle speed = 2339
Feed rate = 279.400mm
Plunge rate = 34.925mm

I’m very new to CNCing so if anyone can offer any advice on what settings to change I would really appreciate it as the endmills are quite expensive and I’d rather not guess and keep breaking them.



(Ron McDavid) #2

Spindle speeds seems awfully low. I would think at least 9500 rpm and slow feed rate way down.

(martin redeby) #3

basic rule is the smaller the bit the higher the rpm.

with those small thing you definitely need to measure your runout and check recommended chipload for that endmill. (from what I’ve read the runout shouldn’t exceed 20% of your recommended chipload)

For a start try (not knowing anything about your endmill… flat? ball?)

doc 0.2mm
woc 0.1mm
feed 120mm/min
plunge 50mm/min

(Ross) #4

Thanks for both of your replies.

Sorry I forgot to mention it is a flat endmill.

That’s interesting about the higher RPM, I wonder why Carbide Create generates such low numbers for the smaller bits.

Martin, how do you go about measuring your runout?

Thank you for these settings, it gives me something to try.

(martin redeby) #5 this video describes it in a decent way.

(William Adams) #6

I would suggest using Carbide Create’s numbers only as a beginning point, then testing them using the technique at:

Also, check and see what numbers MeshCAM generates when in Carbide 3D’s auto machining mode for a Nomad — it seems to do better.

(Ross) #7

The suggested settings also immediately snapped the bit.

MeshCAM doesn’t seem to allow me to select a custom tool to compare the numbers but for the #122 tool the numbers are completely different.


Feedrate - 64mm/min
Plunge Rate - 8mm/min
RPM - 10000

Carbide Create

Feedrate - 246.380mm/min
Plunge Rate - 30.797mm/min
RPM - 4688

I don’t understand how the the two different programs can calculate such different numbers?


You are really at the bitter end of what you can reasonably expect, here.

Based on several sources (one of which is following the X1.5 length of cut 2 flute link), the surface speed you want is between 100 and 300 m/min (350 to 1000SFM). These guys have a circumference of 1.25mm, so 1m/min is 750RPM, and 10000RPM is only about 13m/min, or about 1/20th of the low end of the speed range. This in itself isn’t a show stopper, but it means slow feeds. Real slow.

From the ref above, the feeds want to be 0.00021" (5 micron) per tooth (0.01mm/rev, or 0.0004"/rev for the two flute tool). This gives a feed rate of 100mm (0.1m, or 4") per minute at 10000RPM, which isn’t too far from the MeshCam numbers.

The big problem is probably that at the low feed rate, and the step size of bad math* 0.02mm, you have 2 revs/full step. ***

EDIT: correction: 0.005mm, you have 0.5 revs/ step… still a bit of a jolt into a small tool

On a bit this small, there isn’t really the strength to take the kind of side loading a 1.5% of diameter step in a hard (relatively) material for long.

(I think I have all the numbers right, here. I am not sitting at the machine, so I can’t check the settings in GRBL. Please correct me if I have the step size wrong)


(It’s been a few hours, but I am out of work now, so I can follow up… There may be another follow up when I can get to my machine)

The desired feeds will vary with the tool design (intended cut), material (generally carbide for our purposes), coatings (TiN, diamond, etc), and shape.

How to deal with this, which depends a LOT on the requirements of the part:

One option is reducing the depth of cut to a minimum (0.02 to 0.04mm for the Nomad-- less than 0.002"). Not always a solution, and really slows the work, but it can reduce tool breakage at the expense of increased corner and end wear.

Another is a different tool shape. If you don’t need vertical walls, use a 60 degree flat end cutter, or even a 6 degree (pattern and mold makers use these for draft). I use a 90 degree vee with 0.010" (about 0.25mm) and with 0.1mm (about 0.004") for a number to things. The vee profile gives a lot more strength than the straight cutter. Even the 6 degree taper is surprisingly more robust.

Drill corners and refine the part geometry to allow a larger cutter for the rest.

Use different machining strategies. Small bits really don’t do well for ploughing grooves (slotting). Better CAM systems take the desired feature into consideration and have strategies for efficient tool use and load control for many things that simpler tools, like MeshCam, use basic strategies for.

If you could tell us what you are trying to cut, what software you are generating tool paths with, and where the bit is breaking, that would help determine if a different tool shape/geometry and/or different software will help. There are people here that have done work with bits that small and smaller (including me), but you are into the range where everything matters.

(Phil Gorsuch) #10

This is not entirely apples to apples, but probably some gems to be dug out of here:

(Ross) #11

Thanks for the time you’ve taken to respond to me here.

I’m trying to cut 2D designs into 6082 grade aluminium so I’m using this tiny bit to get the fine detail around small letters and shapes. I’m using Carbide Create to generate tool paths. The bit seems to break off right at the top of the cutting length.


What feature is being cut? For example, is it into a corner? Surfacing? Entering the material?

A straight side bit will often break at the top of the flutes, as the bending stress is highest there (long arm to the bottom, similarly to how it is easier to snap a full length pencil with your hands than a 50mm stub) and there is more material above that point. I would guess, based on this type of break (it is an educated guess, but still a guess), that your feed is too high for the tool engagement. I would not be surprised if it is happening at the first inside corner.

The reference @PhilG put in is good (I didn’t find it yesterday), and recommends about half the feed from the table. Note again that the feed/tooth is roughly the mechanical limit for the machine and the feed is slow enough that it will not be dead smooth. This is harder on the tool, so slowing the feed more is going to be a little less smooth, but between steps there will be several cutting edge doing some work, reducing the tendency for the tool to spring/bend.

Another ting you might try with the aluminum is a little kerosene or WD40. Coolant.lube can help a lot but easing the chip evacuation and reducing heat build up in the cutting edges.