Milling bits: From OK to GOOD

Shortly after I jumped into CNC machining I ordered some single flute mills from Aliexpress (the 5mm one on the left [1]). I’m still happy with the quality of the cuts I can get with them. :slight_smile:

Some weeks ago I ordered the two roughing mills on the right (6 and 4mm with three flutes). I started with 6mm bit [2] and got nice results and less noise during the cutting process. It struggles a bit while diving straight into the wood (ramp plunge would definitely help).

Today I took the 4mm one [3]. I was impressed how easy it cut through the material and diving did not seem to be a problem. :slight_smile:


  • Material: Birch plywood 15mm
  • Mill: dia 4mm; 3 flutes
  • Spindle Speed 12000 RPM
  • Pass depth: 4mm (4 cycles to cut trough the sheet)

[1] 5 stücke Schaft 5mm Hohe Qualität Hartmetall CNC Fräser Eine Einzelne Flöte Schaftfräser Werkzeug 5*25mm|mill tools|single flutecnc router bits - AliExpress
[2 & 3] WeiTol freies verschiffen TCT drei flöten gerade bit 6mm ende mühle holz schneiden werkzeuge gerade router bits für feste holz|bits 6mm|straight router bitstraight bit - AliExpress


That’s really great information. I have not worked with bits like the one on the right so I’ll have to get one of those myself.

1 Like

Great information, great post, really helpfull.


I used to use 2 flute 1/8in bits for a while. However, for me, upon using bits with multiple flutes for long periods of time, the bits started to burn out. From my understanding, this is due to the feed rate. It is difficult to explain that concept, but basically because the Maslow is a slow moving machine the feed rate is too slow to accommodate a bit with many flutes such as those. That said, I would be cautious using those bits for long cut jobs. Signs that the bit is burning out/feed rate is too slow include: increased noise, increased vibration, and a smoky sawdust smell. In addition to that, your bit should be cutting small “chips” (almost like flakes) not sawdust.

I ran 1/4 and 1/8 inch bits (both single flutes) at 30ipm at 8 or 10K rpms and that worked well. (Ideally it would be a little bit faster but the Maslow could not do that)

–Just something that I would watch out for as I would hate to see you make the same mistakes that I had made. Note: This is really important if you plan to use your bits for long periods of time or if you plan to do long milling jobs.

1 Like

I do agree with you and that’s why I started with the one flute mill on the left.

Given values:

  • Feed rate: 600 mm/min
  • Speed: 12000 min-1

Single flute mill:
Feed per flute and revolution = Feed rate / Spindle Speed / Flutes | 12000 / 600 / 1 = 0.05mm

Roughing mill with 3 flutes:
12000 / 600 / 3 = 0.0166mm

I learnt that a feed per flute < 0.01mm is bad for the mill and when working with wood also dangerous. With the given settings I’m on the safe side. :slight_smile:

Since I upgraded my Z-axis the spindle dives into the wood and retracks instantly. So the mill is not scratching the surface a long time.

As I mentioned in the initial post I’m impressed with the qualitiy I get with these tools and settings. And to keep you updated I’ll report back when I have done a longer cut with these roughing mills. :slight_smile:

1 Like

I was a bit concerned that the 4-22 bit would be able to handle this milling job. But it did like a charm:

Material: Beech wood
Thickness: 18mm
Bit: 4mm dia, 3 straight flutes, 22mm long
Pass depth: 3.1mm
Milling time: Approx 3h for all parts (see pictures below)

Since my Maslow can not handle ramp dive, the 4mm bit did a much better job than the 6mm one (diving in without hickups).


Hi Kurt - The z-axis speed is the biggest problem I have with my Maslow, what did you do for your upgrade?

@md8n I am not sure what @kurt did for his Z axis upgrade, but when I did my Meticulous-Z, I put a 10-tooth gear on my lead screw, and a 30-tooth gear on the motor side. It zips up and down pretty good with that gear ratio. I know some have done 20/60 and some other combinations. The only thing you need to do is adjust the z-pitch in GC/WC to ensure it is moving the correct distance.

1 Like

That’s exactly what I did. :slight_smile:

Google Photos


I have been using a two flute 4mm spiral up cutting carbide bit to cut Baltic Birch using a 700mm feed-rate and a 350 mm plunge-rate with a 2.5 mm depth of cut. I’m using a Metal Maslow and have recently switched to a down cutter as the up-cutter seemed to tear the top surface. The down cutter produces a very clean edge. In my project I cut hundreds of 9-10 mm holes and I was using the up cutter to make sure chips were cleared but the down cutter it turns out is sufficiently small compared to the hole size that there is room for the chips to be cleared by the vacuum. The concern about chips vs dust in order to keep the bit cool is appropriate. When using the up-cutter the bag-less vacuum cleaner nicely separated the chips and the foam/paper filter at the outlet has stayed relatively free flowing. However the down-cutter seems to have produced more dust that was caught in the foam/paper filter eventually reducing air flow. With the naked eye I can’t tell if I’m getting chips or dust but the filter says more dust with the down-cutter for what it is worth.