1/8th shank speeds and feeds

Was wondering what kind of speeds and feeds you guys are using for the smaller 1/8th shank bits. I have a small set of metric bits and the recommended speeds seem very slow 16ipm. These bits are small so I assume they break easy but that seems like it would take forever at that speed.

I found some settings running this around 40ipm but broke after the second pass on my test cuts in pine. These were cheap bits so I dont mind that they break to learn but getting them to work without breaking at a decent speed would be useful. Anyone else using the 1/8th collet and small bits? I can just blow through the rest of these to find out but thought I would ask first. This is the set I am using.

@JDog - you should not be breaking bits at 40ipm, unless your DOC is much larger than 50% the diameter (like >100%) . I’ve run 1/8" bits at 80ipm no problems at DOC=0.0625.


1 Like

Hello Tom, I’m curious if you are using the Makita router and if so what brand and where did you find the 1/8" collet for it. Everywhere I search there is no POSSITIVE listing for the Makita? Many adapter collets but not an actual 1/8" collet.

Search for “Elaire” on the forums. It’s where I got mine.


Thanks I think doc is exactly what I had wrong. It was set to 100% bit diameter. I am still trying to understand how doc factors into the feeds and speeds calculations.

1 Like

Hi Bill (@planeoldme) - I have the Elaire collet as indicated by Nick.

@JDog - I wouldn’t expect the bit to break at 100% DOC at 40ipm, but I guess it depends on the engagement strategy and acceleration/jerk settings. Certainly less than 100% would likely produce more positive results.


Those settings were for the 1/8 shank bits the actual bit size I broke was 1.0mm. or .0394in diameter. I think anything under 2.4mm or .0945in should use 50%doc. I had no problem running the full 1/8 bit 100%doc.

I’ve run 1/8 bit through 1/2 plywood full 100% DOC at 40ipm without breaking the bit. RPMs were at 18k though.

Hi Tom,

Is this the general rule for DOC? To make sure it’s 50% or less than the diameter of your bit?

Hi Nathan - yes, generally 50% is considered a good and reliable DOC fro 1/8" and above. I usually do 25-50% for 1/16 and 1/32 but slow down the feed rate. You can go up to 100% depending on speed and material.

Interestingly enough, the formula for feed rate does not consider DOC at all, so it can be a little misleading if you optimize your feeds/speeds/chip load but don’t adjust for the stresses related to DOC.



If you use Amana bits, they have explicit specifications that are a function of depth-of-cut.
I’m sure other manufacturers provide similar data.
Otherwise guessing can get expensive!

For example,
Solid-Carbide-Spektra-Compression-Spirals-v26 (amanatool.com)

Here feed rate is a function of the bits diameter (D) in proportion of depth of cut.
So if your bit is 3mm and you’re cutting more than 3mm, you reduce feed rate proportionally.

1 Like

Hi Alex,

I’m not sure if I understand that picture you attached, can you please explain it to me a bit more?


Is this saying if you’re cutting 1 times the diameter of your bit then use the recommended table, and if you’re cutting 2x your diameter then reduce feed rate by 25% etc…?

That is correct.
The feed specifications are, in the case of Amana bits, based on depth of cut no deeper than the diameter of the bit.

As you go deeper, you need to adjust the feed rate.
This makes sense, as the bit has more work to do and so should be pushed less.


Most bits have more cutting area than they are wide. For most manufactures the chiploads are optimal at 100% bit diameter, but to use the whole cutting area or the rest of the bit you need to reduce chip loads.

  • 20-25% - for depth = 2x tool diameter
  • 40-50% - for depth = 3x tool diameter

The more surface area the bit has to cut the less effective it is at removing the chips out of the way and so the heat removed per revolution is reduced.

The smaller the bit the smaller the chips so it’s harder for heat to transfer from the bit to the chip. The larger the bit the more heat transfer it can handle and so using more of the bit is more optimal.
This is why it is recommend to reduce doc for small diameter bits due to effectiveness of chip heat transfer. Heat is what makes the bit brittle and dull and then break.


There is no one setting that will work for all of your bits.
Running things too conservatively or too little depth and you get into the chips being too small to carry heat and so the bit starts to heat up.
Each bit has its own different cutting characteristics and using the appropriate setting for each bit will give the best results and longest bit life.

In my tests the only bits I have reduced doc on where 1/8 shank and smaller bits.
I run my 1/8 1/4shank at 100%doc but all of my smaller tip 1/4 shank bits I run at 75%- 50%.
I do not run anything under 50% though as I have found it burns the edges of the bit and gets dull below this point.

Thank you for the explanation J, Alex and Tom, once my new 1/16 bits come I will reduce my doc and slow my feed rate down a bit then try again. This community is awesome, so much to learn and everyone is willing to share their knowledge!

Hi, do you happen to have a link where you can get the Collett for the Makita router 1/8 to 1/4 adapter. Thank you


1 Like