Small holes are too small

I’m trying to mill M3 and M4 tapping holes and having difficulties. I’m guessing that either I’m doing something wrong or it’s “the way things are” and I’d like to understand why, either way… To do this, I’m using the 2D Boring operation of fusion using about a 2mm endmill (either 2mm cheapo amazon mill or a 2L 5/64" endmill).

Both M3 and M4 tapping holes (these are 3.3mm) are too small. On my last run, my 3.3mm hole was too small to accept a M3 screw and when I tried to tap the hole, I was only able to get a short distance before it became too difficult to keep advancing the tap.

Using the 2D boring operation, I’m doing various combination using both the crappy 2mm endmill and the good 5/64" (1.98mm):

  • RPM: 23K or 10K
  • Pitch: 0.1mm or 0.05mm
  • Finishing passes: on/off with a 0.1mm stepover
  • Repeat passes: on/off

and my hole ends up consistently small. I tried cutting a “slot” (adaptive clearing of a bigger slot with edge cleanup using the 5/64" bit) and adjusted the bit diameter based on my caliper measurement) giving me a final diameter of 1.83mm for the 5/64" bit. That still didn’t help solve the problem.

What else can I do to make the holes the correct size, or should I just undersize the holes and use a drill press to finish them?

You may need to run a calibration to make sure if you cut 5MM that the cut is 5MM. There are instructions on the site for running a calibration. Sometimes you have to tweek the steps on the stepper motor to ensure you get the size you want. Usually you make a larger circle and square to check that the prescribed distance in the CAM is actually cut to the prescribed distance.

Cutting a square after adjusting the bit size be spot on. Larger holes are fine (5.5mm hole for M5 through holes are reasonably sized when cut with a 1/8" endmill) and calibration of x/y was good l.

Have you tried leaving a roughing clearance and running a finishing pass?

This sounds like a deflection related issue. What size shank is the endmill? Do what you can to minimize stickout. Check for any play in your Z.
Z plus or HDZ?


@WillAdams Yes, I’ve tried with an without a finishing pass (stepover 0.1mm) and with an without repeating passes.

@neilferreri The cheapo amazon bit is 1/8" shank and the 2L bit is a 1/4" shank. Both have about a 1/2" of stickout (I’m cutting a hole 7.9mm deep). This is on a stock pro which has a Z plus. I was thinking deflection as well, which was why I added the finishing pass in fusion. Shouldn’t that take care of any deflection issues?

What is the material you’re cutting?

1 Like

Oops, forgot to include that. For this part I’m cutting the hole 7.9mm deep in 6061-t65xx aluminum.

This was a square, with the same bit, in the same 6061 aluminium?

compensate with negative stock to leave with extra finishing passes. Also it helps to set your bore toolpath up with a rough/finish/spring for precise holes. I have to do this even on $30,000 machines so its pretty normal.

One thing to consider when cutting small circular features is that Fusion calculates feedrate off of tool center point, not the edge. You could be running a much much higher chipload than intended and that could lead to inaccurate hole sizes and tapering.

Check out this video

(Feedrate X ( Hole diameter - Tool Diameter)) / Hole diameter

I also suggest buying pin gages for accurate hole sizing, they will also help with letting you know if your holes are egg shaped due to belt calibration. Last tip, screw hand tapping…threadmill FTW!

1 Like

Thanks for tip on pin gage’s, seen ‘em used, never knew what they were called.
Will order a few from Vermont tool.

Some people call them pin, some call them plug, same same. Amazon seems to have a decent selection but you should also check out


Thanks for the video. Those tip videos are often really helpful! I want to get threadmills figured out but I couldn’t stomach the price tag and decided to try some threadmills from AliExpress which should arrive “some day” so until then I have no choice but to hand tap these things.

I sure wish I had a good pin gauge set (and a good micrometer and an optical comparator and … and …) but that purchase is going to have to wait for another day.

I cut a bunch of test holes and 1 real hole and now that I’ve slowed down to about 2.5 in/min for 2.5mm holes and 4.8 in/min for 3.3mm holes, they are coming out much better. It’s amazing just how slow you need to go with this small endmill.

Thanks, all!


RPM: 23K
Speed: 62 mm/min (2.5mm holes) / 120 mm/min (3.3mm holes)
Depth per rotation: 0.25mm
Multiple passes: On

  • number of stepovers: 1 [aka, 2 passes]
  • stepover 0.01mm
    Repeat passes: On

I assume I can probably get rid of the repeat passes to cut the time in half per hole, but I wanted to get a part finished and didn’t bother experimenting with that just yet.

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