Endmill smaller than it should be?


I wanted to test out the Nomad precision and make something fun at the same time, so I decided to try to make a 90 degree dovetail joint. These pegs/slots are supposed to be .375", and the plywood is ~.5" thick

It’s pretty cool, but the pegs don’t fit into the slots, and calipers verify that the slots, which should be .375" across, are actually more like .371-.372" across, and the pegs, which should also be exactly .375" are too large by the same amount (so the pegs are ~.006-.008" larger than the slots.

I was curious as to why this might be (precision limit of the machine, something else), but the pieces I milled look basically perfect, with no drifting or any other issue like that, and then I noticed that this long, skinny slot:

which was basically a slot made by waterlining a .125" flat mill down (actually, the slot is modeled at .126" or the CAM software wouldn’t make a toolpath through it), is measured by calipers at .123" across, smaller than the endmill size itself.

Is it possible that the endmill is smaller than it should be? It’s hard to get a good caliper measurement on the endmill itself (the fact that it has flutes makes it hard to get a “widest diameter possible measurement”, and also I didn’t want to damage the endmill edges), but it kind of looks like the endmill is only .123" wide near the tip, and .125" at the shoulder. Is this possible, or am I crazy and doing bad measurements biased by my preconceptions? If not, what else might cause this?

Related question: if you were to try to make something like this (cut out a shape, then in another piece cut out a hole that’s the same shape), what size gap would you design in if you wanted to get a nice fit? 0? .001"? .002"? Does that answer change if you’re doing it in hardwood/softwood/plywood/aluminum?

Welcome to the world of tolerances :smile:

When you get cutters in, you’ll discover that it’s not uncommon for them to be slightly more or less than you expect, within a tolerance. The best way to measure the discrepancy is to draw a box in your CAM software to have them mill that, with just waterline passes, and then measure the result.

If you create a series of ~4-5 10mm x 10mm squares in a row, you should be able to measure them to see if they’re consistent in actual size on X&Y, and if there’s an offset, by how much. If your CAM thinks it has made a 10mm x 10mm box, and it’s actually 10.2, then that tells you the cutter is .2mm smaller in diameter (radius applied to both sides of the cut). Or, if it turns out to be 9.8mm, then your cutter is .2mm larger than anticipated.

I just measured one of my .063" tools with calipers, and they’re .062" toward the tip—the method I used was I held the tool in one hand and spun it backwards to how it would turn in the spindle, so that the back-side of the flutes (the ramping side) is what’s pushing against the caliper jaws. I pushed the calipers tight and then spun the tool backwards in this fashion, with the point against a surface so neither the tool nor calipers wouldn’t slip vertically.

I did some joinery recently to make a hot-wire bow for a robotic arm—If you’re trying to do precision fits, you have to be ready to do a little sanding sometimes, and also account for your tool actual size!

1 Like

Thanks for the info! Yeah, the only issue with the endmill being smaller than advertised… it seems like the shaft of the endmill is actually the correct size, which means it is larger than the cutting end. So when I tried to mill vertical walls, by the time it got ~3/8" down, the shaft would rub (slightly) on the higher parts of the wall that were cut in earlier passes. This results in taper on all of my tall vertical wall objects (and it’s not the same taper-only-on-one-side I had back when I had my X axis drift, but it’s real cutter taper/tool-deflection taper). I just milled out a 20mm tall object and the top is basically dead on to my specifications, but the bottom is flared out about .17 mm (.08 on each side). I guess what I should do is buy a bunch more endmills and then find one which is more “perfect” and use that when I need to do tall walls…

I would suggest rather than buying a bunch and guessing, look into getting some long-reach tools—personally I’ve been pleased with the tools from Bits&Bits, but there are a lot of vendors out there that can provide good options.

You’ll want to slow your feeds when doing deeper cuts though, typically you cut speed by 25% when doing 2x depth relative to diameter, and cut speed by 50% when doing 3x depth relative to diameter… but that’s assuming full-plow cuts, so if the increased flute length is just “skimming” the walls, you probably ought not slow things down for that as much.

Good luck!

Did you ever get that joint to fit right ? I’ve been designing a very similar joint with a rabbet instead of the tapered 45 edge. My teeth are always about .015" too wide and my gaps are too small by about the same width (teeth are supposed to be 0.75" and are actually .765" gaps are .735") . After reading this I’m starting to think it’s my bit that is responsible for the offset. the inside distance between teeth is .735" and the outside length of the piece is 6.015" instead of 6" even. I’m thinking the only way the inside cut and the outside cut are off by the same amount is if the bit is smaller than its supposed to be right?