Depth of Cut - #251 Endmill

I’m cutting five 6x4" boxes out of a piece of ash with a #251 end mill, and was wondering about the timing.

To cut the pockets (1.25" deep into stock 1.5" thick) in all five boxes will take over 690 minutes with a DOC of 0.04" (which is the default, and I know id ‘conservative’), but with a DOC of 0.046" the time is reduced to 342 minutes.

0.006" doesn’t seem very much for such a significant time saving, but does anyone think this coud present an issue?

Thanks

sort of rule of thumb: you can bump a DOC to half the diameter without too many issues.

But there is a catch: Your machine more or less has a upper limit for “DOC” times “feedrate” times “engagement/stepover”. (Some folks will also multiply the RPM of the spindle to this but for this lets assume RPM is your maximum of the router and constant)

So you can increase DOC (to half diameter as rule of thumb although folks go deeper)… but once you get to the machine limits, you’re going to have to reduce either feedrate or stepover. Stepover is tricky (since the first part of the cut is always at 100%) so in practice the easy thing to manage is feedrate.
(The maximum also depends on many other things, like a new sharp cutter can go futher than a dull old one… complicated world the formula above is a huge simplification but works quite well)

The CC defaults have a lot of room left before you hit the maximum… So one thing you can do is cut at say 0.08 at the default CC feedrate for your material, but in Carbide motion use the speed override to set it to less than 100% (say 70%). If the machine is happy, you can start increasing it while cutting… even to > 100%. You’ll hear when the machine starts struggling well before it reaches a failure point.

Note: If you care a lot about the quality of the walls or the floor, as you get closer to the max for the machine, the quality will go down a bit. So one common trick is to the the pocket to 1.22" first, and then do another pocket from 1.22 to 1.25" (and if you want an even nicer finish, you can do this final pocket with a reduced stepover, say 25% instead of the default 50%).
If the cut to 1.22 leaves a bit of a rough bottom, this final 0.03" cut will clean it up basically

6 Likes

Thanks, @fenrus, but just so I’m clear, I’ve attached the file and would ask you to take a look to see I’ve understood correctly.

I’ll then do this:

Thank you :+1:

Rectangular Box x5.c2d (239.0 KB)

for your second pocket you set the depth to 1.5" did you mean to do that?
(I thought you wanted 1.25". If you wanted 1.5" then my suggestion would be to do the first pocket to 1.47" or 1.48" but since you said your stock was 1.5" in the original post I suspect this 1.5" was a slight typo in the design file)

Below I fixed the 1.5/1.25 thing but I did one more little tweak: I made a 0.01" offset shape of the inner rectangle, and used that for the first pocket. This will leave a 0.01" wall that the final toolpath will remove in one go, this not leaving horizontal marks.

BTW one more thing to look at. You’re cutting 1.25" deep, but I thought the 251 bit only had 1" long cutting size… (I don’t have an actual 251 so cannot measure) if that’s the case you might need to not do the 0.01" thing, and you my need to be very careful, using the bit above the cutting area has issues.

Rectangular Box x5.c2d (256.7 KB)

Edit: The CC website claims a 0.75" cutting length for #251. With that you need to be careful in two ways:

  1. Make sure that the bit sticks out at least 1.5" from the collet, so well more than just the cutting length, because if it doesn’t, once the toolpath goes deeper than the stickout, the collet will hit your wood and that’ll be a very bad disaster

  2. you need to realize that the “upper 0.75” that is not cutting, will rub against the wood a bunch. In and by itself that isn’t great but also not a disaster, but this rubbing will lead to heat and can even lead slight burning (dark staining) of the wood…

there are ways to deal with this in the design, but they’re a bit more complicated.

Basically the idea is to, instead of a contour, you make a pocket upto 0.75" that is 0.01" or 0.015" or so wider than the bit (so 0.26" ish), and then from 0.75 to 1.5" depth (or however deep you need) you do the contour in the middle of this, so it leaves 0.005" on each side at the top, so that the shaft of the cutter does not actually touch this part of the wood.
(if the toolpath has space to spare, I would suggest an even wider pocket, something like 0.3" or so, but the contour path would still be 0.01" away from the edge of the pocket)

For the pocket, you just turn your first pocket into two; one upto 0.75" and the second 0.01" smaller (so inside offset) for the 0.75" to 1.22"

2 Likes

Whoops. I’m glad you noticed my deliberate mistake! :scream:

Thank you :+1:

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