CNC'ing some dog holes

Hey folks, I’m a total noob at the software side of things, so please excuse my total ignorance here. I’m sure I’m missing something simple, or doing something obviously wrong, but here’s my problem…

I’ve got a simple test model in Fusion360, a 10"x10" block with evenly spaced 4 3/4" holes in it. I have done a couple of test tool paths using a 1/4" spiral downcut bit that I’ve calipered and correctly set up and selected in my pocket / clearing action.

Problem is, no matter what milling action I choose to do this with, they come out undersized - somewhere around .62" instead of .75.

What’s the correct way to generate a tool path for essentially drilling some holes?


how deep are the holes? If they are very deep and you are taking only one pass, it could be tool deflection?

How many passes? how many different depths? Finish pass?

Fusion has a “stock to leave” option active by default on pocket/clearing operations, make sure it’s unchecked

Otherwise, it may simply be the tool not being the diameter it pretends to be

Make two squares, cut one outside the line, the other one inside
If the “outside” one does not fit into the “inside” one, your tool is smaller than advertised
If it’s the other way around, it’s larger
Adjust your tool radius in the tool library accordingly

Also you might want to just “bore” those holes, just make sure the remaining plug stays put

post deleted

Dude, you nailed it. Thank you so much!

Thanks everyone who piped in with ideas - this is such a great community!

So that would essentially hollow out a donut of negative space laving a hole with a boss in the center?

That would make for a lot less milling, but I have no idea how I’d keep that 1/4"ish projectile from taking off…

Not really. I did the math, milling out a 3/4" hole with a 1/4" end mill removes only 12.5% more material than milling out a 3/4" donut with the same end mill.

Also note that you can use this option to your advantage.
Setting a negative “radial stock to leave” value will make the holes slightly larger, and contours slightly smaller.

It’s a great way to separate concerns between design and machining too: I tend to CAD with exact dimensions, and then adjust stock to leave in the CAM program to get a good fit (either snug or loose, depending on the features I need)
This leaves the design somewhat “clean” using the real intended dimensions, rather than weird numbers only suitable to your machine and current bit… much easier to read when you get back at a design a few months later…

Maybe painter’s tape and superglue? but you’d need to have tape pretty much everywhere on your grid

On an MFT top these add up quite quickly, there’s a ton of holes in those things (77 holes on a standard mft)
Also, the boring operation is pretty easy on the mill, it’s just a gentle ramp with continuous engagement of the tool, and you can speed it up substantially without any problem
A pocket or adaptative cleaning operation on the other hand will require to take passes at multiple depth . Both of those operations will also require a finishing pass for good accuracy…

I was thinking about how slow the pocket and adaptive clearing operations were in my tests, and that 1/4 boss… Then I thought “hey, my bit is exactly 1/4”, I wonder if I can just drill the boss away before I do the boring operation?"

So I set that up, and the total machining time (with a finishing pass) is 1/15th of the time for an adaptive clearing operation (neither has been speed optimized, but wow).

I think I can get it down to about 1 minute per dog hole… will be running some more tests this evening!

1 Like