Fillet toolpath for bowl

Hi Folks,

I’ve been trying to figure out how to do a fillet toolpath with a 1/4 radius ball point. I’m using Fusion360 and have tried the 2D contour path but it crashes on the side of the wall the tool path. The area between the 2 arrows is the area i’m trying to target.

What’s the best way to do this on Fusion360? thanks in advance for any help :slight_smile:


You can do a 2D contour around the inside edge of your fillet, that would allow you to do finishing passes as well.

Post the file if you’re still having troubles.

I tried that and somehow it just goes all over the place then. Here’s there file attached to it.
WoodTrayMoon (1015.3 KB)

I made something similar recently. Had to fight a bit with it, but the solution is filleting the inside of the sharp corners to the radius of your bit or more.



A few suggestions on toolpaths and machinability.

  1. The sharp corners are not reachable and will produce a full contact with the cutter which will likely introduce vibration, poor finish, surface burning and a nasty noise, potentially chipping out the wood too. I suggest putting a fillet in here with a radius larger than the cutter you plan to cut the shape with, this allows the cutter to roll around the inner corner without that heavy engagement.

If you want to preserve a sharper corner here you’ll need to do your finish toolpaths with a smaller cutter. That will slow and complicate your other roundovers and fillets.

The sharp outer corners may also chip off during machining, depending on the wood and grain direction. You can get more specific with selecting contours and order of cutting but you need to know what’s chipping and the grain directions first.

  1. The RPM for the 1/4" flat cutter seems to be set to 5,000 which seems rather low, the feedrate seems more consistent with a 20kRPM or so cutter speed.

  2. I grouped the toolpaths by cutter, there’s a bunch of 1/4" flat toolpaths as you previously had it for roughing and flat surface finishing.

  1. I re-ordered the 3D adaptive and the pocket toolpath as the adaptive was wasting lots of time retracting Z and traversing across the pocket not cutting. I told the pocket toolpath to use the stepdown you had in the adaptive clear, leaving the 0.5mm stock to leave you’d configured.

The adaptive then doesn’t have much to do and can’t spend as much time retracting and air cutting, I tweaked the minimum engagement values here to speed that up too.

  1. I suggest doing the inner and outer vertical walls with a contour with a finishing stepover (which avoids full slotting on the finishing pass), not sure how you plan to do the workholding or finish the outer edge but the toolpaths are there, the outer is currently set to stop 5mm above the model bottom, that’s easy to configure.

Inner toolpath

Outer with depth from bottom

  1. A couple of parallel toolpaths, using the avoid / touch surface trick to contain them finish the flat faces to dimension (and finish off that 0.5mm stock to leave from before)

  1. A contour toolpath can use the 1/2" ball nose cutter, but I wouldn’t use it for this piece as it can’t get into those sharper corners and will leave nasty lumps for you to fix when sanding.

  1. Instead I’d suggest using a contour or ramp with the 1/4" ball nose cutter to hit those curved faces with a small enough step down to minimise the sanding afterwards

We can keep the ramp contained to the curved surfaces by using the slope constraints

Also, I’d suggest a little stock to leave on the ball nose toolpaths to allow you to finish sand it flat, if the ball nose digs deeper than the flat finished bottom surface the sanding becomes a pain.


WoodTrayMoon v6 (705.2 KB)


Liam Thank you ever so much!

I learned quite a bit from the file that you sent back. I’ll keep hacking away it, and give this a try. When I saw your reply this morning, gave me hope about good folk in the world :slight_smile:


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