I have a bunch of pieces of a mahogany that are 7.75" wide and between 1.75 and 2" thick that I need to cut the sawtooth detail out of one end. In the first three I did I used a simple profile tool path. That was quick, but I did get some tear out when the bit exited some of the teeth. Does anybody have any suggestions of more clever ways I can set this up so the cuts are cleaner? I use Rhino3D for my CAD work and have VCarve Pro mostly for CAM. I don’t have any experience with Fusion 360 but from what I’ve read Fusion sometimes has better tool path solutions.
I had a similar problem with some custom moldings I was making. One corner always chipped out. So I changed the CAM to cut the end grain side of that corner first - I mean, even before roughing. It would dig a hole down into the wood, make one finish pass across where the one edge would be, then move on to the next problem corner. Then do everything else. Thus, when it got to that corner in the normal flow of things, the cut that would have chipped it had already been done, and fully supported at the time. Every corner came out perfect.
Yeah! In Fusion, you can define where the profile cut starts and ends. In general, you want to do a conventional cut for the profile, but this will leave tear out on the exit. To fix that, I first do a short climb cut just on the 2nd cut’s exit area. You can make it short by setting the “extension” to be negative.
Thanks! Since I have 10 ‘saw teeth’ that would be 10 short climb cuts to the depth of the material. That’s fine. Do you know a clever way to do that with one curve or do you think I’ll need 10 little angle vectors for those cuts in addition to the one main vector for the conventional cut? If that’s the case, VCarve would work too, since I can define where the cuts start in that as well.
I think I’ll also try (in scrap) a test where I I rough out some of the material and then do a final finishing pass, hopefully with less tear out.
In Fusion, you will be doing a 2D contour. You select “Chain” for the selection, and then on the window that comes up click the button for “Open Chain” and select just the line you want to go inwards. You can manipulate the start and end extension (try negative) to make it not cut all the way or to cut further. Here’s a quick photo of this.
Then you’d create another 2d contour with the other direction (sideways compensation in Passes) and select the other side to have it cut the other way.
I’m not sure this is the best approach for that shape..as it will take a lot of time to do the toolpath! Just an idea on something to potentially try. I’d have to see it cutting and see the result to really have more ideas on how to solve it.
Thanks. I think I’ve solved it. First I set up and ran 10 little climb cuts before cutting out the whole thing. Unfortunately, the chip out was about the same. I’m using Eucalyptus Grandis, which is a hybrid farm raised mahogany and it is a bit prone to chipping.
So then what I did is cut the end curve out without any of the teeth first, as is seen in the first photo. Then I did the 10 cuts that would be the exits on the last tool path (second photo), and then I ran that. This worked MUCH better and I have a good result. Since I have to do 15 more of these, this is a very good thing.
