I guarantee this is going to be a simple answer I'm just overlooking, but for whatever reason I can't figure it out. Any chance a Fusion360 expert has an idea?
When I'm building toolpaths, what's the cleanest way to clear the extra stock from around the model? Here's a random toolpath (not fine tuned yet, don't judge, etc etc.) to show what I'm talking about. How do I get rid of the green walls of stock around my part?
I'm an idiot but I think I figured it out. Is adding a 2D contour operation around the outside of the part the correct method?
I've not used fusion 360, but my guess is that it doesn't understand your stock boundary for the first operation up there.
Genetically, the algorithm should have no problem clearing that material, but it looks like it's trying to stay inside of your profile. Look for a way to either define a containment boundary and tell it that it can start "outside" of that, or a way to point it to stock and make sure that's using that?
To answer the question directly, no, adding the 2d contour is not the correct approach, it's inefficient. Notice how you're still doing small spirals to "peel" out the channel that is no longer there? You're also not going to be loading the tool evenly on your outer pass, limiting the feedrate you can achieve.
You need to be using adaptive or whatever Fusion calls their version of Adaptive/Dynamic/iMachining, etc.
I believe this video will get you pointed in the right direction, at least for 2d adaptive:
I'm still at the shop... but fusion 360 has an "adaptive clearing" method built in. That's how I go about doing my roughing passes to get rid of the excess material. Works great in conjunction with REST machining.
I'd go about it by: Larger tool and rough cut to maximum depth (either in passes or all at once depending on machine capability). If the cut is wider than the tool (from Stock OD to cut OD) then adding a contour pass (were still only cutting in a circle path right now) to split the cut into 2 works and still knocks out a lot of material in the shortest tool path. Just to be clear that the tool approaching from the outside of part. Should be rough cutting out everything you can at this point with minimal tool path. Anything where the tool isn't cutting is a waste (this is going to be a balancing act for the DIYer aspect, your time spent tool pathing vs actual cut time.
Once down to the depth where you need to start doing a complex contour then you can switch to actually following the contour. Use the maximum size cutter you can but it should be smaller that your radius sizes. For example if you have a .25 radius corner you can use a .5 end mill BUT that makes a "stop" in the tool path with a hard direction change and they don't like that. The solution is a smaller end mill diameter (like .436) OR plan your radiuses to be bigger (like .28) to make a smoother tool path for the cutter. Depending on how much you got with the rough cut and cutter size vs shape this can/should be just a single pass if the rough was done right.
Then I'd do the drilling and counter bores after that to finish up
Looking at the tool paths you have there is a lot of wasted cut path (air cutting) and way too many rapid travel paths.
If you have trouble getting it to compute the way you need/want you can always draw the cut path you want and use that as the tip control of the tool. Or you can draw an outer boundary around the part and use a pocket program vs a contour and out put the tool path as geometry. Then delete the ramp in sections and make it just plung outside the part and move into the material that way. Honestly there are so many ways to do it.
This touches on my old-guy thinking about CNC in general. Want to make a whole bunch of something, CAD is perfect. Want to make two of something, maybe. Want to make one of something, and I think a manual machine will get it done quicker. Yes I'm generalizing, yes it assume there aren't a bunch of highly critical dimensions, and large arcs are much harder on a manual machine, but still. And then there's the time and money spent on having extra stock for doing test pieces.
This from a guy who's gathering parts to build a CNC router. Why? Because I like building stuff, just not sure what yet, but I expect it to be slow going!
I haven't used F360 in a while but I'd start with a 2D adaptive. Select the lower outer edge of the part and leave .020" for a finish cut.
What does the actual part look like?
Here's the actual part, and my goal is to cut the outside of it on my CNC router, then do the precision work on the interior with the lathe.
And here are the machining boundaries I'm using: An edge on the top of the part, and a circle I sketched that's the size of the stock below it.
I think I solved it--checking "Stock Contours" seems to generate a fairly decent looking toolpath. Needs some refinement but at least it's clearing the stock now!
Success!
Looks great!
You'll need to log in to post.
