I’m wanting to do a simple pocketing operation in Fusion 360. Bulk clear with a .25 and then a fine edging pass with .06. Now in makercam or CC I would create two toolpaths: One pocketing operation with the .25, then an interior contour pass with the .06. I understand I could do this exact thing again with Fusion, but I’m wondering:: is there a smarter way to do this? Is there a multipass (with different cutter) type of path? And is it smart enough to, if I told it to pocket first with .25, then again with .06, to only run the .06 toolpath in areas of the pocket NOT cleared by the .25pass?
You really need to ask technical Fusion 360 questions on the Fusion 360 forum. The Fusion development people, trainers, presenters and certified experts are always on the forums answering questions just like these. If you post your work (or share it) they will look at it, fix it, recommend what you should do, etc., often times giving a presentation you can follow step by step…much like what happens here with the CC program.
The appropriate way is two operations. One with the 0.250" cutter, followed by a second with the 0.062"cutter. The appropriate option to select for the second operation is “rest machining”. This means, literally, that the operation is machining the rest of the material another couldn’t get to.
The second operation must be in the same setup as the first, and, generally, should be the same operation. For example, to do a large rectangular pocket in a softer material (woods, plastics, aluminum on a machine with sufficient spindle power), I would run the larger bit with adaptive clearing(2d), and maybe a 0.005" radial stock to leave (zero axial), followed (edit) 2d pocket operation with the smaller and rest machining selected and te same 0.005" radial stock to leave. The follow up would be a finish operation (2d contour) to clean up the last 0.005" of stock using the 0.062" bit. Why 0.005" for the finishing op? It is a safe single pass with the 0.062" cutter in most materials and is enough to insure that the cutter cuts rather than rubs.
edit: Fusion adaptive does not have rest option. 2d pocket must be used as second op
edit 2: Also, watch the depth of cut. You may need to select multiple depths, especially with the 0.062" cutter, if the pocket is deeper than a few mm.
Thinking this through a bit further, would Rest machining worked if used with a 2DContour op with a straight mill, then a engraving pass with a vbit? Thinking of how to clear large fields in engraved paths without trying to use the vbit and one billion little scratch passes.
Thinking this through a bit further, would Rest machining worked if used with a 2DContour op with a straight mill, then a engraving pass with a vbit?
I haven’t tried that. I don’t think it will work that way, but it wouldn’t hurt to try. I wouldn’t tend to think of this as a good application, though, as what you are describing is really a roughing/finishing sequence. Rest machining is intended for when a cutter doesn’t fit into a feature (a corner, a slot between two pockets, etc) rather than when the cutter shape is changed.
For this type of thing, I use a tool like adaptive clearing with a flat end cutter (multiple depths to Keller it in), then a new operation to remove the stairstepping with a vee (or ball-end) tool. This operation can go fast as there is no need to run multiple depths for bulk material removal and, with the appropriate size vee bit (or, for more general surfacing, ball-end) the surface can be cleaned in few passes.
Can you post screenshots of your CAM setup of your object in Fusion? It’ll make it a lot easier to comment. Also, some additional questions:
Material?
Depth of pockets?
Flute & shoulder-length of 0.06" tool?
Final surface finish desired? (flat, scalloped/textured…)
I would revise on @enl_public’s comments and suggest this instead:
Do a 3D adaptive clearing path with 0.25" tool, with roughing passes and a finish pass at final depth. Make the finish-path step-over 5% of the larger tool (0.25") diameter, and cut using 25-35% step-over as your optimal load. Leave 10% of the smaller tool’s diameter as your radial stock to leave. Unless you want to have a particular pocket bottom finish with the small cutter, there’s no reason leave any extra axial stock if it’s a flat-bottomed pocket, and if you don’t need a perfectly flat bottom. Your step-down depths are going to be material determined, anywhere from 5% to 100% of your cutter diameter. You want your feed-per-tooth to be 0.5-2% of the tool diameter, depending on the material and depth of cut.
Then you’ll load your second cutter (and re-zero the Z for the second tool) and run a 2d contour, possibly with multiple step-downs based on pocket depth, if you’re just cleaning the walls up. You’d use no stock to leave and a 0.5% feed-per-tooth to ensure a smooth wall. If you want to have a completely even-surfaced bottom then you’d run a 2D adaptive or regular 2D pocket, depending on the surface look you’re going for, and you would want to have left about 5% of the small-tool’s diameter as your axial stock to leave in your earlier large-tool roughing operation.
That may be a bit confusing, so I can post an example if you can show some screenshots of the kind of thing you’ve got drawn up.
