Originally Posted by
jwatte
If you get an error about exceeding some dimension, then it means that the mill thinks it would have to jog into the limit switches to perform the operation you asked for.
Move your work slightly to give it a little more room. Also, make sure you always "ref axes" for all three axes each time you turn on the mill. If the ref axes indicator isn't green, you're living in a world where the mill is confused about coordinates.
If your 1/8" end mill was a ball nose, then know that the bottom of a ball is much finer than the side, so you typically will want to feed much slower than you'd feed for a square end mill. Use the formula you'd use for plunging, as a first order of approximation (regular feed divided by number of flutes.)
Your picture says nothing about whether you did it right or wrong. What material was it? What was your depth of cut (axial engagement)? What was your radial engagement? How fast did you spin the spindle? How fast was your feed rate? How many flutes, and other cutter shape parameters? Answer those questions and people can give a reasonable estimate of where you might have been off.
When you pick a tool in Fusion, then the diameter of the tool is important, and the height is important if you rely on Fusion to detect collisions with the collet. Assuming you have entered the correct tool height in the offset table, and assuming you set your Z-height correctly, then the mill will put the end of the tool where it "should" be according to Fusion, even if you didn't tell Fusion about the exact height of the tool -- it's referenced by tip-of-tool.
I haven't engraved letters, but I know people use drag engravers for thin and outline type, and vee bits (spinning) for deeper letters. There is some way to make Fusion engrave as deep as it can within the outline of a particular set of letters; I've seen a YouTube tutorial about it somewhere. For good-looking letters, that's what I would do.
If your tool in fusion is exactly-on-the-dot the same width as the slot you've modeled, then Fusion may detect a collision and refuse to generate the toolpath. However, that's generally not a great idea, because the finish of that slot won't be great; you'll want to have some room to cut in the middle, and then run finishing passes (or at least one finishing pass, on the side that you didn't climb cut on.)
The "oscillating thing" is for material removal (Fusion usually calls these "adaptive," and you will want a finish pass at the end of that to clean up the edges. Typically you will want to leave a few thousandth's of an inch of radial "stock to leave" during the slotting operation, so there's something to actually clean up. If you just want to cut along the edges, rather than go sideways in the slot, use a 2D profile toopath, or if the slot is wider than 1.6x your cutter, use a 2D pocketing toolpath (not adaptive.)
Generally, when you want to clean something up, you make some "stock to leave" for radial (sideways) and perhaps axial (bottom) directions. Then you use a finishing pass along the edges, usually with 2D contour or perhaps the pocketing path. Also, some toolpath generators will let you put a checkbox in to generate the finishing pass last. Because the radial engagement is generally quite shallow, you can typically take much deeper cuts (axial engagement) when finishing; you'll want to shave the entire wall in one operation if you can at that point.
Finally, the limiting factors for spindle speed (RPM) are your cutter materials/coatings compared to the material you're cutting (surface speed,) and the spindle horsepower if you have bigger cutters/deeper cuts. If you think you're taking too much feed rate, you can take less per tooth by increasing the RPM while keeping feed rate constant (assuming you're not at the limit of your spindle.) Meanwhile, if you get a lot of chatter, you can try reducing RPM and perhaps increasing feed a little bit, which generally will quiet down chatter, although at some point that will overload the bit and break it.