As the first part of the new moteus servo mk2, and continuing in my series of learning about CNC by building parts for the quadruped, next up I machined the input to the planet gears on my Pocket NC V2-50. This was a part, that for my quad A0 build, I used a 3d printed part in PETG as it is probably the least stringent part in the gearbox in terms of tolerances and load, although I still expect the plastic ones will likely wear and fail after some time with heavy use.
In the gearbox, this planet input interfaces to a number of different sub-assemblies:
The planet output inserts into its studs, the planet shafts insert into recessed holes in the face, and the planet input bearing fits into its center. Bolts fit through the back to pull the planet output towards the input. There is also an indexing cutaway on the outside for an eventual absolute position system.
I made these from round stock, 1.75in in diameter cut to 1″. The machining was done in two setups, each using the Sherline 4 jaw chuck mounted to the B axis of the Pocket NC.
In the first setup, the back side was roughed out, the center hole was cut out, and each of the holes for the bolts was bored along with a countersunk region.
The second setup, flipped over, first roughed, then proceeded to finish each of the necessary surfaces. There were two more interesting bits here. First, I made an alignment fixture so that I could get the holes from the back and front half to align. That consisted of a cylindrical shell that fit into the mounting pattern on the B table of the pocket NC and a thin plate that fit under the part. The thin plate just stays in place during the machining operation, where the shell pulls out.
The other interesting part was that I ended up clearing away a bit of the inside of each stud so that my bit could reach down to finish the bearing mounting surface. That way I could get away with just using an 11mm flute, which already gave a terrible enough surface finish that going longer would have only made worse.
As I’ve observed in the past, I had yet another problem with tool pullout during this part. Here, the problem was very similar to my past incident, when Fusion left a thin wall, then tried to punch through it. My fix from then was doing the right thing, however the wall was just too thick I believe, causing the toolholder to lose grip. In this clip, you can see that after it breaks through the wall, the mill cuts through some stock as it repositions over. The slip was only about 0.3mm, but that’s enough to mess things up.
However, this time I think I figured out an even better solution. Simply lie to Fusion 360 about the diameter of the cutting tool and say it is slightly undersized. That results in fusion leaving the adaptive passes closer together, and thus no thin walls or foils are left behind. It would be nice if that were just an option in the adaptive settings. I suppose you could override it in the “Compare and Edit” window, but creating a faux “tool” just for roughing makes it easier for me to see that I’ve applied the override correctly.
Here’s a video showing the different tool paths for the finished part:
The stock cut of 1″ is oversized in this part and adds a bit more than an hour to the cycle time over a minimum sized piece of stock. I need to get a setup for cutting stock smaller than an inch here soon.
Also, I’ve discovered that ekramer3 has been testing the 4mm single flute Datron endmill, which should be able to nearly double the MRR for the roughing passes. I’ll give that a try on the next part I make.