After doing my first cuts in aluminum, I wanted to actually try and make a real part, to prove that the Pocket NC v2-50 was capable of making things that I can actually use. My first attempt, was the same part I did my first aluminum cuts in, the sun gear holder from the BE8108 planetary gearbox.
This part attaches to the rotor, the sun gear, the position sense magnet, and has bearing interfaces to the planet input and the back housing. While not terribly big, the number of features and mating surfaces is relatively large.
First, before we start, here’s a video montage of all the machining, apologies for the bad lighting and focus:
Second, be warned that this is a *long* post!
As mentioned earlier, I decided to try an approach that would allow the entire part to be machined from a single piece of stock and a single setup. That is one of the advantages of the 5 axis pocket NC. Even for parts like this, the 3+2 indexing means that I can access all the faces in one go. Then to finish it off, at the end I left a thin tab which would be broken by hand and filed away.
Before I get into the details, let me be clear, that this is the first real part I have ever programmed for a CNC and there is a lot I am likely doing in a sub-optimal, if not terrible way. I won’t document all future parts in this much depth, but writing out my thoughts for this one will, if nothing else, give me a reference to come back to as I find my footing.
I marked all the individual tool paths with an initial bolded number (N:) so that you can correlate them to the video if you like.
I used 1 x 1.5″ rectangular 6061 stock cut to 2″ in length (so it came approximately 2.125″). This was placed into the Pocket NC vise longwise, so that the 1″ side just about exactly matches the vise’s set screws.
This part may have *just barely* fit into a 0.75″ x 1.5″ stock, but I didn’t want to risk having so little margin on my first attempt. I originally chose this orientation because I thought that it would be easier to center by hand, although upon reflection putting the long side against the set screws would allow me to use the narrower 0.75″ stock.
I don’t yet have a reasonable means of cutting stock here, so just had Speedy Metals ship it cut to the correct length.
Back side roughing
1: To start with, I used the 3mm Datron single flute endmill that Pocket NC sells for the bulk roughing of the back side. The majority of the roughing for that side was accomplished using a single adaptive clear. The final path looked like:
I started out with the speeds and feeds I had used last time, derived from Ed Kramer’s posts. Since I was using a 3mm instead of a 2mm end mill, I just upped the stepover to 0.3mm initially and left everything else the same.
This was definitely the tool path that I had the most trouble getting to work — I had a couple of different problems.
First problem – tool pullout
To start with, this tool path worked just fine, if a bit slow. However, once the path got into more complicated geometry, I had what I eventually diagnosed as a tool pull out event that manifested as the spindle stalling out. It looked like the tool pulled out about 0.2 – 0.4mm, and then started just hogging through uncut material. This both caused a defect in the surface and then the spindle to stall out.
My debugging of this problem was complicated by a different issue. I had not really done any math to select a proper stickout for the tool for this path. Slightly past the point of pull-out, with my initial 20mm stickout, the machine faulted because on the next pass the Z axis travel limit would have been reached. However, the fault was so far removed from the program point where the limit would have been reached, I initially assumed it had just pulled out again. Thus, I made a lot of tweaks, none of which fixed the stickout problem, and some of which may have fixed the pullout problem.
Ultimately, I now believe that the pullout problem was likely caused by the “Tolerance” parameter of the 3D adaptive clearing path in Fusion 360. My initial settings for this were 0.1mm or 0.15mm of tolerance and 0.3mm optimal load, which I figured would result in a usable amount of error. However, I hadn’t expected geometries like this:
When the tolerance was set too large, the tool “cut off” that long piece of material, going from an optimal level of engagement to nearly 100% engagement in a heartbeat. The v2-50’s NSK spindle doesn’t have a lot of clamping force on the tool, so that drastic change in load must have pulled it out.
Despite that as my ultimate conclusion, I still ran all the rest of my paths a bit slower at 30k rpm 600mm/min and a stepover slightly under 10%, so 0.25mm for the 3mm endmill because that was what I did my final testing for this problem with. I wanted to get a part in this round, not necessarily optimize speeds and feeds.
Second problem – Z axis travel
As I mentioned above, the second problem I had here was that the Pocket NC Z axis travel was insufficient to reach past approximately the midpoint of my part with a 20mm stickout. In fact, I had to increase the stickout all the way up to 28mm before I could complete this toolpath. I didn’t experience a whole lot more chatter after that change, and my surface finish was equally mediocre before and after, so it was probably reasonable at least for cuts that were this gentle.
The rest of the backside
The remaining pieces of the backside were:
- The central cavity
- The planet input bearing interface
- The back most visible surface
- The “bearing lip” for the planet input bearing
- The back surface that mates against the rotor
2: First, let’s tackle the central cavity. I roughed out the cavity with a bore toolpath. I used a relatively small initial bore diameter, then did multiple stepovers to reach the desired diameter. I later realized this was moderately inefficient, and I should just do a bore of a single diameter and let adaptive clearing handle the rest, but I didn’t bother updating this path with that strategy.
I was pretty apprehensive running this boring operation, as clearing out a cavity is what broke my first endmill. I ran this at a very conservative 0.2mm depth per turn, and at 30k rpm with 400mm/min cutter speed. Also, I discovered that I needed to manually set the top height a bit above the start of the cut to get the cutter to actually start its helix before engaging. With the default 0mm offset, it ended up plunging straight in and sounded terrible.
Even with the helix moving before engaging, it still sounded pretty bad, but did make it through. I guess using an actual drill is probably the only way to achieve this depth of cavity on the Pocket NC without having significant chatter. Fortunately, I didn’t really care about the surface finish, and the chatter didn’t seem bad enough to break anything so I just ran with it.
3: Then I used a 2D face to finish the back most surface:
4: Then I used a 3d adaptive to finish clearing out the bulk material from the central cavity. This is what I should have just let remove all the material after the initial bore:
5: Next I used a 3D parallel to finish off the rotor mounting surface. This was a little bit tricky, as at this point in the program I have the beginnings of a “tab” beneath the part that I don’t want to dig into. Thus I defined a boundary as a sketch in the model for all the things that I wanted to keep away from that tab. Here I used used it as the “Machining Boundary” with the “Tool inside boundary” option and added a random additional offset set to make the simulation not get into the tab.
6/7: Finally, for the back side, I used two 2D circular paths to get the planet input bearing interface, and the “lip” behind it, to their proper diameter. I used a 3mm stepdown for both, although for the best finish the 3mm endmill is long enough I should have just done it in a single cut. I also used the “Wear” tool offset compensation, so that I could enter small offsets into the Pocket NC tool diameter to dial in the exact dimensions I wanted.
The front side
8: For the front side, I initially did as much as possible as I could do with the 3mm end mill. So, that started with a roughing of the non-cavity pieces. This used identical parameters to what I settled on for the back side roughing.
9: Then I used a 2D face to finish the front most surface. This is both ways and has a 0.5mm stepover.
10: I used a bore path once again to carve out an initial hole in the front cavity up until the narrower part of the hole. For this one, I also used a few stepovers, here spaced at 0.25mm and also manually set the top height 0.5mm above the hole.
11: After that, I used another bore to get the narrower hole in the middle.
12: A 2D parallel finished up the front surface. Nothing actually mounts to this, but I figured I might as well make it flat. As with the facing, a 0.5mm stepover was used. I ended up just selecting everything but the back flat face as a “Avoid/Touch Surface” set to avoid to keep the path from trying to get there. I also didn’t do anything special to keep this away from the tab, which resulting in it digging a bit into that region. I was mostly worried about engaging the full width of the cutter, but it didn’t cause too big of a problem, and the 2d parallel path did that a bit anyways as it worked its way around the central post.
13/14: The last two things that I did with the 3mm flute were finishing the interface to the rotor bearing, and the bearing lip using 2D circular paths.
Front side – 2mm end mill
The other features I needed to do on the front side were all too small to complete with the 3mm end mill, so I switched to a 2mm single flute Datron with 5mm long flutes for the subsequent operations.
15: First, bores opened up the four bolt mounting holes that connect the part to the rotor. For these, I used just a single boring pass, but manually set the height to be a bit above and below the part. Above so that the helix would start before it engaged, and below so that I’d be sure to actually get all the way through the part.
16: A 3D adaptive removed most of the remaining material in the front central cavity:
17: And a 2D contour removed the final bit of material:
18: The last thing I did in this tool setup was to clear away the remaining outside material that was above the tab, as all the “heavy” cutting is done. This was done with a single 3D adaptive clearing, with the depth of cut set to 3.5mm so it finished in a single stepdown.
Now that almost all the material is removed, I switched to a 90 degree chamfer mill. This I just got from Shars, part 416-3509. I wanted to break all the sharp edges I could and also needed to cut the countersinks for the mounting bolts.
19: First, the front chamfers. I used a 2D contour with 0.25mm of “Chamfer Width” and 0.25mm of “Chamfer Tip Offset”:
20: Then, while still on the front side, I did the countersinks. For these I also used the 2D Contour toolpath. I used as many stepovers at 0.2mm as I could fit in, which worked out to 7 in this case. Since these chamfers were modeled, I left the “Chamfer Width” and “Chamfer Tip Offset” at 0mm. In hindsight, I probably wanted some tip offset still, as it left a tiny flat at the start of the chamfer.
21: The last thing I did with the chamfer mill was the back chamfers, which were done identically to the front ones, just with a different “Tool Orientation” selected to come from the back side.
Finishing up and parting off
22: At this point, I switched back to the 2mm end mill from before with the same stickout to get ready for parting. First, I used a careful selection of boundary to remove all the material laterally, except for the final parting tab with a 3D adaptive. Because this is reaching in far, and the shank of the tool would otherwise rub, it spends some time carving away at the base of the stock to give room for the shank to reach in.
23: Now, as much of the outer surface is exposed as is going to be exposed, so this is where I stuck my finish pass for that surface. I used a 3D contour, which let me restrict its operation using the same machining boundary I used before so that it didn’t run itself into the tab.
24: And finally, I used a 3D adaptive to clear away all but about 0.2mm of the remaining material in the tab. The selection of tab width was one I was concerned about, never having done this before. Too thick, and breaking it off would be annoying. Too thin, and the part might fall off while the mill is still engaged and spinning. In the end, the 0.2mm was totally reasonable to bend off by hand, but still seemed relatively well fixed as the mill worked under it.
The final result!
Some pictures of the final part:
Clearly, there are plenty of areas for improvement.
Surface finish: As seen in the close ups, the surface finish, is at best, “mediocre”. I didn’t really try to optimize this, but did try to avoid obviously loud chatter. Perhaps I can run some of the paths with the same tools but at smaller stickouts, or perhaps tweak the RPM to find areas of stability to improve things? Also, my choice of finishing paths seems to have left a lot of circular swirls on the front side. I should probably switch to something circular there instead of linear so that the center stud doesn’t cause so much heartache.
Back cavity finish: In this iteration, I didn’t actually do a finish pass on the interior surface of the back cavity. This is a precision surface that the sun gear fits into, so I definitely need to do that and tune it in.
Accuracy: The bearing surfaces’ accuracy is probably best described as “meh”. I tweaked the tool diameter offset until I could fit the bearings on, but the difference between “won’t fit on at all because it binds near the base” and “fits pretty loosely around the whole thing” was not really controllable. There was a moderate taper between the near end of each surface and the far end, despite doing several “spring” passes. I suspect this is just an inherent limitation of the Pocket NC. I believe it only has steps for 0.0002″ in position and isn’t that rigid either, so the tool deflection is pretty measurable. Probably the best I could do would be to run those paths with a smaller stickout tool in the hopes of minimizing deflection based error.
Single run: I did this first part executing each tool path singly with my hand on the estop the whole time. After I get the back cavity bore path working, I’d like to try one with the only intervention being at tool changes.
Wow. This was significantly more involved than I expected, although most of that was due to debugging the tool pull out and the Z axis limit problems. Even still, I spent a good week getting the tool paths programmed and tested. I hope that with practice, I’ll get to where I can turn these around more quickly. Especially since this was the “easy” part I had!