Tag Archives: cnc

moteus servo mk2: Front housing

The front housing is the most complex machined piece in the moteus servo mk2, as it was in the mk1.  It is relatively large and mates with many other components with the associated tight tolerance surfaces.  For mk2, the front housing is even larger in diameter, but otherwise has the same basic features.

front_housing_exploded.png

Manufacturing

Building a prototype of this was a real challenge given the tools I have available to me now.  For mk1, I didn’t even try and just had Xometry build my prototypes, and was lucky enough that the first ones worked.  My only CNC currently is the Pocket NC v2-50, which is just barely big enough to deal with this part, and has no convenient workholding that can be used for the stock.  Also, it has a low material removal rate, such that starting from stock here would be prohibitively time consuming.

Manual preparation

My approach was similar to that of the outer housing, in that I prepared the materials on the Artisan’s Asylum manual machines, then did the remainder of the machining on the Pocket NC.

I started with 4″ diameter round stock cut to 1″ +0/0.125:

dsc_1790

Then, on the mill, I faced the parts to the correct 22mm height:

dsc_1744

Then I drilled a 5/8″ hole close to the center:

dsc_1745

At this point, I switched to the lathe and performed some roughing operations, removing some of the OD and ID to reduce the amount of cutting the Pocket NC needed to do.  These were done with some 3D printed spacers to help align the stock in the lathe’s 4 jaw chuck.

dsc_1767

dsc_1772

dsc_1780

CNC work

Now that the part was roughed out, I first mounted it to the Pocket NC using a machined aluminum plug bolted to a custom 3d printed plate.

dsc_1779

dsc_1785

My first attempt used a 3D printed plug, which just delaminated and failed, thus I re-drilled some more holes for this first prototype offset from the original 8.  This operation threaded the holes on the front side, which are used to secure the piece for the second operation.

In the second operation, a second custom 3d printed fixture is bolted to the newly drilled front holes, and then bolted to a plate that is mounted on the B axis.  This enables the Pocket NC to reach the full back side and around the perimeter.  The bracket needed to be slightly offset from the center of the B-plate, otherwise the mill couldn’t reach all the way around.

dsc_1788

Datron 4mm endmill

This was the first part for which I used a Datron 4mm endmill on the V2-50.  It is definitely a good tool, although it has its shortcomings.  The biggest win is that it can remove material at more than double the rate of anything else I’ve got.  Granted, this isn’t exactly fast, but it is fast for a Pocket NC and makes parts like this front housing even remotely feasible.  It also produces a nicer surface finish, and has less deflection so straight walls are straighter.  For simple geometries I used 47k rpm, 0.25mm optimal load and 4mm stepdown and then slowed those down when dealing with the more complex shapes.

There are some downsides though.  One, it uses a 4mm collet, which negates much of the value in having the convenient tool changing handle.  It takes a longish time to switch collets so I have to arrange toolpaths to do all the 4mm collet things together.  Second, it produces more chips than just about any other tool I’ve used on the Pocket NC.  So much so, that I had to schedule breaks every 45-60 minutes in the program just to clear out chips.  Otherwise the chip tray became too full to use effectively.  For some geometries, such as when clearing pockets, the chips are thrown onto the X ways and require even more frequent clearing, otherwise the mill can’t move to the full X extent as it squishes the chips against the front side of the enclosure.

Machining video

Here’s a video of the third one I made, which used finalized fixtures for all operations.

Fit test

And here’s one of the front housings with all the various things mated in place.

dsc_1835

dsc_1834-1

moteus servo mk2: Outer housing

The outer housing for the moteus servo mk2 is just a precision round tube with some mounting holes drilled peripherally.  Still, manufacturing it was slightly annoying, mostly because of my available machining resources.

outer_housing_cad.png

Manufacturing

I started off with round tube stock with some extra margin on the inside and outside:

dsc_1789

Then I went and used the manual lathe at Artisan’s Asylum to get the correct ID, OD and length:

dsc_1741dsc_1742

At this point, I loaded it into the Pocket NC with Sherline 4 jaw chuck, using a 3d printed bracket to align the assembly with the base of the chuck.

dsc_1761

Now, I could use the B axis as an indexer, and drill and countersink all the holes.

moteus servo mk2: Planet Input

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.

Part description

In the gearbox, this planet input interfaces to a number of different sub-assemblies:

planet_input_exploded

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.

Setup

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.

dsc_1765
Stock

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.

dsc_1722

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.

More pullout

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.

Result

Here’s a video showing the different tool paths for the finished part:

dsc_1762
4x “good enough” planet inputs

Future work

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.

Thread milling on the Pocket NC v2-50

To date I’ve managed to not do any threading on the parts I’ve made on my Pocket NC v2-50.  However, I’m about to do a number that require both M3 and M2.5 threads, so I figured it was time to figure out how to do it.

Online tutorials are kinda all over the place in both how you handle things in the model, and how you program the CAM.  Some assume you model threads as a hole of the major diameter, some as a hole of the minor diameter, although none that I could find used the new Fusion 360 “threaded” hole type, which is what I wanted to use.  That said, using the “threaded” hole type appears to be treated basically as a minor diameter hole with a minor caveat.  You would expect that since Fusion knows the minor and major diameter, the “pitch diameter offset” would be relative to a zero tolerance thread, but in fact it appears to be relative to the minor diameter as if you had modeled a minor diameter hole.  Oh well, I just experimented with increasing pitch diameters until I had threads that fit relatively tight for the two that I cared about, which fortunately can be both made using identical tools, although the M2.5 hole is only on the edge.

M3 M2.5
Hole
Tool Datron 2mm single 5mm flute 0068620G “”
Stickout 14mm “”
Feedrate 400 mm/min “”
RPM 42000 “”
Ramp Angle 2 deg “”
Stock to leave -0.02mm 0.0mm
Top height +1.0mm “”
Bottom height -0.5mm “”
Chamfer
Tool Shars 1/8″ 90 chamfer 416-3509 “”
Stickout 18mm “”
RPM 8500 “”
Chamfer width 0.1mm “”
Chamfer tip offset 0.25mm “”
Thread
Tool Lakeshore Carbide 3-SPTRMLB “”
Stickout 16mm “”
Feedrate 300 mm/min “”
RPM 10000 “”
Pitch 0.5mm 0.45mm
Pitch diameter offset 0.538mm 0.430mm
Stepovers 10 7
Stepover 0.05mm “”
Top height +1.0mm “”

Interestingly, Fusion’s simulation reports that the M2.5 holes have a collision when inserting the threadmill, not on the first couple of insertions, but on the 4th and subsequent ones.  This does appear to occur in real life too, as you can hear slight interference when the tool is inserted.  I don’t fully understand this, as I would expect Fusion’s CAM to just stick the tool down the middle the same way each time.

Results

Here’s a video machining a few M3 and a few M2.5 threads in the same operation, then testing them out.

Revisiting machining the sun gear holder

My very first sun gear holder I machined myself was something of an artistic feat.  Each operation was re-run many times, and as a result the part was largely a one-off.  The final part properties were not really indicative of the final program.  My next step in my learning adventure was to up my Pocket NC game and get to a single reproducible program that would emit a part that I could use, then be able to run it over and over again.

The biggest problem I had in making this happen was pull out problems that manifested intermittently, but persistently.  When machining the part in a single operation, the mill needed to be able to reach all the way to, and slightly past the center of rotation of the B axis of the machine.  With the Z travel of the Pocket NC, that means that you need a stickout of almost 27mm or sometimes even more.  Standard length tools can kind of do that, but they don’t result in much of the shank being in the collet.  All my testing with them resulted in occasional pull out at some point during the hour or two of machining.

I tried getting a Kyocera 2 inch endmill 2 flute end mill, which has a minimum stickout of about 34mm.  To run it without mind numbing chatter required dialing the feeds and speeds so far back that the part would take twice as long to complete.  That hardly seemed worth it.

Next, I stepped back and decided to try a 2 operation approach using the Sherline 4 jaw chuck.  This has the advantage that the part is always kept well within the Z travel of the mill, so that standard length end mills can be used, but the disadvantage that you have to manually flip the part over and try to keep things registered.  I don’t have great, or really any, metrology that would allow me to measure the resulting concentricity errors so I was really trying to avoid using this approach, however, I was kind of at a loss at this point so decided to give it a go.

For this configuration, I used a 1.5″ round stock cut to approximately 1″ long.  The first operation used a Datron 3mm end mill to do nearly everything on the back side, with a final chamfer mill pass to break the edges.  The second operation used a Datron 2mm end mill to do everything there, with the chamfer mill once again to do the countersinks and break edges.

The parts that come off here are usable, and about what I expected to achieve without heroics in terms of final accuracy from a Pocket NC.  All the diameters and dimensions are around at most a thousandth off from what I intended.  The walls aren’t as vertical as I would like, but they are serviceable.

Final part
Final part
dsc_1534
My various experiments, single op in back, multi-op in the front

Granted, I probably won’t be using these parts for much of anything going forward, but it was a great learning experience in making the Pocket NC do what I wanted.  Next in this adventure is probably machining a planet input, which I forsee continuing to use in future iterations of the gearbox.

Improved lighting for Pocket NC

Now that I’m making a lot of videos of machining with my Pocket NC, it was getting annoying setting up lighting for each one.  Thus I rigged up some LED strips in the interior of the enclosure.  Now I can shoot 60fps video any time of the night without having to set up external lighting!  Here’s to hoping a chip doesn’t short it out.

dsc_1488
The strip enters through a small drilled hole
dsc_1489
The power switch is taped to the side

dsc_1490

It lights up!

dsc_1491
Even when the case is closed!

Pocket NC 4 jaw chuck workholding

Workholding on the Pocket NC is still, well, a work in progress for me, and it is for many people.  There aren’t a lot of off the shelf solutions.  The machine does come with a mini-vise, which can hold a surprising amount, but it has some limitations.  For one, it isn’t referenced to the axis of rotation of the B axis.  Another, anything held in it can often be far away from the furthest Z travel available, resulting in the need to use extended reach tooling.

Enter, once again, Ed Kramer @ekramer3 on IG, who came up with a solution consisting of strictly off the shelf parts that results in a 4 jaw chuck being placed about 1.75in off the surface of the B axis plate.  This can hold round stock out to 70mm.

View this post on Instagram

Found a workable mounting solution for the Sherline 4-jaw chuck. Shars ER16 straight shank toolholder has the correct M22x1.5 threads to mate to the hub on the chuck. Time to get busy with some larger stock on the @pocket_nc V2-50. EDIT: For other PNC owners who might be interested in this setup, here are the components I used. From top down: Sherline 4-jaw chuck with ER16 hub (part # 1078). Or part # 1042 if you prefer a 3-jaw chuck. Shars ER16 straight shank collet chuck toolholder (part # 202-1423). Any brand will do, just make sure it is threaded for a M22 x 1.5 collet nut, M19 threads won’t mate with the 4-jaw. All held in a 3/4” ER40 collet using Pocket NC’s ER40 fixture. Your straight shank toolholder may have a different shank diameter so select the correct ER40 collet that fits your particular shank. . #instamachinist #cnc #cncmachining #cncmachinist #cncmilling #cncmill #milling #machinist #digitalfabrication #maker #desktopmachine #desktopmachining #desktopmachinist #pocketnc #pocketncv2 #pocketncv2_50 #fusion360 #makersgonnamake #mindmadewithcnc #mindmade #5axis

A post shared by Edward Kramer (@ekramer3) on

In case Instagram forgets itself, the relevant parts are:

A few pictures of my setup:

dsc_1472

dsc_1473

And here is a short video of it cutting:

Finally, if it is of use to anyone, this is my F360 file containing the fixture.  Bewarned, it is hard-coded to my V2-50’s B-table offset as calibrated by PocketNC.

Improved Pocket NC installation

After having used my PocketNC V2-50 for a while just sitting on top of the air compressor, I decided to try and improve its installation a bit.  For one, when the compressor kicked on or off, it would impart a significant vibration to the whole assembly.  Also, I needed a place to hold stock, tools, and intermediate parts.  Here’s a picture of my new setup.

dsc_1449

The table isn’t particularly rigid, but at least it is now decoupled from the compressor.  The wire shelving below satisfies my storage requirements for now.

Fusion 360 3D adaptive and thin walls

I have been trying to improve the tool paths for the BE8108 gearbox sun gear holder.  The first time, I ended up slowing things down a lot and actually took some of the initial adaptive passes in several iterations as I fixed problems, so it wasn’t clear that any one iteration would be functional from start to finish.

So,  I tried it on a fresh piece of stock, with settings that I thought would resolve the pullout issues I had seen earlier.  Lo and behold, what did I find but more pullout!  It appeared to happen in exactly the same situations as before.  The adaptive clearance would leave a thin sliver of material, then “round it off” very rapidly, resulting in a large chunk of sliver hitting the mill at once.  Increasing the minimum cutting radius and tolerance helped reduce the problems some, but didn’t get rid of them entirely.

Eventually, I managed to find this thread on the Fusion 360 forum where others were having exactly the same issue.  From there, I discovered there is an undocumented parameter, only available in the “Compare and Edit” screen called “Curve in Radius”.  By default, it is calculated based on the tool diameter, but I found that I could add a random fudge factor of approximately 1mm to whatever the calculated version was and boom, the thin slivers were handled in a much more appropriate way and the tool never rolled over them until the sharp point was gone.

I still have more bugs to work out of this toolpath, but at least that’s one down.

 

Machining a sun gear holder on the Pocket NC v2-50

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!

Programming

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.

Setup

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.

20190612_sun_gear_stock_setup.png

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:

20190612_sun_gear_holder_back_rough

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:

adaptive_turnaround

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.

20190612_sun_gear_back_central_rough.png

3: Then I used a 2D face to finish the back most surface:

20190612_sun_gear_back_finish.png

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:

20190612_sun_gear_back_roughing_cavity.png

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.

20190612_sun_gear_mounting_back_finish

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.

20190612_sun_gear_back_bearing

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.

20190612_sun_gear_front_roughing.png

9: Then I used a 2D face to finish the front most surface.  This is both ways and has a 0.5mm stepover.

20190612_sun_gear_front_finish

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.

20190612_sun_gear_front_central_hole_rough.png

11: After that, I used another bore to get the narrower hole in the middle.

20190612_sun_gear_front_central_hole_inner.png

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.

20190612_sun_gear_mounting_front_finish.png

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.

20190612_sun_gear_front_bearing.png

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.

20190612_sun_gear_radial_mounting_holes.png

16: A 3D adaptive removed most of the remaining material in the front central cavity:

20190612_sun_gear_front_central_hole_rough_2mm

17: And a 2D contour removed the final bit of material:

20190612_sun_gear_front_central_hole_finish.png

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.

20190612_sun_gear_outer_rough.png

Chamfer milling

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”:

20190612_sun_gear_front_chamfers

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.

20190612_sun_gear_front_countersinks

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.

20190612_sun_gear_back_chamfers.png

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.

20190612_sun_gear_leave_tab.png

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.

20190612_sun_gear_outer_profile_finish

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.

20190612_sun_gear_thin_tab.png

The final result!

Some pictures of the final part:

dsc_0335-e1560375798649.jpg

dsc_0338

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.

Summary

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!