Tag Archives: pocketnc

moteus servo mk2: Reducing weight

After having produced the first functional demonstration of the moteus servo mk2, my next step was to decrease the weight.  While I was at it, I made two other changes:

  • Axial connections: I switched to a design with entirely axial connectors, which removes the need for 4th axis machining when producing the parts.
  • Planet Input Bearing: I switched the planet input bearing to be inserted from the rotor side.  This way, the bearing is captured between the planet input and the rotor, rather than between the planet input and the gears.  That also improves the ability to assemble and disassemble the unit.

moteus_mk2_reduced_weight_2

Slimming down the housings drops around 100g from the total weight.  I may still try to take out some weight from the planet input and output, but they don’t weigh much to begin with so the potential gains there are small.

Next up I’ll manufacture and assemble this, then get it running.

 

Update on Pocket NC v2-50 Threadmilling

After machining a fair number of parts with threads, I’ve tweaked my thread milling feeds and speeds to both go a little bit faster, give a more reasonable fit, and remove the last bit of niggling interference with the M2.5 recipe.

I’ll list the changes here, and have updated the original recipe

Old New
Chamfer Width 0.10mm 0.05mm
M3 Pitch Diameter Offset 0.538mm 0.568mm
M3 Stepovers 10 6
M3 Repeat Passes NO YES
M3 Lead To Center NO YES
M2.5 Pitch Diameter Offset 0.430mm 0.480mm
M2.5 Stock to Leave 0.0mm -0.02mm
M2.5 Stepovers 7 4
M2.5 Repeat Passes NO YES
M2.5 Lead To Center NO YES

Notably, the “Lead To Center” option found on the linking tab is what prevents the M2.5 threads from rubbing when inserting in later passes.  Thanks to Quincy Jones from Implemented Robotics for that tip over in the mjbots discord!

 

moteus servo mk2: Back housing

The back housing is the final piece of the moteus mk2 servo that I wanted to prototype.  (The planet output is identical to the mk1, so I could use extra stock I had of it for the prototypes).  It is large, and only mates directly to 4 other things, which makes it a little less complex than the front housing.

back_housing_exploded1.png

back_housing_exploded2.png

Design

I had initially designed the back housing to mate to the as-yet-unannounced new version of the moteus controller, the r4.x series.  Unfortunately, I don’t have any of those working yet, so I tweaked the design to temporarily fit a r3.1 controller, which looks like this:

back_housing_exploded_r31.png

It mates to the rotor bearing in the center, the outer housing around the perimeter, provides support, mounting and heatsinking to the controller, and provides a mounting interface for the controller cover.

The only design intent change I made in the mk2 version here was to decouple the outer housing interface axially from the rotor bearing interface.  In mk1, the back housing was a flat plate.  Now in mk2, it is a very shallow cone, to slightly reduce the axial length of the large diameter outer housing and eventually make it possible to reduce the weight more because of it.

Manufacturing

Like the front housing, this was challenging to produce on the Pocket NC.  It required even more steps than the front housing, since it had no final flat surface which also had threaded holes.  Thus I ended up using a manual machining stage, followed by 3 operations on the Pocket NC.

Manual machining

The manual machining merely took 4in round stock that was rough cut to 5/8″ and faced it to approximately 15mm, then drilled a center 1/2″ hole.

dsc_1846

Operation 1

For the first Pocket NC operation, I used a 3d printed bracket to clamp the stock down, and then the four M2.5 holes used to secure the back cover were drilled and threaded.  These will be used in the next operation.

dsc_1827

Operation 2

In operation 2, those holes were used to bolt the stock to another 3d printed fixture, which was then bolted to the same 3d printed assembly as used in operation 1 (and for the front housing).

dsc_1833

Operation 3

The final step of operation 2 drilled and threaded 4x M3 holes on the back surface purely for fixturing purposes.  They are used to bolt the in-progress work to yet another fixture, so that the rest of the back can be machined.

dsc_1836

Video

Here’s a video showing all the machining steps:

 

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

UPDATE 2019-11-27: The feeds and speeds have been tweaked based on further experimentation.

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 “”
Top height +1.0mm “”
Bottom height -0.5mm “”
Chamfer
Tool Shars 1/8″ 90 chamfer 416-3509 “”
Stickout 18mm “”
RPM 8500 “”
Chamfer width 0.05mm “”
Chamfer tip offset 0.5mm “”
Thread
Tool Lakeshore Carbide 3-SPTRMLB “”
Stickout 16mm “”
Feedrate 300 mm/min “”
RPM 10000 “”
Pitch 0.5mm 0.45mm
Pitch diameter offset 0.568mm 0.480mm
Stepovers 6 4
Stepover 0.05mm “”
Repeat Passes YES “”
Lead To Center YES “”
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.