Tag Archives: pocketnc

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
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.

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


It lights up!

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:



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.


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!


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.


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”:


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!


First aluminum cut on Pocket NC

Now that I made a cut in wax, my next step with the PocketNC was doing basically the same thing but in aluminum.  There is of course less room for error with the harder (but I suppose by no means actually hard) material.  It seems that I managed to use up a bit more luck than I expected, but still not too terribly costly so far.  My “learning moments” errr… goofs, so far:

Ensuring the part is contained within the stock

When I first made the toolpath, I programmed the stock a few mm larger than the actual stock to handle any mis-registration between the vise and the machine origin.  This was a good idea, as I still have about a 2 or 3mm mis-registration in the Y axis that I have yet to resolve.  However, when I did that, I managed to get the actual part about 0.5mm outside the actual stock.  This was easy to fix and for this part geometry, I even kept using the same stock for subsequent runs.

Here’s my very first aluminum chips running the first version:

Inconsistent assumptions between tool paths

As I was developing the tool paths for this part, I started out using a 3D adaptive path to cut away most of the outside material using a 3mm Datron single flute mill.


That was then followed by a series of contour paths or circular paths to finish up each of the outside edges.  However, in one incremental stage I had tweaked that first adaptive clearing to stop at the top edge of the wide flange, but still had a contour that traced it out.  Watching the simulation at high speed, I didn’t notice the problem, but when the resulting contour was run, it plunged the mill straight into unmachined material.

When running this, needless to stay the PocketNC, while tough, was in no way able to pull that off and the spindle stalled.  Fortunately, I was watching and actually got the machine safed before the spindle had completely stopped.  My camera had shut off before that point though, so I got no footage.

Switching tools

Next, I wanted to use a second longer reach tool to handle the central cavity, which goes relatively deep.  I dutifully entered the tool geometry into Fusion 360, including the fact that it was a 3 flute mill, but then managed to neglect to even look at what the chip load was and left all the feeds and speeds the same as for the 3mm single flute Datron.

Watching this live, it certainly sounded bad when it was doing the helical ramp in, but I chalked it up to chatter with the longer reach tool.  However, as soon as it started the adaptive clearing inside, it sounded much worse, but seemed to be making forward progress.  However, on the second plunge and adaptive clear, it managed to completely stall out the spindle.  I jogged the Z axis back out, fixed the feed rate, but when I spun up the spindle again, boom.  That was the end of that end-mill.

3rd (or 4th time) is the charm?

At this point, I reworked this first program to do what I could with the 3mm Datron end mill, which just meant I didn’t go all the way deep into the central cavity.  This completed all the way through with no big problems.  The last contour I did on the internal cavity also removed 0.001″ of material axially.  When that first plunged in, it did sound terrible, but only for a fraction of a second.  Still,  I probably wouldn’t do it again that way.

After all that I had this first half-part done.


The tolerances on the surfaces actually seemed to be nearly identical to the wax version, in that it was plus or minus a thousandth.  This was without any actual work to get the size I wanted, so is more of a baseline.  Presumably I can use tool width compensation or just tweak the contouring paths by a thousandth to get it where it needs to be.  That said, it was close enough out of the box that my bearing kinda fits on.


Future versions of this part

Not too long into programming this first part, I realized that with slightly different stock, I can do the entire part in a single setup with a breakaway tab by orienting the part off by 90 degrees.  That’s what I’ll try next.

Lessons learned

I guess these lessons are what I’m trying to get out of these exercises, and while they are certainly obvious to anyone who actually knows machining and CNC, I’ll write them out here as much for my reference as anything.

  • Watch at least the beginning of each tool path in simulation at real-time speed
  • Actually look at the computed chip load when configuring a new tool
  • Don’t rely on contour paths to remove any axial material
  • When it sounds bad, stop and rethink!
  • Run everything on the machine at 30 or 40% speed at least until nothing new happens before upping it to full speed

That said, I’m not trying to create a production environment here.  I’d like to be able to quickly turn my CAD models into tool paths and get parts made, and as long as the machining time is the same order of magnitude as the programming time I’ll be happy.    I am OK with breaking things now and then in service of that goal, so I don’t need to double and triple check of tool paths.

Finally, I want to thank Ed Kramer https://www.instagram.com/ekramer3/ for posting his results with the Pocket NC V2-50.  All the mistakes here were mine, but he has provided a wealth of information on what feeds and speeds are possible in a range of materials with this machine.

Quiet(er) air compressor for Pocket NC

Now that I have a PocketNC, the first thing I noticed was that I had a problem with noise volume.  The air compressor Pocket NC recommends is described as “quiet and durable”.  I can maybe believe the durable part, but quiet I have a harder time believing.

Grainger Compressor

I’m running the machine in my home office and I measured the compressor at upwards of 85dB.  That’s about the same as a bulldozer.  Despite me adding some vibration damping padding, it also did a pretty good job shaking the whole house when in operation.

Since there is no real point in having a mill I can’t run because its air accessory is too loud, I replaced it with a “quiet” compressor from California Air Tools — the 8010SPC.  Granted, no compressor is going to be silent, but this does a pretty good job.  In the office it is totally manageable.  If you close the office door, it is barely audible outside in the rest of the house.


While only about twice the cost of the Grainger unit, the bigger downside is its size and weight.  Clocking in at around 120lb, it is a beast.  Amazon reviews were nothing but shipping damage, so I had mine delivered to the local Home Depot at which it arrived seemingly unharmed, although with somewhat unorthodox packaging.  There was just a 5 sided box dropped on top of it, with the bottom caster wheels exposed out the bottom.

The next steps here are to build a table that the compressor can sit under, and the Pocket NC can sit on top of.  While running, the compressor is relatively vibration free, but it makes a pretty big kick every time it shuts off and a minor kick when it turns on.  It doesn’t seem to bother the Pocket NC that much, but it probably isn’t a good thing generally.


Pocket NC Raspberry Pi Wifi Bridge

The primary UI the Pocket NC presents is a web interface accessible over a virtual USB based ethernet port.  I wanted to be able to run mine not immediately near an ethernet jack, but also didn’t want to have to tote a laptop over every time to check on it.  I had plenty of raspberry pi’s lying around, so rigged one up as a wifi bridge.

First, I found a random case to print from thingiverse, the TurboPi:


Then I gave it a fixed IP address on my wifi network and set up IP forwarding with NAT.

iptables -A POSTROUTING -o eth1 -j MASQUERADE

Then, I saved that config:

iptables-save > /etc/iptables.ipv4.nat

And restored them in /etc/rc.local

iptables-restore < /etc/iptables.ipv4.nat

Finally, I enabled forwarding in /etc/sysctl.conf


Finally, I added a route on my desktop with the raspberry pi’s address as the gateway.  Now I can transparently access the PocketNC from anywhere!

Raspberry Pi forwarding network traffic to the Pocket NC

New machine day – Pocket NC

With my efforts to build a gearbox transmission and subsequent plans for a quadruped, there are a lot of parts which just can’t be made effectively from 3d printed plastic.  To date, I’ve sent out a few parts of the gearbox to CNC shops, which while effective, has a relatively slow turn around.  The best you can get without paying an arm and a leg is something like a week turnaround.  One thing I’ve learned from having a 3d printer on site is how transformative it is to be able to have single day turnaround for parts.  Thus, I thought I would experiment with CNC machining on a small scale locally and recently acquired a PocketNC V2-50.



Since this is the V2-50 version, it has a 50,000 rpm spindle, theoretically giving it at least passable material removal rates in aluminum.  Most of my gearbox parts look like they could be machined in an hour or so.

To date, all I’ve done is machine half of a sun gear holder out of the wax stock that ships with the mill.   I took it plenty slow and consider it a success that I managed not to break anything on the first try.

The result is approximately a thousandth off from what I was aiming for on the two critical dimensions I tested, although that probably doesn’t mean much since it was just wax.  It remains to be seen what I can achieve in aluminum.


Now I actually need to get the tools and fixturing that will let me machine the other half.