D1 is now a B140, which is a MacroFab house part.  It's actually a bit
more expensive from distributors than the SS14FL, but the lack of a
labor charge makes it quite a bit cheaper for PCBA.  It's also larger,
so in order to fit the new part, I moved it between Q2 and J1.  This is
possible because…

Q2 is now a DMP3017SFG.  This is a cheaper, smaller, and less
over-specified MOSFET which should be fine for the job of controlling
the PD Buddy Sink's output.  It uses a proprietary Diodes Inc. package
whose footprint I contributed to KiCad's library.  Because the new
MOSFET is so much smaller than the old one, I was able to fit it close
to the board edge where R9 used to be.

The whole output circuit has been rearranged, and I like its layout a
lot more now.  Also, the new position of D1 allowed me to move a bunch
of reference designators closer to their footprints, which is nice.

The components on the bottom, SW1 and P1, were using slightly modified
footprints from the KiCad library (default, but with no paste on any
pads) in v0.3.  Now they're back to the default footprints, but with
local paste clearance set to -100% to make sure there's no paste on any
of their pads.

There's not really any reason for mounting holes to have thermal relief,
since they don't normally get soldered.  Removing the thermal relief may
make them resist tearing more, too.

It used to be an MMBT2222, now it's an MMBT3904.  The new transistor is
slightly lower-spec'd, but is still more than plenty for this
application.  Also, it's a MacroFab house part, so the boards will be
even cheaper to manufacture.

Now signal vias are MacroFab's minimum size, and power vias have a
slightly smaller drill than before to not be slightly pushing
MacroFab's design rules.

Now that my pull request for the AP2204 regulators has been merged, I
can finally update the PD Buddy Sink schematic to use it.

U2 was moved to remove ambiguity.  Q1 was moved to ensure it isn't cut
off by a hole.  U1 was moved to stay away from where MacroFab put their
secret manufacturing code.

In the previous board version, there was a trace (OUT_CTRL) between the
Boot switch's pins 2 and 3.  Since those two pins are the ones that
need to be shorted to enter DFU mode, it's possible that users wanting
to upgrade the device's firmware would want to short them with a blob
of solder rather than buying a switch.  While the soldermask *should*
prevent this solder blob from shorting the OUT_CTRL line high,
soldermask can be accidentally scraped off, so I don't want to rely on
it in this case.

This commit moves the OUT_CTRL trace out from between SW1 pins 2 and 3,
and adds a keepout zone between those two pins.  This should make it
much safer to bridge those pins with a blob of solder.

Assuming I'm going to keep ordering boards from MacroFab, it makes sense
to use their house parts as much as possible.  Therefore, the next
boards will use a C&K PTS810 as the Setup switch instead of an Alps
SKQG.  In addition to saving money, this change allows room for larger
"Setup" and "GND" labels.

By removing clearance around the printed piece, I was able to shrink the
board to 95.6% of the area it had before.  That'll save me a few cents.

MacroFab wants oval drills to be marked on the board edge layer, so
that's what I'm doing.  Hopefully they'll be able to handle oval drills
better soon, given a recent comment on their blog.

My USB Type-C connectors were merged into the KiCad
Connectors_USB.pretty footprint library, so I can use it from the normal
library now.

The power lines had been drawn as regular wires with net labels.  That's
not great, so I changed them to use power symbols.  It's better now!

With the VBUS symbol merged into the KiCad library, I no longer need to
use my own.  This commit changes the schematic to use the standard VBUS
symbol rather than a custom one.

The footprints have been updated to be used with the mainline KiCad
schematic symbol, so the symbols in the pd-buddy library were useless.
They were also overall a lot worse, and furthermore, they were unused.
This commit removes the old USB connector schematic symbols from the
pd-buddy library.

The SOT-89 footprint changed its name slightly in the KiCad library,
so the voltage regulator has been updated accordingly.  It has a nice
new 3D model too.  It's not weird and blue anymore.  I like it.

The SOD-123 was also updated to have a 3D model.  The board now only
lacks models for the footprints I made myself.  Heh.

That library is getting less important though, thankfully.  Still, while
it has symbols we need, it should be accessible.

It's a small board, just a bit bigger than a PD Buddy Sink v0.1.
Nothing unexpected, just pogo pins and connectors and two resistors
because it has a USB Type-C receptacle for power input.  The plastic
piece screws on and the whole thing should work just great, making the
SWD header unnecessary on the v0.3 PCBs.  It's even compatible with the
boot switch, and with a 2-pin 0.1 in. male header on the bottom as an
output connector.

In preparation for adding a second board (the programming jig) to this
repository, I've moved the PD Buddy Sink files to their own directory.

Now they're MM3Z5V6T1G, an SOD-323 5.6 V 300 mW Zener diode.  Similar to
the old part, but easier to solder and cheaper.  One of those two points
matters.

KiCad has the right footprint now, so I don't have to substitute an
SOD-323 footprint.  The 3D model looks less inaccurate I suppose, but
still not right for the particular diodes I'm using.

The footprints haven't been merged yet, but the symbol has.  Therefore,
I updated the footprint in the pd-buddy library to match the new symbol
(changed shield pin number to S1) and changed the schematic to have the
new connector symbol.  The board looks the same except that a couple
references changed.

Now that the appropriate pull requests have been merged, I can use the
standard part rather than the one I created in this repository.
Speaking of which, this commit removes FUSB302B and MLP-14 from this
repository.

Set the _KI_LIB_GIT path to point to a local copy of the kicad-library
Git repository.  Then this project will pick up the Git libraries
instead of the system ones.

It'll make the LED a bit brighter, and it's a more common value.

Now the board is within spec for MacroFab.  Also, the power traces at
the USB connector are thicker, so should be able to carry high currents
more easily.

2 oz copper is no longer needed, and neither is a thin board.

This is a major change!  Almost all the components have changed to
smaller versions, with 0603 and 0402 passives and a QFN microcontroller.
The board now has four layers, with internal layers used for VBUS and
GND.  The board now measures a mere 25×30 mm!  The SWD header and Boot
switch footprints have been moved to the bottom to help with this
shrinkage.  Two test points were added to the bottom as well to make it
possible to power the board without using the USB connector.  The
mounting holes are now slightly smaller (better sized for M3), and only
17 mm apart instead of the old 18 mm.

To sum up, everything is smaller and that's almost entirely a good
thing, except now it's not really possible to build one by hand.

As it was, it wasted around 85 mW whenever the output was turned on at
20 V.  That's a silly waste of power.  A 100 kΩ pullup works just fine,
so I changed it.  Now there's only 4 mW wasted, so I'm happy.

There's now quite a bit of stuff located under the USB connector.  A lot
of manufacturers mark that area as a keep-out zone, but luckily,
Amphenol is not one of them.

It's a USB Type-C connector just like the one used in v0.1 and v0.2, but
with only SMT pins (except the fixing pins, of course).  They're
slightly cheaper and probably nicer for automated assembly, but
impossible to hand-solder.  That's okay though: where we're going, we
don't need hand-solderability.

That's the name they should have, since the board hasn't been called PD
Buddy since v0.1.

The traces to the thermal vias for U1 shouldn't have been as small as
they were.  Not that U1 gets particularly hot, but it would just be
nicer to use thick traces to extend to the thermal vias.

The edge of the power output connector no longer overhangs the edge.
Now only the USB connector does, and it really should.

The slider for the Boot switch is no longer overhanging the board edge.
This is nice for designing enclosures, as now nothing overhangs the long
sides of the board.

I don't know how that mounting hole got mispositioned, but it was.

Now the board should be much happier carrying 5 A, possibly even with
1 oz copper.  I'd still prefer to get it made with 2 oz copper as a
matter of principle, but IPC-2152 calculations make it look like I'd
probably be okay with 1 oz.