Hooray, new stuff! The STM32 symbol is a reasonable size now! We have
a sym-lib-table! Everything is great, and I'm excited!
The board's a bit of a mess though, as the silkscreen needs to be laid
out nicely. Oh well, details.
More test points will be needed for automated testing, so I've added the
first two I know of.
With firmware version 1.2.0+, there's not much reason to install SW1
anymore. This commit replaces it with R11, an unpopulated resistor
footprint that does the same thing as bridging the two pins of SW1 used
to do, just in case an upgrade make the `boot` command stop working.
More vias near Q2, one via removed near J2 to make the VBUS plane have
more effective width.
The "PD Buddy Sink v1.0" text has been moved to once again be entirely
over copper.
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.
Made mounting holes have solid connection to zones
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.
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.
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.
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 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.
