My previous blog posts talked about diode-free keyboard designs using topology, and specifically using a partial Tutte-Coxeter graph for keyboards with 30~42 keys. As hinted at, I spent June making my own no-diode topology-based 36-key ergonomic keyboard PCB design using the Open Source tools Ergogen and KiCad. This is designed as an alternative PCB to fit the existing Gamma Omega keyboard's 3D printed case design (case design or modification can be a future project).
Erogegen v4.1.0
This tool lets you describe an ergonomic keyboard layout and easily adjust the splay and stagger to suit your taste or hands - and can handle mirrored designs as easily as split designs. In this case I was starting from an existing split PCB design (two reversible 18-key boards) and turning it into a single larger mirrored 36-key board, but Flat Foot Fox'n blog post "Let's Design A Keyboard With Ergogen v4" series was incredibly helpful.
I changed the choc-switch footprint settings (the original design used reversible footprints) to single-sided, which is simpler. Mine will be hot-swapped, but the footprint makes it easy to allow attaching the switches either with hot-swap sockets (in the "North" orientation), or directly soldered (rotated 180 degrees in the "South" orientation - this would need changes to the original bottom case though). The direct solder sockets act as vias (conductive holes through the board) making adding the traces (electrical wiring) a little easier. This was an idea copied from the Old Man's "The End Game" keyboard PCB.
The existing case design assumed a particular USB-C variant of the Raspberry Pi Pico micro-controller, with a hole in the bottom plate to access the boot button (for re-flashing the firmware), so I have assumed the same. This now needs a matching hole in the PCB, and a cutout to give enough room for the USB-C socket.
The original two-PCB design only needed a header footprint for half the controller. With a full board we need a full micro-controller footprint. I used the proposed Raspberry Pi Pico footprint on this Ergogen pull request. I guess smaller controllers with support built into Ergogen are more popular, but the fact the larger RP Pico controllers expose at least 26 GPIO pins is precisely why I want to use them.
Currently Ergogen (as of v4.1.0) doesn't let you define silk-screen art (images, lines, circles, arcs), or even text. I spotted how the author of the Caldera keyboard added text using a custom Ergogen footprint. I took this one step further to define my own line-art as a Ergogen silk-screen footprint for the partial Tutte-Coxeter graph (since drawing this by hand in KiCad is very fiddly). This was generated in Python, but could in principle be done directly in JS with the same logic (some simple loops and geometry).
KiCad v9.0.2
The main output from running Ergogen v4.1.0 is a KiCad v8 PCB file, which the current version KiCad v9.0.2 can open fine. I then had to layout the wiring for my traces, and used Flat Foot Fox's blog post "Let's Design A Keyboard With Ergogen v4" finale which was incredibly helpful.
 |
| Un-wired TC36k keyboard PCB from Ergogen opened in KiCad v9.0.2 |
The scanning-columns were assigned to the physical columns as in my previous blog post, and done on the underside (along with the hotswap sockets). This time I added some of the row-scanning traces here too. The rest are on the top side - and due to the stagger and small margin of the PCB where it hugs the top ring and middle finger keys, I could not run traces there - so the final pin assignment and wiring needed redoing.
For my traces I tried to follow the local key footprint orientation - which due to the splay between the columns for each finger meant a lot of rotation - and all to frequent discovery that the latest edits had left the traces on the other side out of place. I recommend stopping to run the board checks ("Design Rules Checker") and saving a separate new version frequently. Sadly although the KiCad PCB file is plain text, it does not play nicely with version control - all those board rotations result in floating-point number noise.
This design only has a wiring matrix on the board, so the power and ground pins are unused. To satisfy the wiring net checks, I added traces to connect all the controllers ground pins to each other. Then, while I probably didn't need to, I used this example with a ground plane to add one anyway. This meant tweaking my trace placement in lots of places to leave enough space for a "ghost trace" from the automatically filled ground plane. I got the vast majority of the board covered on both sides without any extra vias.
 |
| TC36k keyboard PCB in KiCad v9.0.2 |
For the final steps I actually copy-and-pasted the traces from a working copy to a fresh clean output from Ergogen. This just left the fairly easy challenge of dropping it all in the right place - and fine tuning a couple of traces which ended up ever so slightly too close to a hole etc.
QMK Firmware
This is a wired USB keyboard, so QMK was the natural firmware to try - although complicated by ongoing changes to how the main repository is organized. Most custom keyboard designs are seemingly created in forks of the main QMK firmware repository. I looked at this but couldn't get all the dependencies installed on macOS. Instead, I'm using their QMK Userspace approach with GitHub Actions to build the firmware (with a preparation_command trick as this is a custom keyboard). All that was the hard bit.
The actual core of my partial Tutte-Coxeter 36 key firmware is very simple - one keyboard.json file listing the 13 GPIO pins for my scanning columns, the 13 GPIO pins for the scanning rows, and the 36 keys as positions in the sparse 13 by 13 scanning matrix following the existing LAYOUT_split_3x5_3 ordering (shown here as Qwerty with L1, L2, L3, R3, R2, and R1 for the thumbs):
| GP11 | GP10 | GP3 | GP4 | GP7 | GP26 | GP27 | GP28 | GP15 | GP21 | GP19 | GP20 | GP16 | |
|---|---|---|---|---|---|---|---|---|---|---|---|---|---|
| GP12 | Z | J | |||||||||||
| GP8 | Q | S | ; | ||||||||||
| GP9 | X | C | |||||||||||
| GP1 | D | R | O | ||||||||||
| GP6 | V | G | |||||||||||
| GP2 | W | T | Y | ||||||||||
| GP22 | H | M | R3 | ||||||||||
| GP0 | E | U | I | ||||||||||
| GP13 | B | K | L2 | ||||||||||
| GP14 | A | L1 | L | ||||||||||
| GP18 | N | . | R2 | ||||||||||
| GP17 | , | R1 | / | ||||||||||
| GP5 | F | P | L3 |
In hindsight I should have tried harder to have Q top left, as by convention the key at that matrix position is used in QMK for reset on startup.
Making a Vial compatible firmware was also fairly easy - I wanted this as Vial makes tinkering with a layout without re-flashing really easy. And I managed to build Miyoku QMK firmware for my keyboard too, since I followed the LAYOUT_split_3x5_3 community standard.
Assembly Production Files
I decided fairly early on that I would try JLC PLC to fabricate my PCB (minimum order of five), and also solder on all of the hotswap sockets with their assembly service. That would leave me with just the controller daughter board to solder in before adding the switches and case (which JLC PCL can 3D print for me too).
PCB fabrication needs Gerber format files which are easily exported from KiCad. For assembly you also need a "Bill of Materials" (BOM) table with part numbers (fairly easy here with just 36 of the hotswap sockets), and a Component Placement List (CPL), also known as a Centroid, Pick and place, or position file. That lists the exact position for each part, including the rotation - not something to attempt manually!
I installed Benny Megidish's JLCPLC Fabrication Toolkit which does all that (currently version 5.1.0), but needs the part numbers first. For that, I installed Bouni's Kicad JLCPBC Tools plugin (currently version 2025.04.02), and clicked the icon in KiCad. This found three different "components" from the footprints on the board:
- RPi_Pico_SMD_TH - The Raspberry Pi Pico controller, not asking for this in the assembly, so turn off BOM and POS for this.
- mounting_hole_plated - The case screw points, again turn off BOM and POS as nothing to assemble here
- switch_choc_v1_v2 - The low-profile choc switch footprints - these must have BOM and POS ticked. Double click and search for part number CPG135001S30, which gave two Kailh options - neither in stock:
- LCSC part C9900009224, significantly cheaper: Pre-order Items Pricing, Estimated unit price: $0.0006 - I wanted to pick this, but it shows as unavailable with only consignment was offered (i.e. buy elsewhere and send it to JLCPLC).
- LCSC part C5333465, much more expensive, one in stock: Pre-order Items Pricing, Estimated unit price: $0.1029 - I could pre-order this, but a working day later, bad news: "We are sorry to inform you that the below parts are out of stock and unable to get quotation".
So, no assembly with the hotswap sockets. Nor were any choc-switches in stock or available to pre-order (since they can alternatively be directly soldered with this design, and could be used with the assembly service).
Back in KiCad, I saved the hot swap part assignments anyway. And then clicked the JLCPLC Fabrication Toolkit icon, left the defaults, and clicked generate. That made a production/ sub-folder with five files (and a sub-folder of backup PCB files):
- gamma-omega-tc36k_v1.0.0.zip - the Gerber files to fabricate my PCB, including drill files
- bom.csv - the Bill of Materials (BOM)
- positions.csv - the Component Placement List (CPL)
- designators.csv - list of footprint identifiers used
- netlist.ipc - IPC netlist file
I think we just need the first three to order an assembled board at JLCPCB, but just the Gerbers ZIP file for the board alone. The PCB production files are in the repository.
PCB Fabrication
I logged into JCLPLC, and uploaded gamma-omega-tc36k_v1.0.0.zip - this was correctly recognized as a 2-layer board, about 23.3cm by 11.1cm. I look the defaults except the black finish (with white silk-screen art), lead free HASL finish, and removed the order number from the board - cropped screenshot at the top of the post.
I tried toggling assembly on, defaults except I ticked "Confirm Parts Placement". Clicked next, uploaded the BOM and positions CSV files, but then was stuck on the parts shortfall. So no assembly service for me (see above).
The five boards were only USD $16.50. I opted for the cheaper slower shipping, and added the 3D printed Gamma Omega keyboard case in SLA resin, and KLP Lamé Choc Saddle keycaps too:
- Gamma Omega case top in JLC Black resin at $17.64 x1
- Gamma Omega case bottom in Grey resin at $10.24 x1
- KLP Lamé Choc Saddle Part 1 in JLC Black resin at $1.10 x2
- KLP Lamé Choc Saddle Part 2 in JLC Black resin at $1.45 x2
My JLCPCB order total to the UK:
Merchandise Total: $49.46
Shipping Charge: $12.24
Customs duties & taxes: $12.34
Order Total: $74.04
I'm waiting on the PCB confirmation email, and still need to order a set of choc v1 switches, hot-swap sockets, and controller(s).
