GitHub - iandchasse/silkscreen-pcb: Silkscreen: open-hardware ESP32-S3 e-paper reader mainboard (KiCad 9). Formerly the de-link hub.

An open-source, open-hardware e-reader mainboard.

Silkscreen is a build-it-yourself e-reader. The name covers both this board and a reader built around it; this repository covers the mainboard. You order the board already assembled from a factory, add an e-paper display, a battery and a microSD card, and put it in a case of your own choosing. It is a 2-layer ESP32-S3 board with a 24-pin display connector, optional touch and frontlight, microSD and single-cell Li-ion/LiPo power.

It is the successor to de-link. This repository was the de-link project hub until September 2026; the hub's pages and photos are kept on the de-link-old branch. I designed Silkscreen in KiCad 9.0.6, but you do not need KiCad to order a board. Every file a factory asks for is already in the production/ folder of this repository, ready to upload.

Back (all components)	Front (silkscreen art)

What it is

• Brain: an ESP32-S3 module with 16 MB of flash and 8 MB of PSRAM, with USB built in. You plug a USB-C cable straight into it, no adapter.
• Screen: a 24-pin connector for SPI e-paper panels. The primary target is Good Display's 4.26" panel family, in plain, touch, frontlight, or touch + frontlight versions. The plain panel is sold as GDEY0426T82; the others are GDEQ0426T82 with a suffix for the variant (-T01C touch, -FL01C front light, -FT01C both), so always order by the full part number.
• Power: charges and runs from a single-cell Li-ion/LiPo pack over USB-C, with charger, cell protection and a 3.3 V regulator on board.
• Storage: a push-push microSD socket.
• Buttons: eight page/navigation buttons, plus power and reset.
• Size: 60.05 × 111.30 mm, 1.6 mm thick. Every part is soldered onto the back face, so the front is clear for the display.

Silkscreen is built to run the open firmware made for Xteink's readers, starting with CrossPoint. Setting them up for this board is closed-beta work, so there is no firmware release for it yet. Read Firmware before you order.

The complete picture of the project, the story behind it, the cost breakdown and the build configurator are on the project website. As of 21 September 2026 the website is still locked while I wait for the first boards. It opens, and this README links to it, as soon as I have tested a board in my hands.

Everything about how the board works, pin by pin, is in one document: docs/HARDWARE.md. It covers every circuit block, the GPIO map, what firmware has to do for the hardware, and the dimensions a case needs.

What you need besides the board

The factory sends you a populated circuit board and nothing else. You also need:

Battery lead order. On the board, J5 pin 1 is battery negative and pin 2 is battery positive, and the board prints - + with the word CHECK right beside the connector's mouth. A pack's wire colours are a good guide (black is negative, red is positive), but there is no industry standard for which side of a JST-PH plug each wire goes in: packs ship both ways round, and the two look identical in a photo. So before you plug a pack in, with USB unplugged, check that its black wire lines up with the - mark and its red wire with the +. If they are the wrong way round, swap the two wires in the plug (how to reverse a JST battery plug). A multimeter is the surest check.

Screws and case are not on this list. The board has six M2 mounting holes, but which screws you need depends on the case you use, and no case is supplied here. See The board and your case.

Order an assembled board, step by step

You do not need KiCad and you do not need to know how a PCB is designed. A factory makes the board and solders every part onto it. You will be clicking through a web shop and uploading three files that are already in this repository. Unfamiliar words are defined in Words used on the factory's website.

Or let the builder make the files. The Build one page on the website walks you through the panel variant and the optional blocks, estimates what the result costs, and gives you the three upload files for exactly that build: the same Gerber zip, plus a BOM and CPL with the parts you left off already removed (see Choosing a configuration). For the standard build they are byte-for-byte the files in production/. The website is not open yet, and the steps below are the same either way.

What it costs and how long it takes

The minimum order is 5 bare boards, and you choose how many of them the factory assembles: as few as 2, all 5, or more boards if you want them. Most of the bill is one-off (the bare boards, setup, the solder stencil, and a small loading fee for each of about two dozen "Extended" part types the factory has to fetch), so the price per assembled board falls quickly as you build more. The website's cost page breaks the cost down by order size and explains where each fee comes from.

For scale, my own order on 21 September 2026 (no coupons, US delivery): five boards with two assembled came to $223.95 for boards, parts and assembly, and $305.23 at checkout once shipping, US tariffs and tax were added. That is about $150 per working board at two, and the cost page puts the same build at roughly $77 per board with all five assembled and about $50 at ten. Prices, shipping and import charges move, so treat every figure as an expectation, not a promise.

Step 1: get the three files

Download this repository (green Code button, then Download ZIP) and unzip it. Everything you need is in the production/ folder. You upload exactly three files:

Ignore everything else in that folder. These three belong together and come from the same export. Do not mix one of them with an older copy of another.

Step 2: order the bare board

1. Sign in at jlcpcb.com, click Order now, then Add Gerber file and choose Silkscreen_Reader_PCB_1.0.zip.
2. The viewer draws the board. Confirm it says 2 layers and about 60 × 111 mm. If it does not, you uploaded the wrong file.
3. Set PCB Qty = 5, Thickness = 1.6 mm, Outer Copper Weight = 1 oz. Surface finish and solder-mask colour are your choice; nothing in this design needs a particular one.
4. Leave everything else at its default.
5. Scroll the viewer to the board edges and check the USB-C cut-out, the microSD opening and the two narrow slots on the outline are open, not filled. The long one (47.04 × 1.30 mm) is the display-flex slot; the short one at the tongue neck is 5.30 × 1.10 mm. Both are at or above JLCPCB's 1.0 mm minimum routed-slot width, so neither should raise a design-for-manufacture (DFM) message. (Earlier revisions had four 0.5 mm perforation slots there; those are gone.)

Step 3: turn on assembly

PCBA means "printed circuit board assembly": the factory buys the parts and solders them on for you, instead of shipping you a bare board.

1. Switch PCB Assembly on.
2. Choose Standard, not Economic. JLCPCB runs two assembly services, and the ESP32-S3 module this board is built around can only be placed on Standard, so for a complete board Standard is the one you need. (If you are happy to hand-solder the module yourself, you could leave it off the order and use the cheaper Economic service for everything else. That is an experienced builder's choice, not the path I recommend.)
3. Because this board is 60 mm wide and Standard's conveyor wants at least 70 mm, the factory may add snap-off edge rails: narrow strips of extra board material along the edges for the machine to grip. There is nothing for you to design. Expect a small fee in the quote, and snap the rails off when the boards arrive.
4. Set Assembly side: Bottom. Every part on this board is on the back. If you leave this on Top you will receive blank boards and a bag of parts.
5. Set the assembly quantity to the number of boards you want built, from 2 up to the number of bare boards in the order.
6. Leave Tooling holes on Added by JLCPCB.
7. Set Confirm Parts Placement to Yes. It costs a small fee and is worth it on a first order: it lets you look at a picture of where each part will go before the machine runs.
8. Click Confirm, then Next.

Step 4: upload the parts list

1. Add BOM file: production/jlc_bom.csv
2. Add CPL file: production/positions.csv
3. Click Process BOM & CPL.

Step 5: check the parts the factory picked

You get a table with one row per part. Most rows will already be matched.

• Rows with a blank part number are meant to be blank. Eleven references (TP3 TP4 TP5, R43 R45 R58 R66 R72 R74, SW6 and U14, the alternate clock chip; the board uses U13) are tagged "DNP (standard build)". DNP means "do not populate": a spot on the board deliberately left empty. Leave them unselected.
• Every other row must show a match. If a row says No Parts Selected or out of stock, or shows a manufacturer's part number instead of an LCSC code (the C… number that identifies a part in the factory's own warehouse), click Search and look it up. fabrication/BOM.md lists an approved alternative for every part on this board. Use that list rather than picking a look-alike yourself, because several of these parts have near-identical siblings with different pinouts.
• The part most often short is TPS923610DRLR (U10, LCSC C52919131), the frontlight driver. Check its stock. If you are not fitting a frontlight panel, untick it along with the rest of the Frontlight group in Choosing a configuration. If you are fitting one and it is out of stock, see If the frontlight driver is out of stock. Stock may well be back by the time you order, so check first.
• If you are deliberately leaving a block off, remove its parts from the BOM and the CPL, or untick them here.
• Click Next.

If the frontlight driver is out of stock

JLCPCB's stock of the TPS923610DRLR comes and goes, and restocking is unpredictable. It isn't a dead end, just a slower one. In order of preference:

1. Pre-order it through JLCPCB. Any account can do this; it just takes lead time. While LCSC lists several suppliers for this part, the wait should be short.

   1. Sign in to JLCPCB and open Parts Manager → Order Parts.
   2. Search C52919131. Enter the quantity you need, plus one or two spares, and add it to My Parts Lib.
   3. Go to the cart and check out within the hour, or the cart is cancelled. JLCPCB emails the final price within 48 hours and refunds or charges the difference.
   4. Wait until the parts reach JLCPCB's warehouse. Pre-ordered parts can't be used before then, and they are never shipped to you; they only go into your assembly orders.
   5. Place the board order as above. At Step 5, U10 matches from your private library.

   JLCPCB's own guide: What is JLCPCB Parts Pre-order Service? · Pre-ordering terms

2. If you can't pre-order it, swap two parts, not one:

   Ref	Stock part	Swap to
   U10	TPS923610DRLR	TPS923611DRLR
   D3	SMAJ26A	SMAJ33A

   The TPS923611 shares the TPS923610's datasheet, package (SOT-563, DRL), pinout and 1.8 A switch limit, so it fits the same footprint. The one difference is its output ceiling: about 30 V, with over-voltage protection at 29.6–31.4 V, where the TPS923610 stops at about 24.5 V. The stock D3, an SMAJ26A clamp on LED_SW, starts conducting at 28.9 V. With a TPS923611 and the stock D3, a disconnected light lets the driver push current into D3 before its own protection trips, and D3 can burn out. An SMAJ33A doesn't conduct until about 36.7 V, so the driver's protection trips first. Don't leave D3 off instead: it protects the light connectors (J3, J6).

   The TPS923612 is not an option: it only comes in a 2 × 2 mm WSON (DRV) package, which doesn't fit this footprint.

Step 6: check the placement preview (do not skip this)

You see a drawing of the board with every part on it. This is your last chance to catch a part that is rotated wrongly, and the factory's own checker has corrected several on this board before. A matched part code does not prove the part is the right way round.

If something looks wrong, use the preview's rotate and move tools to fix it, and save a screenshot of the corrected preview. Click Next.

Step 7: through-hole parts, soldered by the factory or by you

Thirteen parts have legs that pass through the board rather than sitting on its surface. That is THT (through-hole technology), as opposed to SMD (surface-mount) for everything else. They are the USB-C socket J1, the battery connector J5, the expansion header J6 and the ten buttons SW1 to SW5 and SW7 to SW11. They are already in the files you uploaded, so this is a choice, not extra work:

• Let the factory solder them. JLCPCB charges a one-off hand-soldering fee (about $3.60 per order) plus roughly $0.016 per joint, which is about $1.20 per assembled board on top of the fee. It adds about a day. Confirm on the quote page that through-hole soldering appears as a line item.
• Solder them yourself. You get the parts loose and put in 74 joints per board: the USB-C shell pins, the JST battery connector, the 12-pin expansion header and ten buttons. The USB-C shell is the fiddly one. Worth doing if you own a decent iron and a fine tip; not worth it on a first board.

Step 8: pay, and keep the paperwork

Read the price summary: bare boards, setup fee, per-part-type fees, the parts themselves, assembly. Place the order. Then keep in one folder the order confirmation, the accepted BOM as the factory matched it, any substitutions it proposed, and your screenshot of the approved placement preview. If you order again, you will want to know exactly what was built the first time.

Using a different factory (PCBWay, NextPCB, others)

Nothing in the design is tied to JLCPCB. Upload files for other assemblers are kept in production/other_fabs/: a PCBWay BOM with KiCad's own placement file, a NextPCB BOM and centroid file in NextPCB's template (plus SMD-only and through-hole-only pairs in split/), and a bottom-side assembly drawing. They use the same Gerber zip as the JLCPCB order and are regenerated from the current design with:

python fabrication/make_fab_files.py --split

Know what you are taking on, though. JLCPCB is the only factory I have ordered boards from so far. My NextPCB attempt did not end in an order (what went wrong, and what it would have cost, is in fabrication/NEXTPCB_REV0_NOTES.md), and I have not tried PCBWay. Another factory is a fine choice if you prefer one. You will be doing the part matching, the rotation check and the back-and-forth with their engineers yourself, without a known-good order to compare against. Everything else in this guide assumes JLCPCB.

Choosing a configuration

The files in production/ build the full standard build: every block fitted except the DNP options. The board is a core that is always fitted, plus add-on groups you can leave off. For a reduced configuration, download its files from the builder on the website, or do it by hand: delete the listed references from the BOM and the CPL and leave the pads empty.

Each group lists every part that exists only to serve it, taken from the schematic netlist (rails and the shared I²C bus aside), so leaving a group off leaves nothing behind that does no work. The website's builder uses the same groups.

Notes:

• The panel choice drives touch and frontlight. The four 4.26" Good Display variants are GDEY0426T82 (plain), GDEQ0426T82-T01C (touch), -FL01C (frontlight) and -FT01C (touch + frontlight). Fit the touch parts only for a touch variant and the frontlight parts only for a light variant.
• U8, CR2, CR3 and F2 are J6's own protection and come off with it. U8 protects only J6 pins; CR2 and CR3 clamp the 3V3 and raw-battery pins where they leave the board, and the resettable fuse F2 sits in series with that battery pin and feeds nothing else. The 33 Ω series resistors R65/R68/R69 only reach J6 too; they cost nothing, so leaving them fitted on a header-less board is harmless. Do not remove U9, D3 or D8 with J6. U9 also protects the microSD data lines, and D3/D8 belong to the frontlight: they clamp its nets whether or not J6 is fitted.
• C12 belongs to the frontlight. It is on the shared LDO_IN rail but sits beside U10 as the driver's input capacitor; the LDO and power mux have their own, C4. Without the frontlight it can go.
• An external light needs J6. J3 only mates a panel with a bonded light; for any other light, the frontlight group drives it through the header.
• Fit only one of the two touch pin-order options. The default build fits R42 R44 R46 R52. The alternate wiring (R43 R45 R58 R66, DNP here) is for panels with the swapped pin order. Confirm the panel's pinout first.
• Leaving a button off needs nothing else changed. Its ladder resistor then does nothing and can be left off with it, but fitting it is harmless. Keep a ladder's pull-up and filter (R4/C27 bottom, R28/C28 side) as long as any key on that ladder is fitted.
• SW6 (boot button) and TP3-TP5 are DNP in every standard build. R64 (100 Ω) is fitted but only connects SW6, so it does nothing unless you fit the boot button.
• Per-board part totals are in fabrication/BOM.md.

Getting into download mode

SW6, the BOOT button, is left unfitted to save cost. You will normally never need it: the ESP32-S3 has native USB, so it presents itself to your computer without any button press. If you ever do need download mode (a firmware that has wedged the USB stack, for instance), bridge the two SW6 pads with a pair of metal tweezers while you tap RESET (SW11).

SW11 (RESET) is set back from the board edge on purpose: it is meant to be pressed through a pin-hole in the case with a paperclip, not by a finger.

Cutting the board down for a smaller display

The back of the board is marked with a line showing where it can be shortened for a smaller panel. If you do that:

• Disconnect the battery first. Battery positive runs across the cut line. Cutting into it with a pack connected can short the cell.
• It will not snap by hand. More than half the tab width is solid 1.6 mm FR-4, with live copper crossing it. Use a rotary tool (Dremel or similar) and cut along the marked line.
• You lose the expansion header J6 with its protection parts (U8, CR2, CR3, F2), the power button SW10, mounting hole H1 (five mounting points remain) and the two frontlight clamps D3/D8, which sit on that tongue. A cut board therefore runs its frontlight without those two clamps; read HARDWARE.md §7 before you drive a frontlight from one. After the cut, UP(2) can serve as the power button instead: leave R36 and R73 unpopulated and populate R72 and R74. The same instruction is printed on the schematic and on the board.
• Plan the cut before you order, so you can leave the parts you are cutting off out of the BOM. J6's series resistors R65/R68/R69 stay on the main board near the ESP32 but have nothing left to connect to, so they can be left out too.

Firmware

Silkscreen is built to run the open firmware made for Xteink's readers, starting with CrossPoint, which de-link, the reader before it, ran. There is no firmware release for this board yet: setting them up for its pins is the closed beta's work.

The plan is to bring the FreeInk SDK to the board, so that CrossPoint, CrossInk and the other Xteink X4 firmwares can add Silkscreen as a supported board, and to help maintain that support. First-power-up instructions come with it.

The board will never be locked. You can flash any firmware you like over USB-C.

Until the first Rev 1.0 boards check out, a board you order is one to build on. If you just want a reader to read on, wait for them to check out, or for the open-beta kits.

If you want to write firmware for it, docs/HARDWARE.md is the whole reference. The GPIO map is section 13, and section 13.1 lists what the board needs firmware to do: how to decode the charge-status pin, the frontlight driver's enable timing and over-voltage latch, the microSD power sequence, and the ADC limits.

The board and your case

This board is not tied to one enclosure. It is meant to work with many different case designs, of whatever style you like. No reference enclosure is supplied in this repository, so the case is yours to design or to take from someone else's.

What you need in order to design around it:

• A 3D model of the board is provided as a STEP file: docs/mechanical/silkscreen_pcb.step.
• Board outline 60.05 × 111.30 mm, 1.6 mm thick.
• Six M2 mounting holes (H1 to H6). Use screws with heads of 4 mm or less and no metal washers. Tracks run close to the holes under the solder mask.
• Every component is on the bottom face. The top face carries only the silkscreen art and the protruding legs of the through-hole parts, so the display sits over a nearly clear surface.
• Keep the antenna corner clear. The ESP32 module's PCB antenna overhangs a cut-out in the board edge with no copper under it. Do not lay the battery over that corner, and keep screws, metal inserts and the display's metal backplane away from it.
• Hole positions, connector locations, cavity heights, apertures and the rest of the mechanical reference are in docs/HARDWARE.md, section 16.

Specifications

Connection and GPIO reference: docs/HARDWARE.md.

Words used on the factory's website

Licence

The hardware is licensed under the CERN Open Hardware Licence Version 2, Strongly Reciprocal (CERN-OHL-S-2.0). See LICENSE. What that means:

• You may build this board, use it, modify it and sell it, including commercially. You do not need to ask.
• If you distribute or sell a board based on this design, you must make your design source available under the same CERN-OHL-S v2 licence, and pass on the copyright and licence notice, including any changes you made. That is what "strongly reciprocal" means.
• There is no warranty of any kind. If you build one and it does not work, that is your risk.

This is a plain-language summary, not legal advice; the licence text in LICENSE governs.

Copyright © 2026 idc LLC. This source describes Open Hardware and is licensed under the CERN-OHL-S v2. You may redistribute and modify this source and make products using it under the terms of the CERN-OHL-S v2 (https://ohwr.org/cern_ohl_s_v2.txt). This source is distributed WITHOUT ANY EXPRESS OR IMPLIED WARRANTY, INCLUDING OF MERCHANTABILITY, SATISFACTORY QUALITY AND FITNESS FOR A PARTICULAR PURPOSE. Please see the CERN-OHL-S v2 for applicable conditions.

SPDX-License-Identifier: CERN-OHL-S-2.0

Third-party component library files (from SnapEDA, Ultra Librarian and SamacSys) retain their own terms and are not covered by the project licence. See fabrication/THIRD_PARTY.md.

Working on the design

Nothing below is needed to order a board.

docs/HARDWARE.md is the one document to read before changing anything. It walks through every block of the schematic, explains why each part is there and what its value was chosen for, gives the GPIO and connector maps, and ends with the design conventions and the things that look like mistakes but are deliberate.

Plots and renders

Schematic PDF (single A2 sheet) and PCB layout PDF (2 pages: the front, then the back as you see it). Both are plotted from the current source. The board images at the top are renders of the same files, not the release record.

Repository layout

silkscreen_pcb.kicad_pro / .kicad_sch / .kicad_pcb   KiCad 9 project
sym-lib-table / fp-lib-table                          project-local library tables (${KIPRJMOD}-relative, resolve after a plain clone)
KiCad/9.0/3rdparty/                                   vendored symbols/footprints/3D models actually used by the design
docs/HARDWARE.md                                      hardware documentation
docs/mechanical/                                      board STEP model for case design
docs/images/                                          schematic block crops, full sheet, board renders
docs/silkscreen_pcb_schematic.pdf / _layout.pdf       schematic and PCB plots
fabrication/                                          part_fields.csv + apply script, make_fab_files.py, BOM.md / hand-build BOM, how-to
production/                                           release upload files: JLCPCB gerber zip + jlc_bom.csv + positions.csv; other_fabs/ for PCBWay and NextPCB
LICENSE / NOTICE                                      CERN-OHL-S v2

A plain git clone opens without missing libraries: every project library path is relative, all in-repo 3D models resolve, and everything else comes from KiCad's standard libraries (KiCad 9.0.x).

Bill of materials sources

fabrication/BOM.md is the current, netlist-derived sourcing reference: the optimized JLC build and the hand-build (DigiKey) list, with prices and the reasons for each swap. Both come from fabrication/part_fields.csv, which maps every reference to its prime manufacturer part number and its LCSC code. Accepted factory changes must still be frozen in the release records.

Regenerating the release files

The project and the reviewed exports use KiCad 9.0.6. Keep a backup before saving with a newer major version; newer file formats may not reopen in KiCad 9.

For JLCPCB, use the KiCad Fabrication Toolkit plugin for the placement export: it applies JLC's part-rotation database and reads the LCSC field from the footprints (set by fabrication/apply_part_fields.py, see fabrication/README.md). Regenerate the whole Toolkit set after every schematic or PCB save. A stale positions.csv silently misses new parts.

Raw kicad-cli exports, as a cross-check only and not a replacement for the reviewed Toolkit set:

kicad-cli pcb export gerbers -o fabrication/gerbers/ \
  --layers F.Cu,B.Cu,F.Mask,B.Mask,F.SilkS,B.SilkS,F.Paste,B.Paste,Edge.Cuts \
  --no-protel-ext --subtract-soldermask silkscreen_pcb.kicad_pcb
kicad-cli pcb export drill -o fabrication/gerbers/ --format excellon \
  --drill-origin absolute --excellon-units mm --excellon-separate-th silkscreen_pcb.kicad_pcb
kicad-cli pcb export pos -o fabrication/assembly/cpl.csv --format csv --units mm --side both silkscreen_pcb.kicad_pcb

See fabrication/README.md for the release-file workflow and the assembly checklist.

Predecessor project: de-link.me.