Skip to the content
2 layers100 × 50 mm4x8x8-LED Matrix Clock KLP5e, the printed circuit board in 3D

4x8x8-LED Matrix Clock KLP5e

futureshocked/KLP-5e-Vol2-Projects

KiCad Like a Pro, 5th Edition, Volume 2: finished KiCad projects and saved stages (custom parts, LED matrix, DRV8833 motor drivers)

Size
100 × 50 mm
Copper layers
2
Thickness
1.6 mm
Parts
39
Nets
107
Pads
257
Tracks, vias
728, 74
Pours
5
Routed
Yes
KiCad
KiCad 10.0 (file 20260206)
Created
17 Oct 2026
Updated
26 Oct 2026

Overview

4x8x8-LED Matrix Clock KLP5e is an open-source printed circuit board by futureshocked, from the futureshocked/KLP-5e-Vol2-Projects repository on GitHub, published under the MIT licence. It is a 2-layer board of 100 × 50 mm with 39 parts on 107 nets, routed with 728 tracks and 74 vias.

It is built around the MAX7219CWG+ and AO3401A. Its parts include 10 resistors, 8 capacitors, 4 ICs, 3 switches and 1 transistor. It belongs with the lEDs and displays and robots and motor control boards and the AVR (ATmega, ATtiny) boards of this library.

Main components

2

README

ch04-project/README.md

Chapters 4-5 — the canonical board

Status: chapter 4 complete and signed off (2026-08-01); chapter 5's schematic merged in (2026-08-07). This is the chapter-4 deliverable and the base every later chapter builds on. It was promoted here from ch03-04-05-06-ch04-stages/02-gnd-zones; the other stages and the old J1-only "live" ch03-04-05-06/ project are in ../_archive/ and are superseded.

⚠ The schematic and the PCB deliberately disagree by nine parts. Do not run "Update PCB from Schematic". C2-C8, R2 and R3 exist in the schematic only, because chapter 5's two figures are Symbol Fields Table shots that never touch the board. Pushing them onto the PCB would change a board that chapter 4's fourteen zone figures and chapter 6's gerber and paste figures were captured from. Placing them is a separate, later pass. See "Chapter 5 merge" below.

The file stem is still ch03-04-05-06.*. That is deliberate: KiCad requires the .kicad_pro, .kicad_pcb, .kicad_sch, .kicad_prl and .kicad_dru to share a stem, and the directory name already carries the meaning. Do not rename the files.

What the board contains

A 42 × 30 mm two-layer board, origin at (150, 50) mm, carrying the chapter-3 board setup (Default and Power net classes, pre-defined sizes, and the "Power minimum width" custom rule) plus all of chapter 4's copper work.

ObjectLayerPriorityNotes
GND_top zoneF.Cu0solid fill, thermal reliefs, remove islands "Always"
GND_bottom zoneB.Cu0same settings
VM_Zone zoneF.Cu1fillet corner smoothing, 2 mm radius; higher priority so it wins the overlap with GND_top
Mounting hole rule areaF.Cu, B.Cu, Edge.Cuts—keeps out tracks, vias and zone fills around the 2.5 mm hole; pads and footprints deliberately allowed, see below

Zone settings shared by all three pours: clearance 0.2 mm, minimum width 0.2 mm, pad connections "Thermal reliefs", thermal relief gap 0.5 mm, thermal spoke width 0.3 mm.

Twelve vias: a 3 × 3 grid of stitching vias in the top-right corner (x 187.3–189.8, y 52.9–56.6) tying the two ground pours together, plus three routing vias. The twelve-via array under U1's exposed pad is not counted here — those are pad 17 of the custom DRV8833 footprint, not board vias.

Footprints: J1, U1 (custom DRV8833_PD), C1, R1, and one MountingHole_2.5mm.

Figures captured from this board

All fourteen images/ch04/ch04-zones-*.png screenshots come from this project. Two of them, ch04-zones-solid-reliefs.png and ch04-zones-thermal-reliefs.png, are a matched pair showing header pad 6 under both pad-connection settings; the board is saved with thermal reliefs, so the solid capture came from a temporary toggle.

Figures are per-chapter snapshots, not one continuous build (policy set 2026-08-07). Each concept chapter is self-contained, and the chapter 8 and 9 capstones are where the reader sees every technique on a single board. So a later chapter changing this project does not oblige a re-capture here. Re-capture only when a figure becomes wrong about the thing its own chapter is teaching.

Custom library resolution

sym-lib-table and fp-lib-table use ${KIPRJMOD}/../ch01-02-custom-parts/…. That resolves correctly from this directory and is one reason the project lives at projects/ level rather than inside a stages subfolder. Opened from a stages subfolder the same path pointed at nothing, which produced the misleading "current configuration does not include the symbol library" warning.

DRC state (drc.rpt, regenerated 2026-08-01 with kicad-cli 10.0.4)

0 unconnected pads. 19 violations, none of them copper problems:

  • 1 × starved_thermal — U1 pad 13 reaches GND_top through a single spoke where "Minimum thermal relief spoke count" asks for two. (That constraint is KiCad's shipped default of 2, not something imported in chapter 3, so this check is on by default.) It is the acknowledged cost of running "Thermal reliefs" uniformly on a board that mixes through-hole and fine-pitch surface-mount pads, and the chapter walks through why it is safe to accept here: pad 17 beside it is on the same net and bonded to the same plane through twelve vias. No exclusion is recorded in the project (drc_exclusions is empty), so a fresh run still reports it and the count above still reads 19. The chapter presents "Exclude with comment…" as the reader's decision rather than making it for them.
  • 5 × track_width — /BOUT2 and /AOUT2 segments at 0.3 mm against the chapter-3 "Power minimum width" rule's 0.8 mm floor. Pre-existing routing, not zone work.
  • 2 × text_thickness and 11 × silk_edge_clearance — silkscreen warnings on U1 and J1. Pre-existing.

Settled: the keep-out does not exclude pads or footprints

The Mounting hole rule area excludes tracks, vias and zone fills, and deliberately leaves "Keep out pads" and "Keep out footprints" clear. Do not re-tick either. The 2.5 mm hole is itself a footprint with a plated pad, and it sits inside the area, so excluding either kind makes the rule flag the very object it exists to protect. An earlier version of the board had "Keep out pads" ticked and produced exactly that items_not_allowed violation; the board and ch04-zones-keep-out-1.png were both re-done on 2026-08-01 to fix it.

Known cosmetic issue

The mounting-hole footprint is unannotated: its reference reads REF**, which is visible on the silkscreen in ch04-zones-keep-out-2.png, -3.png and in the 3D render -4.png. Annotating it to MH1 would invalidate those three captures, so it has been left as is and no caption draws attention to it.

Chapter 5 merge (2026-08-07)

Chapter 5's schematic content now lives here. ../ch03-04-05-06-ch05-stages/ is history: useful for its design notes, but no longer a thing to resume from.

It could not be merged as a file copy. The ch05 stages were cut from _archive/ch03-04-05-06-live-stale/ at 09:14 on 2026-08-01, and this project's schematic was saved at 11:41 the same day, two and a half hours later, as a complete re-layout: every wire, label, no-connect and symbol moved, J1 changed from Conn_01x08_Pin to Conn_01x06_Pin, and the wire count went from 19 to 10. Copying the stage schematic over this one would have reverted all of that and desynced it from the PCB's 1x06 footprint.

What was done instead, since U1 moved by a uniform (-64.77, -2.54) with no rotation:

  • Decoupling bank transplanted unchanged. C2-C8 (100 nF 0603) on a rail at y 132.08 with #PWR05-#PWR11 beneath, joined to VM by label. It sits clear of everything this project already had, so its original coordinates still work.
  • Sense cluster translated by the same delta as U1. R2/R3 (0R2 0603) now at (171.45, 97.79) and (182.88, 97.79) with #PWR12/#PWR13 beneath, and the AISEN/BISEN stubs moved onto U1's pin ends at (163.83, 68.58) and (163.83, 78.74). The two no-connects that were sitting on those two pins were removed.
  • MPN and Supplier added to C1, J1, R1 and U1, matching the values the stage had already set on the other nine parts.
  • J1's Value corrected from Conn_01x08_Pin to Conn_01x06_Pin. The symbol had been 6-pin since 2026-08-01, but its Value string still claimed 8, which would have shown as a contradictory row in chapter 5's Figure 1.
  • .kicad_pro: four keys transplanted, not the file. schematic.drawing.field_names (the MPN/Supplier templates), bom_settings, bom_fmt_settings and bom_export_filename (bom_${VARIANT}.csv). Everything else, including chapter 3's net classes and the .kicad_dru "Power minimum width" rule, is untouched.

⚠ J1's MPN needs your confirmation

The stage had PPTC081LFBN-RC, the 8-position Sullins part. J1 is now 6-position, so this is set to PPTC061LFBN-RC, the same series with the position count corrected. Two things to check, because both are visible in Figure 1: that the derived part number is the one you want, and that the PPTC series is right at all, since it is a female socket while the footprint is a male pin header. That mismatch predates this merge.

Verification

  • ERC unchanged from the pre-merge baseline. 3 violations before and after, the same classes: 2 power_pin_not_driven, 1 lib_symbol_mismatch on U1. Both reports are kept, as erc-premerge.rpt and erc.rpt. Adding 18 symbols introduced nothing new.
  • Netlist confirms pin placement, which ERC alone cannot: /AISEN 2: R2.1, U1.3 and /BISEN 2: R3.1, U1.6 (AISEN is pin 3, BISEN pin 6), /VM with 10 nodes and GND with 13. Saved as net.net.
  • Grouped BOM gives the row chapter 5 promises, in bom.csv: "C2-C8","7","100nF","Capacitor_SMD:C_0603_1608Metric","CL10B104KB8NNNC","Digi-Key". bom-ungrouped.csv is the Figure 2 view. ch03-04-05-06.svg is a plot of the merged sheet.
  • Note that kicad-cli sch export bom ignores the project's saved bom_settings unless you pass --fields/--group-by explicitly. The GUI does use them, so the figures will be right; the CSVs above were generated with the flags spelled out.

What comes next

  1. The without-sense design variant. DONE 2026-08-17, and it did not need the GUI after all: the override is a nested s-expression written directly into the schematic. It overrides R2/R3's Value (0R2 → 0R), not their fitting. DNP would be electrically wrong here, because AISEN/BISEN are the bridge ground return. DONE 2026-08-18: a second override on the same two parts sets MPN to CRCW06030000Z0EA, a 2 A-rated 0 Ω 0603 jumper. Both BOM exports are regenerated and differ on exactly one row and two cells. Full reasoning in the fence at the top of ../../manuscript/05-bom-in-depth.md.
  2. Chapter 5's figures. DONE 2026-08-18. Five were re-shot off this project, not the three first thought: 5.1, 5.2, 5.3, 5.10 and 5.11. 5.1 and 5.10 joined because the global MPN_global template postdates them, so leaving them alone would have put the chapter's four Symbol Fields Table figures on two different field lists. Verified mechanically: no ticked DNP anywhere, override shading on 5.11's Value cell alone, and 5.10/5.11 identical in size and field list. If you ever re-shoot these, capture from this project, never from ../ch03-04-05-06-ch05-stages/03-variant/, which has no variant at all, and change nothing in the dialogue but the variant selection.
  3. Later, separately: placing C2-C8 and R2/R3 on the PCB. See the warning at the top.

Parts

39
QtyValueFootprintReferences
4100nCapacitor_SMD:C_0603_1608MetricC1, C3, C5, C7
410uCapacitor_SMD:C_0805_2012MetricC2, C4, C6, C8
412kResistor_SMD:R_0603_1608MetricR1, R2, R3, R4
4MAX7219CWG+Package_SO:SOIC-24W_7.5x15.4mm_P1.27mmU1, U2, U3, U4
4TA08-81GWAklp5e-ch07:LED_Matrix_TA08-81_20mm_8x8DS1, DS2, DS3, DS4
310kResistor_SMD:R_0603_1608MetricR5, R6, R10
25.1kResistor_SMD:R_0603_1608MetricR7, R8
2SW_PushButton_Switch_THT:SW_PUSH_6mmSW2, SW3
1100kResistor_SMD:R_0603_1608MetricR9
1AO3401APackage_TO_SOT_SMD:SOT-23Q1
1Arduino_Nano_v3.xModule:Arduino_NanoA1
1LOGOte:TE_Logo_11.6x4G***
1SW_SPDTButton_Switch_THT:SW_CK_JS202011AQN_DPDT_AngledSW1
1USB_C_Receptacle_PowerOnly_6PConnector_USB:USB_C_Receptacle_GCT_USB4125-xx-x-0190_6P_TopMnt_HorizontalJ1

The 33 most common of 39 parts.

More from futureshocked/KLP-5e-Vol2-Projects

9
  • 2 layers100 × 50 mm4x8x8-LED Matrix Clock KLP5e, the printed circuit board in 3D

    4x8x8-LED Matrix Clock KLP5e

    futureshocked/KLP-5e-Vol2-Projects

    KiCad Like a Pro, 5th Edition, Volume 2: finished KiCad projects and saved stages (custom parts, LED matrix, DRV8833 motor drivers)

    32 partsMIT
  • 2 layers83.8 × 48 mmCh08-drv8833, the printed circuit board in 3D

    Ch08-drv8833

    futureshocked/KLP-5e-Vol2-Projects

    KiCad Like a Pro, 5th Edition, Volume 2: finished KiCad projects and saved stages (custom parts, LED matrix, DRV8833 motor drivers)

    29 partsMIT
  • 2 layers52 × 48 mmCh08-drv8833, the printed circuit board in 3D

    Ch08-drv8833

    futureshocked/KLP-5e-Vol2-Projects

    KiCad Like a Pro, 5th Edition, Volume 2: finished KiCad projects and saved stages (custom parts, LED matrix, DRV8833 motor drivers)

    20 partsMIT
  • 2 layersCh10-multi channel, the printed circuit board in 3D

    Ch10-multi channel

    futureshocked/KLP-5e-Vol2-Projects

    KiCad Like a Pro, 5th Edition, Volume 2: finished KiCad projects and saved stages (custom parts, LED matrix, DRV8833 motor drivers)

    17 partsMIT
  • 2 layers60 × 38 mmKlp5e net tie demo, the printed circuit board in 3D

    Klp5e net tie demo

    futureshocked/KLP-5e-Vol2-Projects

    KiCad Like a Pro, 5th Edition, Volume 2: finished KiCad projects and saved stages (custom parts, LED matrix, DRV8833 motor drivers)

    15 partsMIT
  • 4 layers57.5 × 52.9 mmCh10-recipes, the printed circuit board in 3D

    Ch10-recipes

    futureshocked/KLP-5e-Vol2-Projects

    KiCad Like a Pro, 5th Edition, Volume 2: finished KiCad projects and saved stages (custom parts, LED matrix, DRV8833 motor drivers)

    10 partsMIT
  • 2 layersDRV8833-Stage, the printed circuit board in 3D

    DRV8833-Stage

    futureshocked/KLP-5e-Vol2-Projects

    KiCad Like a Pro, 5th Edition, Volume 2: finished KiCad projects and saved stages (custom parts, LED matrix, DRV8833 motor drivers)

    8 partsMIT
  • 2 layers42 × 30 mmCh03-04-05-06, the printed circuit board in 3D

    Ch03-04-05-06

    futureshocked/KLP-5e-Vol2-Projects

    KiCad Like a Pro, 5th Edition, Volume 2: finished KiCad projects and saved stages (custom parts, LED matrix, DRV8833 motor drivers)

    5 partsMIT
  • 2 layersNPN LED, the printed circuit board in 3D

    NPN LED

    futureshocked/KLP-5e-Vol2-Projects

    KiCad Like a Pro, 5th Edition, Volume 2: finished KiCad projects and saved stages (custom parts, LED matrix, DRV8833 motor drivers)

    4 partsMIT

Similar boards

  • 2 layers100 × 100 mmCan ssr, the printed circuit board in 3D

    Can ssr

    czalinski/ThlHats

    Test devices with Raspberry PI HAT form factor

    201 partsMIT
  • 2 layers97.8 × 97.8 mmOH - UIP - Led Distribution, the printed circuit board in 3D

    OH - UIP - Led Distribution

    bnepethomas/bne-arduino-flight-simulator-interfaces

    Automatically exported from code.google.com/p/bne-arduino-flight-simulator-interfaces

    57 parts17
  • 2 layers75 × 160 mmOven2, the printed circuit board in 3D

    Oven2

    bybzmt/practise

    51 parts
  • 2 layers192.2 × 150.5 mmDjinn, the printed circuit board in 3D

    Djinn

    tzarc/keyboards

    @tzarc's custom keyboard designs.

    292 parts993CERN-OHL-S-2.0
  • 4 layers102.9 × 96.7 mmPicoGUS chipdown, the printed circuit board in 3D

    PicoGUS chipdown

    polpo/picogus

    Emulation of ISA sound cards and CD-ROM on Raspberry Pi Pico (GUS, SB/Adlib, MPU-401, Tandy, CMS, Panasonic CD-ROM) with USB mouse/joystick support

    99 parts805
  • 6 layers237.9 × 80.5 mmXG Mobile Dock, the printed circuit board in 3D

    XG Mobile Dock

    osy/XG_Mobile_Station

    Open source eGPU dock for ROG Ally and ROG Flow

    300 parts712CC-BY-4.0
  • 2 layers60 × 111.3 mmSilkscreen pcb, the printed circuit board in 3D

    Silkscreen pcb

    iandchasse/silkscreen-pcb

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

    189 parts589CERN-OHL-S-2.0
  • 2 layers89.2 × 82.6 mmDesktop 50 Pin TopConn, the printed circuit board in 3D

    Desktop 50 Pin TopConn

    BlueSCSI/BlueSCSI-v2

    BlueSCSI v2/Ultra - an open source, open hardware, SCSI emulator using the Pi Pico PR2040 and Pico 2 RP2350

    108 parts459GPL-3.0

Questions

How big is the 4x8x8-LED Matrix Clock KLP5e PCB?

It measures 100 × 50 mm and has 2 copper layers, 1.6 mm thick.

What parts does the 4x8x8-LED Matrix Clock KLP5e use?

39 parts, built around the MAX7219CWG+ and AO3401A. The full list of its parts is on this page, with links to each part's symbol and footprint where PCBKit's library has them.

Where can I download the 4x8x8-LED Matrix Clock KLP5e KiCad files?

From the futureshocked/KLP-5e-Vol2-Projects repository on GitHub, at the commit this page was made from: the board is ch07-project/led-matrix-final/4x8x8-LED-Matrix-Clock-KLP5e.kicad_pcb. PCBKit opens the board in the browser, with nothing to install.

Can I use the 4x8x8-LED Matrix Clock KLP5e design in my own project?

Its repository publishes it under the MIT licence: you may reuse it on that licence's terms (keep the author's notice, and for a copyleft licence share your changes alike).