
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)

KiCad Like a Pro, 5th Edition, Volume 2: finished KiCad projects and saved stages (custom parts, LED matrix, DRV8833 motor drivers)
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.
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superseded.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.
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.
| Object | Layer | Priority | Notes |
|---|---|---|---|
GND_top zone | F.Cu | 0 | solid fill, thermal reliefs, remove islands "Always" |
GND_bottom zone | B.Cu | 0 | same settings |
VM_Zone zone | F.Cu | 1 | fillet corner smoothing, 2 mm radius; higher priority so it wins the overlap with GND_top |
Mounting hole rule area | F.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.
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.
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.rpt, regenerated 2026-08-01 with kicad-cli 10.0.4)0 unconnected pads. 19 violations, none of them copper problems:
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.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.text_thickness and 11 × silk_edge_clearance — silkscreen warnings on U1
and J1. Pre-existing.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.
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'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:
#PWR05-#PWR11 beneath, joined to VM by label. It sits clear of everything this
project already had, so its original coordinates still work.#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.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.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.
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./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.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.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.without-sense design variant.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.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.| Qty | Value | Footprint | References |
|---|---|---|---|
| 4 | 100n | Capacitor_SMD:C_0603_1608Metric | C1, C3, C5, C7 |
| 4 | 10u | Capacitor_SMD:C_0805_2012Metric | C2, C4, C6, C8 |
| 4 | 12k | Resistor_SMD:R_0603_1608Metric | R1, R2, R3, R4 |
| 4 | MAX7219CWG+ | Package_SO:SOIC-24W_7.5x15.4mm_P1.27mm | U1, U2, U3, U4 |
| 4 | TA08-81GWA | klp5e-ch07:LED_Matrix_TA08-81_20mm_8x8 | DS1, DS2, DS3, DS4 |
| 3 | 10k | Resistor_SMD:R_0603_1608Metric | R5, R6, R10 |
| 2 | 5.1k | Resistor_SMD:R_0603_1608Metric | R7, R8 |
| 2 | SW_Push | Button_Switch_THT:SW_PUSH_6mm | SW2, SW3 |
| 1 | 100k | Resistor_SMD:R_0603_1608Metric | R9 |
| 1 | AO3401A | Package_TO_SOT_SMD:SOT-23 | Q1 |
| 1 | Arduino_Nano_v3.x | Module:Arduino_Nano | A1 |
| 1 | LOGO | te:TE_Logo_11.6x4 | G*** |
| 1 | SW_SPDT | Button_Switch_THT:SW_CK_JS202011AQN_DPDT_Angled | SW1 |
| 1 | USB_C_Receptacle_PowerOnly_6P | Connector_USB:USB_C_Receptacle_GCT_USB4125-xx-x-0190_6P_TopMnt_Horizontal | J1 |
The 33 most common of 39 parts.

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)

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)

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)

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)

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)

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)

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)

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)

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)


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



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

osy/XG_Mobile_Station
Open source eGPU dock for ROG Ally and ROG Flow

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

BlueSCSI/BlueSCSI-v2
BlueSCSI v2/Ultra - an open source, open hardware, SCSI emulator using the Pi Pico PR2040 and Pico 2 RP2350
It measures 100 × 50 mm and has 2 copper layers, 1.6 mm thick.
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.
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.
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).