Skip to the content
4 layers60 × 40 mmDaedalus core pdn, the printed circuit board in 3D

Supplied KiCad 8 board asset for the Daedalus core PDN exercise (CC0-1.0)

Size
60 × 40 mm
Copper layers
4
Thickness
1.54 mm
Parts
6
Nets
2
Pads
231
Tracks, vias
49, 57
Pours
10
Routed
Yes
KiCad
KiCad 8.0 (file 20240108)
Created
23 Oct 2026
Updated
23 Oct 2026

Overview

Daedalus core pdn is an open-source printed circuit board by chibiosya, from the chibiosya/daedalus-core-pdn repository on GitHub, published under the CC0-1.0 licence. It is a 4-layer board of 60 × 40 mm with 6 parts on 2 nets, routed with 49 tracks and 57 vias.

README

README.md

daedalus-core-pdn

Supplied KiCad 8 board asset for the Daedalus core power-delivery-network (PDN) exercise: a 60 x 40 mm, 4-layer board carrying a 225-ball SoC (U1) with its core-supply fanout, a VRM output (U2), a GND plane, a VDD_CORE plane, four mounting holes and a set of named keepout areas. It is meant to be designed onto: you add decoupling capacitors, their vias and tracks; everything that is already here is a supplied item and must not be moved or changed.

FilePurpose
daedalus_core_pdn.kicad_pcbThe board (KiCad 8 format, version 20240108, all footprints embedded, zones filled)
daedalus_core_pdn.kicad_proProject: numeric design-rule constraints and the Default net class
daedalus_core_pdn.kicad_druCustom rules: no via-in-pad, the keepout rules, the mounting-hole copper keepout
supplied_items.jsonUUID + geometry of every supplied item (footprints, tracks, vias, zones, rule areas, edge cuts, groups) and the U1 ball map
tools/Reproducible generator / zone filler / verifier / build script
images/SVG renders of F.Cu, B.Cu, In1.Cu and In2.Cu

Keep the three daedalus_core_pdn.* files together. kicad-cli pcb drc loads the .kicad_pro and .kicad_dru that sit next to the board; without them KiCad falls back to its defaults (0.2 mm net-class clearance) and the supplied BGA fanout no longer passes DRC.

Validation status (KiCad 8.0.9, kicad-cli)

text
kicad-cli pcb drc --severity-error   --exit-code-violations daedalus_core_pdn.kicad_pcb   -> exit 0, 0 violations, 0 unconnected
kicad-cli pcb drc --severity-warning --exit-code-violations daedalus_core_pdn.kicad_pcb   -> exit 0, 0 violations (no warnings remain)

The keepout rules were proven to fire with a negative-test board (tools/generate_board.py --negative-test): a C_0402 capacitor placed inside KO_BGA_TOP, a via inside KO_VRM, a track inside KO_DDR_CHANNEL on B.Cu, a via inside KO_MH1 and a via inside a non-U2 SMD pad are each reported as an error by the corresponding rule (ko_bga_top, ko_vrm, ko_ddr_channel, ko_mh1 + mounting_hole_copper_keepout, no_via_in_pad), and a via centred between two adjacent U1 balls (A1/A2, at 94.8, 74.4) fails on clearance to the ball pads while ko_bga_top fires only on the capacitor, not on any via. A positive-test board (--positive-test) with one via at an outer-ring interstitial position of the ball grid (A1 + (0.4, 0.4) = 94.8, 74.8, inside KO_BGA_TOP but outside the core 7x7 field) passes DRC with 0 violations. tools/build.sh re-runs both tests every build.

Board

  • Outline: rectangle 60 x 40 mm on Edge.Cuts, corners (70,60) (130,60) (130,100) (70,100). All coordinates in this document are KiCad board coordinates in mm (x to the right, y downwards).
  • Finished thickness 1.54 mm, 4 copper layers. Stackup is stored in the board file (Board Setup > Physical Stackup):
#LayerTypeThicknessNote
1F.Cucopper0.035 mmsignal, components
dielectric 1prepreg FR40.200 mm
2In1.Cucopper0.035 mmGND plane
dielectric 2core FR41.000 mm
3In2.Cucopper0.035 mmVDD_CORE plane
dielectric 3prepreg FR40.200 mm
4B.Cucopper0.035 mmsignal

Solder-mask layers are entered with 0 thickness so the stackup total shown by KiCad equals the specified 1.54 mm.

  • Nets: GND (net 1) and VDD_CORE (net 2). There are no other nets; 176 of the U1 balls are intentionally unconnected.
  • Planes: In1.Cu is a filled GND zone, In2.Cu a filled VDD_CORE zone. Both cover the board with a 1.0 mm clearance to the edge (outline (71,61)-(129,99)), zone clearance 0.1 mm, minimum width 0.2 mm, solid (no thermal relief) connections. The fills are stored in the file.
  • Mounting holes H1..H4: non-plated 3.2 mm drill at (73,63), (127,63), (73,97), (127,97). Copper is kept 3.5 mm (radius) away from each hole centre on every layer, see mounting_hole_copper_keepout below and the KO_MH rule areas.

U1: SoC BGA (supplied, do not change)

  • Footprint BGA-225_15x15_0.8mm, reference U1, centre (100.000, 80.000), rotation 0, body 12 x 12 mm, courtyard (F.CrtYd) 13 x 13 mm centred on U1.
  • 15 x 15 balls on a 0.8 mm pitch. Pad: SMD circle 0.400 mm, NSMD (solder-mask margin +0.05 mm). Rows A B C D E F G H J K L M N P R (JEDEC, I/O/Q skipped), columns 1..15. Ball A1 is top-left in the KiCad view at (94.4, 74.4); ball R15 is bottom-right at (105.6, 85.6). Ball (row r, col c) is at x = 94.4 + 0.8 (c-1), y = 74.4 + 0.8 (index of r).
  • Core region: the central 7 x 7 balls, rows E..L (E F G H J K L) x columns 5..11, checkerboard: VDD_CORE where (i + j) is even (25 balls), GND where odd (24 balls), i,j = 0..6 inside the block. Every other ball has no net.

Ball map (V = VDD_CORE, G = GND, . = no net):

row \ col123456789101112131415
A...............
B...............
C...............
D...............
E....VGVGVGV....
F....GVGVGVG....
G....VGVGVGV....
H....GVGVGVG....
J....VGVGVGV....
K....GVGVGVG....
L....VGVGVGV....
M...............
N...............
P...............
R...............
  • Dog-bone fanout, one per core ball (49): F.Cu track, width 0.15 mm, from the ball centre to a via at (+0.400, +0.400) mm from the ball centre (towards +x, +y, i.e. down-right in the view). Via: through-hole, drill 0.200 mm, diameter 0.450 mm, same net as the ball. The vias sit on the interstitial positions of the ball grid, at x = 94.8 + 0.8 (c-1), y = 74.8 + 0.8 (row index), for c = 5..11 and row index 4..10. All 49 tracks and 49 vias are members of the group U1_FANOUT.

U2: VRM output (supplied, do not change)

  • Footprint VRM_OUT, reference U2, centre (75.000, 80.000), courtyard 6 x 8 mm centred on U2.
  • Pad 1, net VDD_CORE: SMD rectangle 4.0 x 3.0 mm on F.Cu centred at (75.0, 78.0).
  • Pad 2, net GND: SMD rectangle 4.0 x 3.0 mm on F.Cu centred at (75.0, 82.0).
  • 4 through vias per pad, drill 0.3 mm, diameter 0.6 mm, same net as the pad, at x = 73.8 and 76.2, y = pad centre y -0.8 and +0.8, i.e. (73.8|76.2, 77.2|78.8) for pad 1 and (73.8|76.2, 81.2|82.8) for pad 2. These 8 vias are members of the group U2_VIAS.

Via sizes

UseDiameterDrillAnnular ring
U1 dog-bone vias (49)0.450 mm0.200 mm0.125 mm
U2 output vias (8)0.600 mm0.300 mm0.150 mm
Default net class via (for anything you add)0.450 mm0.200 mm0.125 mm

Keepouts (rule areas)

The keepouts are named rule areas with no keepout flags of their own; the enforcement lives in daedalus_core_pdn.kicad_dru so that supplied items can be exempted while anything added later is checked. Inside each area footprints, vias and tracks are forbidden on the listed layers, with one exception: KO_BGA_TOP forbids footprints and tracks only. Vias are allowed under the BGA, subject to the normal rules against the ball pads (0.100 mm clearance, 0.250 mm hole-to-copper clearance, no_via_in_pad). In practice that means the interstitial positions of the ball grid (ball centre + (±0.4, ±0.4) mm), where the supplied dog-bone vias already sit with 0.141 mm clearance; a via centred between two adjacent balls overlaps their pads and fails.

NameLayersForbidsShapeCoordinates (mm)Exempt supplied items
KO_BGA_TOPF.Cufootprints, tracks (vias allowed)14 x 14 mm squarex 93..107, y 73..87 (centre 100,80)U1, group U1_FANOUT
KO_DDR_CHANNELF.Cu, B.Cufootprints, vias, tracksrectanglex 108..130, y 64..96none
KO_CONNECTORF.Cu, B.Cufootprints, vias, tracksrectanglex 70..90, y 60..70H1
KO_VRMF.Cu, B.Cufootprints, vias, tracksrectanglex 70..81, y 74..86U2, group U2_VIAS
KO_MH1all copperfootprints, vias, trackscircle r 3.5 mm (72-gon)centre (73,63)H1
KO_MH2all copperfootprints, vias, trackscircle r 3.5 mm (72-gon)centre (127,63)H2
KO_MH3all copperfootprints, vias, trackscircle r 3.5 mm (72-gon)centre (73,97)H3
KO_MH4all copperfootprints, vias, trackscircle r 3.5 mm (72-gon)centre (127,97)H4

Rule areas in KiCad are polygons, so each circle is a 72-sided polygon with its vertices on the 3.5 mm radius. A footprint counts as inside an area when its courtyard intersects the area (KiCad semantics), so give your capacitors a courtyard.

Design rules

Numeric constraints (.kicad_pro, Board Setup > Constraints):

ConstraintValue
Minimum clearance0.100 mm
Minimum track width0.150 mm
Minimum via diameter0.450 mm
Minimum via drill (through hole)0.200 mm
Minimum annular ring0.125 mm
Hole-to-hole clearance0.250 mm
Copper-to-hole clearance0.250 mm (KiCad default)
Copper-to-edge clearance0.500 mm
Courtyard overlaperror
Silkscreen / solder-mask rulesKiCad defaults

Net class Default: clearance 0.100 mm, track width 0.200 mm, via 0.450 / 0.200 mm. (The clearance is set equal to the minimum clearance because KiCad's default of 0.2 mm would fail the specified BGA fanout, whose via-to-neighbouring-ball gap is 0.141 mm.)

Custom rules (.kicad_dru, KiCad 8 syntax):

text
(rule no_via_in_pad
	(condition "A.Type == 'Via' && B.Type == 'Pad' && B.Pad_Type == 'SMD' && !B.memberOfFootprint('U2')")
	(constraint physical_clearance (min 0.1mm)))

No via may touch or come within 0.1 mm of any SMD pad, regardless of net. U2's pads are supplied with vias inside them and are the only exemption.

text
(rule ko_bga_top
	(layer "F.Cu")
	(condition "A.intersectsArea('KO_BGA_TOP') && !A.memberOfFootprint('U1') && !(A.Type == 'Footprint' && A.Reference == 'U1') && !A.memberOfGroup('U1_FANOUT')")
	(constraint disallow footprint track))

One such rule per keepout (ko_bga_top, ko_ddr_channel, ko_connector, ko_vrm, ko_mh1..4), each restricted to the area's layers ((layer outer) for F.Cu + B.Cu, no layer clause for all-copper) and exempting only the supplied items listed in the table above. All of them except ko_bga_top use (constraint disallow footprint via track); ko_bga_top omits via, so vias under the BGA are governed by the clearance, hole-to-copper and no_via_in_pad rules only.

text
(rule mounting_hole_copper_keepout
	(condition "B.Pad_Type == 'NPTH, mechanical'")
	(constraint hole_clearance (min 1.9mm)))

Hole edge (radius 1.6 mm) + 1.9 mm = the 3.5 mm copper-free radius around each mounting hole. This is honoured by the zone filler (the planes already have the cut-outs) and by DRC for any copper you add.

Capacitor via proximity is checked by the grader, not by DRC.

Capacitor footprints you may use

From the official KiCad library Capacitor_SMD: C_0201_0603Metric, C_0402_1005Metric, C_0603_1608Metric, C_0805_2012Metric, C_1210_3225Metric. The Value field must be exactly one of 0.1uF 0.22uF 0.47uF 1.0uF 2.2uF 4.7uF 10uF 22uF 47uF 100uF (as allowed per package in the brief).

Supplied items

supplied_items.json lists every supplied object with its UUID and geometry: 6 footprints (U1, U2, H1..H4), 49 tracks, 57 vias, 2 planes, 8 rule areas, the Edge.Cuts rectangle and the 2 groups, plus the U1 ball map. UUIDs are deterministic (UUID v5 of the item name) so a regenerated board has the same IDs. python3 tools/verify_board.py daedalus_core_pdn.kicad_pcb supplied_items.json checks that all of them are still present and that the geometry matches this document.

Rebuilding

text
KICAD_APP=/Applications/KiCad/KiCad.app tools/build.sh

tools/generate_board.py (stdlib Python, no KiCad needed) writes the three KiCad files and supplied_items.json from the numbers above; tools/finalize_board.py (KiCad's bundled python, pcbnew) fills the zones and re-saves in canonical KiCad 8 format; tools/build.sh then runs DRC at error and warning severity, the negative and positive keepout tests, the verifier and the SVG exports. Built and validated with KiCad 8.0.9 on macOS.

Renders

F.CuB.Cu
F.CuB.Cu
In1.Cu (GND plane)In2.Cu (VDD_CORE plane)
In1.CuIn2.Cu

Notes and assumptions

  • The mounting-hole footprints have no courtyard on purpose: KiCad tests "footprint in area" with the courtyard, and the holes sit inside their own KO_MH areas and (H1) inside KO_CONNECTOR.
  • Solder-mask thickness is 0 in the stackup so the total equals 1.54 mm; nothing else depends on it.
  • Keepout rules use intersectsArea (any overlap is a violation), the same test KiCad uses for its own rule-area keepouts.
  • Reference designators of H1..H4 are hidden; U1/U2 references are on F.SilkS outside their pads.

Changelog

  • v1.1 (2026-10-24): ko_bga_top no longer disallows vias (disallow footprint track instead of disallow footprint via track). The keepout was meant to keep components and tracks off the top side under the BGA, not to forbid through vias at the interstitial positions of the ball grid, which the supplied dog-bones already use. Vias under the BGA are governed by the normal clearance, hole-to-copper and no_via_in_pad rules. Negative test extended (via between two balls must fail on clearance) and a positive test added (interstitial via must pass). Board, project file and supplied_items.json are unchanged.
  • v1.0 (2026-10-23): initial release.

Licence

CC0 1.0 Universal (public domain dedication), see LICENSE.

Parts

6
QtyValueFootprintReferences
4MountingHole_3.2mmMountingHole_3.2mmH1, H2, H3, H4
1SoCBGA-225_15x15_0.8mmU1
1VRM_OUTVRM_OUTU2

Similar boards

  • 4 layers37.1 × 61.5 mmMCLZ8 PCB, the printed circuit board in 3D

    MCLZ8 PCB

    MicroCoreLabs/Projects

    Ted Fried's MicroCore Labs Projects - FPGA CPU cores and emulators for the 8088, 8086, 8051, 6502, 68000, Z80, Risc-V, and also Typewriter and EPROM Emulator projects.

    6 parts534
  • 4 layers15.6 × 51.4 mmHyperram 3p3v, the printed circuit board in 3D

    Hyperram 3p3v

    loxodes/vna

    Under development open hardware microwave vector network analyzer

    6 parts205
  • 4 layers37 × 27 mmProbecard pinheader, the printed circuit board in 3D

    Probecard pinheader

    azonenberg/starshipraider

    Open hardware test equipment

    6 parts193BSD-3-Clause
  • 4 layers312 × 111.2 mmPCIexpress x1 full, the printed circuit board in 3D

    PCIexpress x1 full

    lucanastasio/PCIexpress-KiCad

    PCI express libraries and templates for KiCad

    6 parts170
  • 4 layersEsp32s3 Wroom 1, the printed circuit board in 3D

    Esp32s3 Wroom 1

    BerkeleyHCI/PolymorphicBlocks

    A Python-based hardware description language for PCBs for higher-level (block-diagram / system-architecture level) PCB design through libraries of directly reusable subcircuit generators.

    6 parts94BSD-3-Clause
  • 4 layers29.4 × 22.1 mmAssembly power, the printed circuit board in 3D

    Assembly power

    buganini/Kikakuka

    Kikakuka — KiCad Workspace, Panelization, Build Variants, Differ & FreeCAD PCB Bending and Assembly

    6 parts81MIT
  • 4 layers30.2 × 40.6 mmMicrostrip width nightly, the printed circuit board in 3D

    Microstrip width nightly

    matthuszagh/fmcw

    6GHz frequency-modulated continuous-wave radar with real-time range detection

    6 parts66Apache-2.0
  • 4 layers149.9 × 99.1 mmArchimedes bus scope, the printed circuit board in 3D

    Archimedes bus scope

    google/myelin-acorn-electron-hardware

    Phillip Pearson's retro hardware projects for the Acorn Electron

    6 parts59Apache-2.0

Questions

How big is the Daedalus core pdn PCB?

It measures 60 × 40 mm and has 4 copper layers, 1.54 mm thick.

What parts does the Daedalus core pdn use?

6 parts. 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 Daedalus core pdn KiCad files?

From the chibiosya/daedalus-core-pdn repository on GitHub, at the commit this page was made from: the board is daedalus_core_pdn.kicad_pcb. PCBKit opens the board in the browser, with nothing to install.

Can I use the Daedalus core pdn design in my own project?

Its repository publishes it under the CC0-1.0 licence: you may reuse it on that licence's terms (keep the author's notice, and for a copyleft licence share your changes alike).