SN-L00/hardware/kicad/PCB_LAYOUT.md

SN-L00 PCB Layout Guide

Quick Start - Complete the Layout in KiCad

1. Open the project: SN-L00.kicad_pro
2. Import footprints:
   • Open PCB Editor
   • Tools → Update PCB from Schematic (F8)
   • Click "Update PCB" to import all footprints
3. Place components:
   • In Scripting Console (Tools → Scripting Console):

   exec(open('scripts/place_components.py').read())
   

   • Or manually place using coordinates below
4. Add mounting holes:
   • Place MountingHole:MountingHole_3.2mm_M3 at (14, 5) and (14, 95)
5. Route traces:
   • Use Freerouting: File → Export → Specctra DSN, then import routed SES
   • Or route manually with 'X' key
6. Fill zones:
   • Press 'B' to fill all zones
7. Run DRC: Inspect → Design Rules Checker
8. Export Gerbers: File → Fabrication Outputs → Gerbers

Board Dimensions

Parameter	Value	Notes
Width	28.0mm	6HP panel = 30mm, PCB 1mm clearance each side
Height	100.0mm	Fits standard 3U with clearance
Thickness	1.6mm	Standard PCB
Layers	2	Front + Back copper
Depth (mounted)	~22mm	Skiff-friendly (<25mm)

Mounting Holes

Hole	Position	Size
MH1 (top)	14.0, 5.0	3.2mm (M3)
MH2 (bottom)	14.0, 95.0	3.2mm (M3)

Component Placement (Top to Bottom)

     0mm                    28mm
      │←────── 28mm ───────→│
      ┌────────────────────┐ ─┬─ 0mm
      │    ○ MH1 (M3)      │  │
      │                    │  │ 5mm
      ├────────────────────┤ ─┤
      │                    │  │
      │  ┌──────────────┐  │  │
      │  │    OLED      │  │  │ 10-25mm
      │  │   MOD2       │  │  │
      │  │  (128x32)    │  │  │
      │  └──────────────┘  │  │
      │                    │  │
      ├────────────────────┤ ─┤
      │       [BTN]        │  │ 28-35mm
      │        SW1         │  │
      ├────────────────────┤ ─┤
      │                    │  │
      │  ┌──────────────┐  │  │
      │  │  RP2040-Zero │  │  │ 38-55mm
      │  │    MOD1      │  │  │
      │  │  (18x23mm)   │  │  │
      │  └──────────────┘  │  │
      │                    │  │
      ├────────────────────┤ ─┤
      │  SMD Components    │  │
      │  U1 U2 U3          │  │ 58-75mm
      │  C1-C5 R1-R6       │  │
      │  D1-D4 D2(LED)     │  │
      ├────────────────────┤ ─┤
      │                    │  │
      │  ○ J2    ○ J3      │  │ 78-88mm
      │  TRIG   RETURN     │  │
      │                    │  │
      ├────────────────────┤ ─┤
      │  ═══════════════   │  │ 88-95mm
      │       J1           │  │
      │  (Eurorack 2x5)    │  │
      ├────────────────────┤ ─┤
      │    ○ MH2 (M3)      │  │ 95mm
      └────────────────────┘ ─┴─ 100mm

Detailed Placement Coordinates

Modules (Hand-solder)

Ref	Component	Center X	Center Y	Rotation
MOD2	OLED 128x32	14.0	17.5	0°
MOD1	RP2040-Zero	14.0	46.5	0°

User Interface

Ref	Component	Center X	Center Y	Rotation
SW1	Tactile 6x6mm	14.0	31.5	0°
D2	Power LED	24.0	31.5	0°
R2	LED resistor 1K	24.0	36.0	90°

Connectors

Ref	Component	Center X	Center Y	Rotation
J2	Thonkiconn TRIG	7.0	83.0	0°
J3	Thonkiconn RETURN	21.0	83.0	0°
J1	2x5 Eurorack	14.0	92.0	0°

Power Section (Back side recommended)

Ref	Component	Center X	Center Y	Rotation	Side
D1	SS14 Schottky	7.0	65.0	0°	Back
U1	AMS1117-3.3	14.0	65.0	0°	Back
C1	10uF input	10.0	60.0	0°	Back
C2	10uF output	18.0	60.0	0°	Back
C3	100nF output	21.0	60.0	0°	Back

Signal Conditioning

Ref	Component	Center X	Center Y	Rotation	Side
U2	74LVC1G17	7.0	72.0	0°	Front
C4	100nF (U2)	7.0	68.0	0°	Front
R3	100R trig	7.0	76.0	90°	Front
U3	MCP6001	21.0	72.0	0°	Front
C5	100nF (U3)	21.0	68.0	0°	Front
R4	10K input	21.0	76.0	90°	Front
R5	10K divider	18.0	76.0	90°	Front
R6	22K divider	18.0	72.0	90°	Front
D3	BAT54 clamp	24.0	70.0	90°	Front
D4	BAT54 clamp	24.0	74.0	90°	Front

Button

Ref	Component	Center X	Center Y	Rotation
R1	10K pullup	10.0	35.0	0°

Routing Guidelines

Net Classes

Class	Width	Clearance	Via Drill
Default	0.25mm	0.2mm	0.3mm
Power	0.5mm	0.3mm	0.4mm
Signal	0.2mm	0.2mm	0.3mm

Power Routing

1. +12V path: J1 pin 4 → D1 → C1 → U1 VIN
2. +3.3V path: U1 VOUT → C2/C3 → distribute to all ICs
3. GND: Use ground pour on back layer, via stitch near decoupling caps

Signal Routing Priority

1. I2C (SDA/SCL): Keep short, parallel, 0.5mm spacing
2. TRIG_OUT: Direct from RP2040 GP2 → U2 → R3 → J2
3. RETURN_IN: J3 → R4 → divider → U3 → RP2040 GP3
4. BTN: RP2040 GP4 → R1 → SW1 → GND

Ground Plane

• Fill back copper with GND zone
• Via stitch every 5-10mm
• Keep clear around power input for thermal relief
• Connect GND pins of J2/J3 directly to plane

Design Rules (PCBWay Compatible)

Parameter	Value
Min trace width	0.15mm (0.2mm preferred)
Min clearance	0.15mm (0.2mm preferred)
Min via drill	0.3mm
Min via diameter	0.6mm
Min hole size	0.3mm
Min annular ring	0.15mm

Silkscreen

Front

• Component references (small, 0.8mm text)
• Jack labels: "TRIG" and "RETURN"
• "SN-L00 v0.1" at bottom
• "SubModular" at top

Back

• "SN-L00" centered
• Pin 1 indicators for ICs
• Polarity markers for D1, power header
• "git.sub-net.at/submodular/SN-L00"

Gerber Output

When exporting for PCBWay:

Required files:
- F.Cu (Front copper)
- B.Cu (Back copper)
- F.SilkS (Front silkscreen)
- B.SilkS (Back silkscreen)
- F.Mask (Front soldermask)
- B.Mask (Back soldermask)
- Edge.Cuts (Board outline)
- *.drl (Drill file)

Settings:
- Format: Gerber X2
- Drill: Excellon
- Units: mm
- Coordinate format: 4.6

Assembly Notes

1. PCBWay can assemble all SMD parts on both sides
2. Hand-solder: MOD1 (RP2040-Zero), MOD2 (OLED)
3. Jacks (J2, J3) can be assembled or hand-soldered
4. Power header (J1) usually hand-soldered for alignment

Checking Before Order

• DRC passes with no errors
• All nets connected (no airwires)
• Mounting holes align with panel
• Jacks align with panel holes
• Power header polarity marked
• Silkscreen readable and not over pads
• Ground plane connected properly