Vca as3360-circuit

Eurorack Modules

A collection of Eurorack module designs using KiCad. Each module has separate KiCad projects for the circuit PCB and the front panel.

Modules

daisy-seed-multi — Digital Multi-Purpose Module

• Core: Electrosmith Daisy Seed
• Description: Programmable digital module — function determined by firmware (oscillator, effects, sequencer, etc.)
• Based on: fablabnk/DaisyDelayHardware (KiCad 6+ project)
  • Includes Eurorack power, audio I/O with level shifting, CV inputs, pots, and custom footprints
  • See notes_schematic.md and notes_pcb.md for design rationale

vco-as3340 — Voltage Controlled Oscillator

• Core IC: AS3340 (CEM3340 clone)
• Reference design: Eddy Bergman's Digisound 80 AS3340 VCO
  • Blog: https://www.eddybergman.com/2020/01/synthesizer-build-part-18-really-good.html
• Based on: markthompson117/DigiSound80VCO (KiCad 6+ project)
  • Includes schematic and stripboard-to-PCB layout adaptation

vcf-as3320 — Voltage Controlled Filter

• Core IC: AS3320 (CEM3320 clone)
• Reference design: hermflink's 3320VCF
• Based on: hermflink/3320VCF (GPL-3.0 license, legacy KiCad format)
  • ⚠️ Legacy KiCad format (.sch/.pro) — open in KiCad 8 to auto-convert to modern format
  • Multimode filter: 24dB LP, 12dB BP, 6dB HP+18dB LP, 6dB LP+6dB HP+12dB LP
  • Designed for ±15V but works with ±12V

vca-as3360 — Voltage Controlled Amplifier

• Core IC: AS3360 (CEM3360 clone, dual VCA)
• Reference design: Kassutronics Dual VCA / LMNC 1181
• Based on: EchelonForce/vca_as3360 (CC-BY-NC-SA, KiCad 6+ project)
  • Hierarchical schematic (input block, output block, VCO block sub-sheets)
  • Includes front panel designs (FreeCAD .FCStd, DXF, SVG, PDF, and STEP files)

adsr-as3310 — ADSR Envelope Generator

• Core IC: AS3310 (CEM3310 clone)
• Reference design: Eddy Bergman's Digisound 80 ADSR
  • Blog: https://www.eddybergman.com/2020/05/synthesizer-build-part-33-digisound-80.html
• Based on: DIYSynthMNL/Eurorack-3310-ADSR (KiCad 6+ project)
  • Single-channel Eurorack ADSR with multiple schematic revisions included

Project Structure

Each module folder contains two KiCad projects:

• circuit/ — main electronics PCB
• panel/ — front panel PCB (for PCB-based panels)

The VCF uses legacy KiCad format and should be opened in KiCad 8 for automatic conversion.

Getting Started: Schematic to PCB Workflow

If you're new to KiCad, here's the recommended step-by-step process for turning a schematic into a finished PCB layout.

1. Review and Edit the Schematic

Open the .kicad_sch file in KiCad's Schematic Editor.

• Read through the circuit and make sure you understand what each section does. The reference design blog posts (linked above) are invaluable for this.
• Make any changes you want — swap component values, add/remove jacks, change pot tapers, etc.
• Assign footprints to every component (Tools → Assign Footprints). Each symbol needs a physical footprint that matches the real part you'll solder. For example:
  • Resistors → Resistor_THT:R_Axial_DIN0207_L6.3mm_D2.5mm_P10.16mm_Horizontal (typical through-hole)
  • DIP ICs → Package_DIP:DIP-16_W7.62mm (check your IC's pin count)
  • 3.5mm jacks → Connector_Audio:Jack_3.5mm_QingPu_WQP-PJ398SM_Vertical (Thonkiconn, the Eurorack standard)
  • Potentiometers → Potentiometer_THT:Potentiometer_Alpha_RD901F-40-00D_Single_Vertical
• Run Electrical Rules Check (Inspect → Electrical Rules Check) and fix any errors before proceeding.

2. Import Components into the PCB Editor

Open the PCB Editor (.kicad_pcb) and press F8 (or Tools → Update PCB from Schematic).

• This imports all your components as a pile of footprints with a "rats nest" of thin lines showing which pads need to be connected.
• Click OK to accept — don't worry, it looks like a mess at first. That's normal.

3. Define the Board Outline

Before placing components, draw the board outline on the Edge.Cuts layer.

• For Eurorack, the board height is 128.5mm (the 3U standard).
• Board width depends on your module's HP: 1 HP = 5.08mm. Common sizes:
  • 8 HP = 40.64mm
  • 10 HP = 50.80mm
  • 12 HP = 60.96mm
  • 14 HP = 71.12mm
• Use Place → Rectangle on the Edge.Cuts layer, or draw lines with the Draw Line tool.
• Add mounting holes at the standard Eurorack positions (3mm holes, 3.2mm from the top/bottom edges, 7.5mm from the left/right edges).

4. Place Components — The Most Important Step

Good placement is 90% of a good PCB. Take your time here.

General strategy:

1. Start with connectors and mechanical parts — place the Eurorack power header, jacks, pots, and switches first. These are constrained by the front panel layout and physical access.
2. Group related components together — keep each functional block (e.g., the expo converter, the waveform shapers, the output buffers) in its own area.
3. Follow the signal flow — arrange components so the signal path flows logically across the board (typically left-to-right or top-to-bottom). This makes routing easier and reduces noise.
4. Keep the main IC central — the AS3340/AS3320/AS3360/AS3310 should be near the middle of its associated circuitry.
5. Place decoupling capacitors right next to their IC's power pins — this is critical for noise performance. Within 5mm, as close as physically possible.

Analog audio tips:

• Keep audio signal traces away from digital signals and power traces.
• Keep input and output sections on opposite sides of the board to prevent feedback.
• Leave room for a ground plane (see step 6).

5. Route the Traces

Now connect all the pads according to the rats nest lines.

• Press X to start routing a trace. KiCad's interactive router will push other traces out of the way.
• Recommended trace widths:
  • Signal traces: 0.25–0.3mm (fine for audio and CV)
  • Power traces (+12V, -12V): 0.5–0.8mm (carry more current)
  • Ground: 0.5mm+ or use a ground plane (see below)
• Route critical signals first:
  1. Ground connections
  2. Power (+12V, -12V)
  3. Audio signal paths (keep these short and direct)
  4. CV and control signals
• Use 45° angles (KiCad's default) — avoid 90° corners on signal traces.
• Use vias to switch between front and back copper layers when traces need to cross.
• If you get stuck on a difficult route, try moving components slightly — often a small placement adjustment makes routing much easier.

6. Add a Ground Plane

A ground plane dramatically improves noise performance for analog audio circuits.

• Select the back copper layer (B.Cu)
• Place → Add Filled Zone → select the GND net → draw a rectangle covering the entire board
• Press B to fill the zone
• This connects all ground pads through a continuous copper pour, reducing ground loops and EMI.
• You can add a ground plane on the front (F.Cu) too, but leave enough clearance around signal traces.

7. Run Design Rule Check (DRC)

Before ordering, run Inspect → Design Rules Check to catch:

• Unconnected nets (missed connections)
• Clearance violations (traces too close together)
• Missing footprints
• Courtyard overlaps (components physically overlapping)

Fix every error. Warnings can sometimes be acceptable — review them individually.

8. Generate Manufacturing Files

When your layout is complete and DRC passes:

1. Gerber files: File → Fabrication Outputs → Gerbers — these are what the PCB manufacturer needs
   • Include: F.Cu, B.Cu, F.SilkS, B.SilkS, F.Mask, B.Mask, Edge.Cuts
   • Also generate the drill file (File → Fabrication Outputs → Drill Files)
2. Review in Gerber Viewer: Inspect → Gerber Viewer or use an online viewer like Tracespace to double-check before ordering
3. Upload to your fab — JLCPCB, PCBWay, OSH Park, etc. all accept KiCad Gerber output directly

9. Front Panel PCB

Each module also has a panel/ folder for designing the front panel as a PCB:

• Create a board outline matching the module's HP width × 128.5mm height
• Add cutouts for jacks, pots, switches, and LEDs as mounting holes or non-plated through-holes (NPTH)
• Add labels and graphics on the F.SilkS (silkscreen) layer for a professional look
• Standard Eurorack mounting slots: oval holes (3.2mm × 4mm) at top and bottom, centered at 3mm from each horizontal edge
• Order with a different solder mask color than your circuit board for visual distinction (e.g., black panel, green circuit board)

Using Freerouting for Auto-Routing (Optional)

KiCad doesn't have a built-in autorouter, but you can use Freerouting:

1. In KiCad PCB Editor: File → Export → Specctra DSN
2. Open the .dsn file in Freerouting → click "Autoroute"
3. Export the result as a .ses (Specctra Session) file
4. Back in KiCad: File → Import → Specctra Session

Caveat: Autorouting works best for digital boards. For analog audio modules, you'll likely want to hand-route critical audio paths and use the autorouter only for less-sensitive connections like power distribution and LED indicators.

Notes

• All modules target standard Eurorack format (3U height, ±12V power)
• Panel width (HP) to be determined per module
• Source projects are used as starting points — modify and adapt as needed