KiCad Project Workflow

Complete workflow for creating a PCB design in KiCad, from schematic to manufacturing files.

Prerequisites

CRITICAL: Before starting, ensure your KiCad project files are located at the repository root:

zudo-pd/          ← Repository root
├── zudo-pd.kicad_pro       ← Project file must be here
├── zudo-pd.kicad_sch       ← Schematic file
├── zudo-pd.kicad_pcb       ← PCB file (created later)
└── footprints/             ← Footprint library
    └── kicad/
        └── zudo-power.pretty/

The ${KIPRJMOD} variable in KiCad points to the directory containing the .kicad_pro file. If your project is in a subdirectory (like kicad/ or pcb/), relative paths to footprints and libraries won't resolve correctly.

Overview

KiCad uses a modular workflow where you work with different editors in sequence:

1. Symbol Editor - Create/import schematic symbols

2. Schematic Editor - Draw circuit diagrams

3. Footprint Editor - Create/import PCB footprints

4. PCB Editor - Layout the physical board

5. Manufacturing Output - Generate Gerber files

Stage 1: Symbol Management

1.1 Check Existing Libraries

Before creating custom symbols, check if they already exist in KiCad's standard libraries:

Common libraries for this project:

• Device - Resistors, capacitors, inductors, diodes, LEDs

• Regulator_Linear - LM78xx, LM79xx series

• Regulator_Switching - LM2596, buck/boost converters

• Connector - USB connectors, power jacks, headers

• power - GND, VCC, voltage symbols

To check:

1. Open Symbol Editor

2. File → Add Library... → Browse standard KiCad libraries

3. Search for your part number or category

1.2 Import Symbols from Standard Libraries

For parts already in KiCad libraries:

1. Open Schematic Editor

2. Press A (Add Symbol)

3. Search by part name (e.g., "LM7812", "USB_C_Receptacle")

4. Browse by library category if unsure

1.3 Create Custom Symbols

For parts NOT in standard libraries (like STUSB4500, specialized ICs):

Method 1: Import from EasyEDA/LCSC

Use easyeda2kicad.py to download both symbols and footprints:

# Download symbol + footprint for STUSB4500 (LCSC ID: C2678061)
easyeda2kicad --lcsc_id C2678061 --symbol --footprint

# Files saved to:
# ~/Documents/Kicad/easyeda2kicad/easyeda2kicad.pretty/  (footprints)
# ~/Documents/Kicad/easyeda2kicad/easyeda2kicad.kicad_sym (symbols)

Method 2: Manual Creation

1. Open Symbol Editor

2. File → New Library... → Create project-specific library (e.g., zudo-power.kicad_sym)

3. Create New Symbol

4. Define:

• Pin numbers and names (from datasheet)

• Pin electrical types (input, output, power, passive)

• Symbol shape (rectangle, specialized)

• Reference designator (U, R, C, J, etc.)

Best practices:

• Match datasheet pin numbering exactly

• Use descriptive pin names (VIN, VOUT, FB, EN, etc.)

• Set correct electrical types for ERC (Electrical Rule Check)

• Add datasheet link in symbol properties

Stage 2: Schematic Creation

2.1 Create New Schematic

1. Open Schematic Editor (zudo-pd.kicad_sch)

2. Set up page properties:

• Title: "USB-PD Modular Synth Power Supply"

• Revision: v1.0

• Date: (automatic)

• Company/Organization (optional)

2.2 Place Symbols

1. Press A to add symbols

2. Search and place all components

3. Use logical groupings:

• USB-PD input stage (left side)

• DC-DC converters (center)

• Linear regulators (right)

• Output connectors (far right)

Recommended layout flow:

Left to Right = Signal Flow
USB-C Input → DC-DC Conversion → Linear Regulation → Outputs

2.3 Wire Connections

1. Press W to start wiring

2. Click start point → Click end point

3. Use labels for:

• Power nets: +15V, +13.5V, +12V, +5V, -12V, -15V

• Ground: GND (use power symbol)

• Signal names: PG (Power Good), EN (Enable), FB (Feedback)

Best practices:

• Use net labels instead of long wires across the page

• Group related components close together

• Keep power flow left-to-right, top-to-bottom

• Add No Connect flags (X) to unused pins

2.4 Add Power Symbols

1. Press P to add power symbols

2. Add for each voltage rail:

• +12V, +5V, -12V (outputs)

• +15V, +13.5V, -13.5V (intermediate)

• GND (ground reference)

2.5 Add Values and References

For each component:

1. Select component

2. Press E to edit properties

3. Set:

• Reference (auto-numbered: U1, R1, C1, etc.)

• Value (10µF, 5.1kΩ, LM7812, etc.)

• Footprint (assigned in next step)

• Datasheet URL (optional but recommended)

2.6 Annotate Schematic

Auto-number all reference designators:

1. Tools → Annotate Schematic

2. Select "Use entire schematic" (for multi-sheet projects)

3. Click "Annotate"

Result: R?, C?, U? become R1, R2, C1, C2, U1, U2, etc.

2.7 Electrical Rules Check (ERC)

Before proceeding to PCB:

1. Inspect → Electrical Rules Checker

2. Run ERC

3. Fix all errors:

• Unconnected pins

• Power pins not driven

• Conflicting outputs

• Missing power connections

Stage 3: Footprint Assignment

3.1 Import Footprints

For JLCPCB-compatible parts:

See KiCad Parts Download Guide for detailed instructions.

Quick workflow:

# Download footprint by LCSC ID
easyeda2kicad --lcsc_id C970725 --footprint

# Copy to project directory
cp ~/Documents/Kicad/easyeda2kicad/easyeda2kicad.pretty/*.kicad_mod ./footprints/kicad/

3.1a Add Footprint Library to KiCad

IMPORTANT: Before adding the footprint library, ensure your KiCad project (.kicad_pro file) is located in the repository root directory. The ${KIPRJMOD} variable points to the project file location, so if your project is in a subdirectory (like kicad/), the relative paths won't resolve correctly.

Project structure:

zudo-pd/          ← Repository root
├── zudo-pd.kicad_pro       ← KiCad project file should be here
├── zudo-pd.kicad_sch       ← Schematic file
├── zudo-pd.kicad_pcb       ← PCB file
└── footprints/
    └── kicad/
        └── zudo-power.pretty/   ← Footprint library
            ├── C0603.kicad_mod
            ├── C0805.kicad_mod
            └── ... (37 footprints)

Steps to add footprint library:

1. Open Preferences → Manage Footprint Libraries

• From main KiCad window (NOT Symbol Editor)

• Or from PCB Editor: Preferences → Manage Footprint Libraries

2. Click "Project Specific Libraries" tab (at bottom)

3. Add new library:

• Click folder icon (➕) to add library

• Set values:

  • Nickname: zudo-pd (or any name you prefer)

  • Library Path: ${KIPRJMOD}/footprints/kicad/zudo-power.pretty

  • Library Format: KiCad

  • Options: (leave blank)

4. Click OK

Example configuration:

The dialog should show:

• Library nickname: zudo-pd

• Library path: ${KIPRJMOD}/footprints/kicad/zudo-power.pretty

• At the bottom, "Available path substitutions" shows the resolved path

Verify the library loaded:

1. Open Footprint Editor (from main KiCad window)

2. Check left panel - you should see zudo-pd library

3. Click on it to expand and browse 37 footprints

4. You should see footprints like:

• C0603, C0805 (capacitors)

• TO-252-3, TO-263-2 (IC packages)

• SOP-8, SSOP-10 (IC packages)

• Component-specific footprints

Troubleshooting:

• Library appears empty: Verify the path points to zudo-power.pretty directory (not .pretty or other directories)

• Path not found: Check that ${KIPRJMOD} resolves correctly by looking at "Available path substitutions" at bottom of dialog

• Wrong symbols showing: You opened Symbol Libraries instead of Footprint Libraries - close and reopen the correct dialog

3.2 Assign Footprints to Symbols

1. In Schematic Editor: Tools → Assign Footprints

2. For each component, select appropriate footprint:

• Resistors/Capacitors: 0805, 1206 (SMD sizes)

• ICs: Match package type from datasheet (SOIC-8, SOT-23-6, etc.)

• Connectors: Match mechanical dimensions exactly

• Large components: Verify pad sizes for current rating

Example assignments:

• LM7812 → TO-252-2 (DPAK)

• LM2596S → TO-263-5 (D2PAK)

• STUSB4500 → QFN-24 (from LCSC)

• 10µF capacitor → C_0805_2012Metric

• 5.1kΩ resistor → R_0805_2012Metric

3.3 Verify Footprint Assignments

1. Check that ALL components have footprints assigned (no "No Footprint" entries)

2. Verify footprint sizes match your requirements:

• Small passives: 0805 or 1206 (easy hand soldering)

• ICs: Match JLCPCB assembly capabilities

• Connectors: Match mechanical specs exactly

Stage 4: PCB Layout

4.1 Generate Netlist and Import to PCB

1. In Schematic Editor: Tools → Update PCB from Schematic (F8)

2. Click "Update PCB"

3. PCB Editor opens with all components loaded

First import: Components appear in a cluster, ready to be positioned

4.2 Set Board Dimensions

1. Select Edge.Cuts layer

2. Draw board outline:

• Press Ctrl+Shift+P for polygon tool

• Draw rectangle or custom shape

• Recommended: Start with 100mm × 80mm for this project

4.3 Place Components

Strategic placement:

1. Input stage (left):

• USB-C connector on board edge

• CH224Q near connector

• Input capacitors near CH224Q

2. DC-DC stage (center):

• LM2596S converters in row

• Inductors next to each converter

• Output capacitors after inductors

3. Linear regulators (right of center):

• LM7812, LM7805, LM7912 in row

• Input/output capacitors adjacent

4. Output connectors (right edge):

• Power headers on board edge

• Fuses before output

• TVS diodes near output

Best practices:

• Keep signal paths short (especially high-current paths)

• Place decoupling capacitors close to IC power pins

• Orient components for logical layout

• Leave space for heat dissipation (regulators, DC-DC)

• Group by function, not just by type

4.4 Route Traces

Layer strategy:

• F.Cu (Top layer): Power traces, signal routing

• B.Cu (Bottom layer): Ground plane + additional routing

Trace widths (for 1oz copper):

• Power traces (1A+): 0.5mm minimum, 1.0mm recommended

• Signal traces: 0.25mm minimum, 0.3mm recommended

• Ground/return: Wide as possible, or use ground plane

Routing order:

1. Route power traces first (+15V, +12V, +5V, -12V)

2. Route critical signals (feedback, enable pins)

3. Route remaining connections

4. Add ground plane on bottom layer (Fill Zone)

Tools:

• Press X to start routing

• Press V to add via (switch layers)

• Press D to drag component while maintaining connections

4.5 Add Ground Plane

1. Select B.Cu layer

2. Press Ctrl+Shift+Z to add filled zone

3. Draw zone around entire board

4. Set net: GND

5. Press B to rebuild all zones

4.6 Design Rule Check (DRC)

Before manufacturing:

1. Inspect → Design Rules Checker

2. Run DRC

3. Fix all errors:

• Trace clearance violations

• Unconnected nets

• Board outline issues

• Silkscreen over pads

Stage 5: Manufacturing Output

5.1 Generate Gerber Files

1. File → Fabrication Outputs → Gerbers (.gbr)

2. Settings:

• Include layers: F.Cu, B.Cu, F.Mask, B.Mask, F.Silkscreen, B.Silkscreen, Edge.Cuts

• Coordinate format: 4.6, unit mm

• Check "Use Protel filename extensions"

3. Click "Plot"

5.2 Generate Drill Files

1. File → Fabrication Outputs → Drill Files (.drl)

2. Settings:

• Drill units: Millimeters

• Drill map: PostScript or PDF (for verification)

3. Click "Generate Drill File"

5.3 Generate BOM (Bill of Materials)

1. In Schematic Editor: File → Fabrication Outputs → BOM

2. Use built-in generator or:

• Export to CSV

• Use external tool (KiBoM, InteractiveHtmlBom)

For JLCPCB assembly:

• Must include: Reference, Value, Footprint, LCSC Part Number

• Export as CSV format

• Match JLCPCB template exactly

5.4 Generate Pick-and-Place File

For SMT assembly:

1. File → Fabrication Outputs → Component Placement (.pos)

2. Format: CSV

3. Units: Millimeters

4. Includes: Reference, X, Y, Rotation, Layer

5.5 Verify with Gerber Viewer

1. Open GerbView (included with KiCad)

2. Load all Gerber files + drill file

3. Check:

• Board outline correct

• All pads visible

• Silkscreen readable (not over pads)

• Drill holes aligned with pads

• Layers aligned correctly

Stage 6: Order from JLCPCB

6.1 Prepare Files

Create ZIP archive with:

• All Gerber files (.gbr)

• Drill file (.drl)

• BOM (CSV format, JLCPCB template)

• Pick-and-place file (CSV format)

# Example ZIP structure
gerbers.zip
├── F_Cu.gbr
├── B_Cu.gbr
├── F_Mask.gbr
├── B_Mask.gbr
├── F_Silkscreen.gbr
├── B_Silkscreen.gbr
├── Edge_Cuts.gbr
└── drill.drl

bom_jlcpcb.csv
cpl_jlcpcb.csv

6.2 Upload and Configure

1. Go to jlcpcb.com

2. Upload gerbers.zip

3. Configure:

• PCB quantity: 5 (minimum)

• PCB thickness: 1.6mm (standard)

• Surface finish: HASL (lead-free) or ENIG (better quality)

• Copper weight: 1oz (standard for <3A)

4. Add SMT assembly service (optional):

• Upload BOM + CPL

• Review component placement

• Check part availability/substitutions

Workflow Summary

1. Symbol Editor
   ↓
2. Schematic Editor → [ERC Pass] → Assign Footprints
   ↓
3. Update PCB from Schematic
   ↓
4. PCB Editor → Place Components → Route → [DRC Pass]
   ↓
5. Generate Outputs (Gerber, Drill, BOM, CPL)
   ↓
6. Verify in GerbView
   ↓
7. Order from JLCPCB

Troubleshooting

Common Issues

Problem: Symbol not found when placing component

• Solution: Add library containing the symbol (Preferences → Manage Symbol Libraries)

Problem: Footprint assignment shows "No Footprint"

• Solution: Add footprint library (Preferences → Manage Footprint Libraries)

Problem: DRC shows "unconnected nets"

• Solution: Check for missing wires in schematic, or use "No Connect" flags

Problem: Gerber viewer shows misaligned layers

• Solution: Check drill origin settings, regenerate Gerbers with correct settings

Problem: JLCPCB BOM upload fails

• Solution: Verify CSV format matches template, check for special characters

Next Steps

After completing the KiCad workflow:

1. Documentation:

• Export circuit diagram as SVG (see Create Circuit SVG Files)

• Export footprint previews (see Create Footprint SVG Files)

• Update parts list with LCSC IDs

2. Testing plan:

• Order PCBs without assembly first

• Verify board dimensions and mounting holes

• Check component footprints with actual parts

• Then order with assembly

3. Version control:

• Commit KiCad project files (.kicad_pro, .kicad_sch, .kicad_pcb)

• Commit Gerber outputs for reference

• Tag release versions (v1.0, v1.1, etc.)

References

• KiCad Documentation

• KiCad Parts Download Guide

• JLCPCB SMT Assembly

• Create Footprint SVG Files