sistemas-cibernetico-fisicos/docs/EASYEDA_PRO_TO_KICAD_GUIDE.md

Exporting EasyEDA Pro Projects to KiCad

Document ID: SE-HW-GUIDE-001
Version: 1.0
Date: 2026-05-10
Audience: Hardware Team

---

1. Overview

This guide covers exporting a full EasyEDA Pro project (schematics + PCB) to KiCad 8.x format for version control in savearth-hw-project/kicad/.

---

2. Prerequisites

Tool	Version	Notes
EasyEDA Pro	Latest (Web or Desktop)	Desktop app recommended for large projects
KiCad	8.0+	Install from kicad.org
easyeda2kicad (optional)	Latest	Python CLI for component library conversion

Install the Python converter (for component libraries):

pip install easyeda2kicad

---

3. Method A: Native EasyEDA Pro Export (Recommended)

EasyEDA Pro has built-in KiCad export since late 2024.

3.1 Export Schematic

1. Open your project in EasyEDA Pro
2. Go to File → Export → KiCad...
3. In the export dialog:
   • Format: KiCad 8 (.kicad_sch)
   • Include: ☑ Schematics ☑ Symbols
   • Output directory: Choose a temporary folder
4. Click Export
5. You will get:
   • *.kicad_sch — Schematic file(s)
   • *.kicad_sym — Symbol library

3.2 Export PCB Layout

1. Open the PCB editor in EasyEDA Pro
2. Go to File → Export → KiCad...
3. In the export dialog:
   • Format: KiCad 8 (.kicad_pcb)
   • Include: ☑ PCB ☑ Footprints ☑ 3D Models
   • Output directory: Same temporary folder
4. Click Export
5. You will get:
   • *.kicad_pcb — PCB layout
   • *.kicad_mod — Footprint library
   • *.step / *.wrl — 3D models (if available)

3.3 Create KiCad Project

1. Open KiCad 8
2. File → New Project...
3. Navigate to savearth-hw-project/kicad/
4. Name: savearth-ssm-01
5. This creates:
   • savearth-ssm-01.kicad_pro — Project file
   • savearth-ssm-01.kicad_sch — Empty schematic
   • savearth-ssm-01.kicad_pcb — Empty PCB
6. Replace the empty .kicad_sch and .kicad_pcb with the exported files
7. Copy symbol and footprint libraries to savearth-hw-project/kicad/libs/

3.4 Verify Import

1. Open the project in KiCad
2. Check schematic:
   • All components should be present
   • Net names should be preserved
   • Run ERC (Electrical Rule Check)
3. Check PCB:
   • All footprints placed correctly
   • Copper traces intact
   • Run DRC (Design Rule Check)
   • Verify layer mapping (see Section 5)

---

4. Method B: JSON Intermediate Format

If the native export has issues, use the JSON intermediate format:

4.1 Export from EasyEDA Pro as JSON

1. In EasyEDA Pro, go to File → Export → EasyEDA...
2. Export as .json format (EasyEDA native format)
3. Save the JSON file(s)

4.2 Convert JSON to KiCad

Use the community easyeda2kicad tool:

# Convert component library (symbols + footprints)
easyeda2kicad --full \
  --lcsc_id C2296507 \
  --output ./kicad/libs/

# For a full project, you may need to convert each component's
# LCSC part number individually

Warning

The easyeda2kicad tool converts individual components (by LCSC part number), not full projects. For full project conversion, Method A (native export) is strongly recommended.

4.3 Alternative: LCSC Component Converter

For individual components that fail to export:

# Export a specific component by LCSC number
easyeda2kicad --full --lcsc_id C12345 --output ./kicad/libs/

# This creates:
# ./kicad/libs/C12345.kicad_sym   (symbol)
# ./kicad/libs/C12345.kicad_mod   (footprint)
# ./kicad/libs/C12345.step        (3D model, if available)

---

5. Layer Mapping (EasyEDA Pro → KiCad)

EasyEDA Pro and KiCad use different layer names. Verify these mappings after import:

EasyEDA Pro Layer	KiCad Layer	Notes
TopLayer	F.Cu	Front copper
BottomLayer	B.Cu	Back copper
Inner1	In1.Cu	Inner copper 1
Inner2	In2.Cu	Inner copper 2
TopSilkLayer	F.SilkS	Front silkscreen
BottomSilkLayer	B.SilkS	Back silkscreen
TopPasteSolderLayer	F.Paste	Front solder paste
BottomPasteSolderLayer	B.Paste	Back solder paste
TopSolderMaskLayer	F.Mask	Front solder mask
BottomSolderMaskLayer	B.Mask	Back solder mask
BoardOutLine	Edge.Cuts	Board outline
Multi-Layer	*.Cu	All copper layers (vias)
Document	Cmts.User	Comments / documentation
Mechanical	User.1	Mechanical outlines

---

6. Common Issues & Fixes

6.1 Missing Footprints

Symptom: PCB opens but some footprints show as "not found"

Fix:

1. Ensure the exported .kicad_mod library is in kicad/libs/
2. In KiCad: Preferences → Manage Footprint Libraries...
3. Add the library path: ${KIPRJMOD}/libs/savearth.pretty

6.2 Net Name Mismatches

Symptom: DRC shows unconnected nets that should be connected

Fix:

1. Compare net names in schematic vs PCB
2. EasyEDA sometimes uses NetLabel_X format
3. Manually rename in KiCad schematic editor if needed
4. Run Tools → Update PCB from Schematic to re-sync

6.3 Copper Fill / Ground Pour Issues

Symptom: Ground pour zones don't render correctly

Fix:

1. Select the zone in KiCad PCB editor
2. Edit → Edit Zone Properties...
3. Set correct net (usually GND)
4. Edit → Fill All Zones (press B)

6.4 Component Values Not Imported

Symptom: Resistors/capacitors show generic values

Fix:

1. Open schematic in KiCad
2. Edit → Edit Symbol Fields...
3. Cross-reference with the EasyEDA Pro BOM
4. Update Value field for each component

6.5 3D Models Not Loading

Symptom: 3D viewer shows missing models

Fix:

1. Copy .step and .wrl files to kicad/libs/3d/
2. In Footprint Editor: Edit Footprint Properties → 3D Models
3. Update path to: ${KIPRJMOD}/libs/3d/component_name.step

---

7. Post-Import Checklist

After importing into KiCad, verify:

• All components present in schematic (compare component count with EasyEDA)
• All nets correctly named
• ERC passes with 0 errors (warnings acceptable)
• PCB footprints match schematic (run Update PCB from Schematic)
• DRC passes with 0 errors
• Board outline (Edge.Cuts) is correct
• Drill files can be generated (plot test)
• BOM can be exported from KiCad
• 3D model renders correctly in 3D Viewer

---

8. Repository Structure

After export, the savearth-hw-project/kicad/ directory should look like:

kicad/
├── savearth-ssm-01.kicad_pro          # KiCad project file
├── savearth-ssm-01.kicad_sch          # Schematic
├── savearth-ssm-01.kicad_pcb          # PCB layout
├── libs/
│   ├── savearth.kicad_sym             # Symbol library
│   ├── savearth.pretty/               # Footprint library
│   │   ├── ESP32-S3-WROOM.kicad_mod
│   │   ├── USB-C-Connector.kicad_mod
│   │   └── ...
│   └── 3d/                            # 3D models
│       ├── ESP32-S3-WROOM.step
│       └── ...
├── gerber/                            # Generated Gerber files (for fab)
└── bom/                               # Bill of Materials exports

---

9. Git Configuration for KiCad

Add to savearth-hw-project/.gitattributes:

# KiCad files — treat as text for better diffs
*.kicad_sch text
*.kicad_pcb text
*.kicad_pro text
*.kicad_sym text
*.kicad_mod text

# Binary files
*.step binary
*.wrl binary

Tip

KiCad 8 uses S-expression text format for all design files, making them diff-friendly in Git. Always commit after meaningful design changes with descriptive messages.

---

This guide is maintained in savearth-hw-project/docs/. Updated as EasyEDA Pro export features evolve.