# 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](https://www.kicad.org/download/) |
| **easyeda2kicad** (optional) | Latest | Python CLI for component library conversion |

Install the Python converter (for component libraries):
```bash
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:

```bash
# 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:

```bash
# 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.*