How to Convert Altium Files to KiCad: Complete Migration Guide for PCB Engineers

Converting Altium Designer projects to KiCad has become remarkably easier over the past few years. Whether you’re transitioning away from expensive licensing, collaborating with teams using open-source tools, or simply working with reference designs distributed in Altium format, KiCad now handles these imports with impressive fidelity.

Having worked through numerous Altium-to-KiCad migrations myself, I can tell you the process has matured significantly. KiCad 7 introduced native Altium import support, KiCad 8 expanded library compatibility, and KiCad 9 now supports complete project file imports. This guide walks you through every step of the conversion process, from understanding which files you need to verifying your converted design.

Why Convert Altium Projects to KiCad?

The reasons engineers convert Altium designs to KiCad vary widely. Some are driven by budget constraints—Altium Designer subscriptions aren’t cheap, and KiCad offers professional-grade capabilities at zero cost. Others need to work with reference designs from semiconductor manufacturers who distribute their evaluation boards in Altium format.

Common scenarios driving Altium to KiCad conversion include:

Cost Reduction: Small companies and individual engineers often find Altium’s pricing prohibitive. KiCad provides a fully functional PCB design suite without licensing fees, making it attractive for startups and hobbyists scaling to production.

Collaboration Requirements: When working with clients or partners who use KiCad, receiving an Altium project creates friction. Converting to a common format eliminates compatibility headaches during design reviews and modifications.

Reference Design Access: Many chip vendors provide evaluation board designs in Altium format. Engineers using KiCad need conversion capability to leverage these validated designs as starting points.

Tool Evaluation: Engineers evaluating whether KiCad can replace Altium in their workflow often import existing projects to assess how well their designs translate to the new environment.

Understanding Altium Designer File Types

Before starting any conversion, you need to know which files matter. Altium Designer projects consist of multiple file types, each serving a specific purpose.

File Extension	Description	KiCad Import Support
.PrjPcb	Project file	Yes (KiCad 9.0.3+)
.SchDoc	Schematic document	Yes (KiCad 7+)
.PcbDoc	PCB layout document	Yes (KiCad 7+)
.SchLib	Schematic symbol library	Yes (KiCad 8+)
.PcbLib	PCB footprint library	Yes (KiCad 8+)
.IntLib	Integrated library	Yes (KiCad 8+)
.OutJob	Output job configuration	No
.PrjPcbStructure	Project structure	No

The essential files for conversion are your schematic documents (.SchDoc), PCB layout (.PcbDoc), and any custom libraries the project references. Project files (.PrjPcb) can now be imported directly in KiCad 9.0.3 and later, significantly streamlining the workflow.

KiCad Version Requirements for Altium Import

KiCad’s Altium import capabilities have evolved rapidly across recent versions. Using the latest stable release is strongly recommended for the best conversion results.

KiCad Version	Altium Support Level
KiCad 6.x and earlier	No native support (requires third-party tools)
KiCad 7.x	Schematic (.SchDoc) and PCB (.PcbDoc) import
KiCad 8.x	Added symbol library (.SchLib) and footprint library (.PcbLib, .IntLib) support
KiCad 9.x	Added project file (.PrjPcb) import with flat schematic support

If you’re running KiCad 6 or earlier, upgrade before attempting any Altium import. The improvement in import quality between versions is substantial, and older releases require third-party conversion tools that produce less reliable results.

Preparing Your Altium Project for Conversion

Proper preparation prevents most conversion failures. Spending fifteen minutes organizing your Altium project before import saves hours of troubleshooting afterward.

Pre-Conversion Checklist

Verify Project Integrity:

• Open the project in Altium Designer and run a full design rule check
• Ensure all schematic sheets link correctly to the PCB layout
• Confirm that component footprints are properly assigned

Library Organization:

• Locate all custom libraries your project uses
• Note the paths to .SchLib, .PcbLib, and .IntLib files
• Standard Altium libraries typically convert without issues

File Format Considerations:

• Altium supports both binary and ASCII file formats
• Binary format (.SchDoc, .PcbDoc) is standard and imports correctly
• ASCII format may provide better compatibility in edge cases

Multi-Sheet Designs:

• For hierarchical schematics, note the top-level sheet
• KiCad imports hierarchical designs correctly when you select the top sheet
• Flat (non-hierarchical) multi-sheet designs require KiCad 9.0.3+ for direct import

Taking notes on your layer stack configuration helps during the layer mapping step of the import process.

Method 1: Importing Altium Projects in KiCad 9

KiCad 9.0.3 introduced direct project import, which is the fastest method for complete migrations. This approach handles schematics, PCB layout, and libraries in a single operation.

Step-by-Step Project Import

Step 1: Launch the Import Wizard

Open KiCad’s Project Manager and navigate to File → Import Non-KiCad Project → Altium Project. This opens the project import dialog.

Step 2: Select Your Altium Project File

Browse to your Altium project folder and select the .PrjPcb file. Click Open to proceed.

Step 3: Choose Output Directory

Select an empty folder where KiCad should save the converted project files. Using an empty folder prevents any file conflicts and keeps your converted design organized.

Step 4: Configure Layer Mapping

The layer mapping dialog appears, showing Altium layers on one side and KiCad layers on the other. You have two options here:

• Auto-Match Layers: Click this button for automatic mapping. Works well for most standard designs.
• Manual Mapping: Adjust individual layer assignments if your design uses non-standard layer configurations.

Altium Layer	KiCad Equivalent
Top Layer	F.Cu
Bottom Layer	B.Cu
Mid Layer 1, 2, etc.	In1.Cu, In2.Cu, etc.
Top Overlay	F.SilkS
Bottom Overlay	B.SilkS
Top Solder	F.Mask
Bottom Solder	B.Mask
Top Paste	F.Paste
Bottom Paste	B.Paste
Keep-Out Layer	Edge.Cuts or User.Drawings
Mechanical 1-16	User.1 through User.9

Step 5: Execute Import

Click OK or Import to begin the conversion. KiCad processes the project and opens the converted files in an unsaved state.

Step 6: Save the Converted Project

Review the imported schematic and PCB, then save all files. The project is now native KiCad format and ready for editing.

Method 2: Importing Schematics and PCBs Separately

For KiCad 7 and 8 users, or when troubleshooting problematic conversions, importing schematics and PCB layouts separately provides more control.

Importing Altium Schematics into KiCad

1. Open KiCad’s Schematic Editor in standalone mode (launch Eeschema directly, not from the Project Manager)
2. Go to File → Import → Non-KiCad Schematic
3. Change the file filter to Altium Designer Schematic (*.SchDoc)
4. Select your schematic file and click Open
5. For hierarchical designs, select the top-level sheet—KiCad automatically imports sub-sheets

KiCad creates a project-specific symbol library containing all components from the imported schematic. This ensures your design remains self-contained.

Importing Altium PCB Layouts into KiCad

1. Open KiCad’s PCB Editor in standalone mode (launch Pcbnew directly)
2. Navigate to File → Import → Non-KiCad Board File
3. Change the file filter to Altium Designer PCB (*.PcbDoc)
4. Select your PCB file and click Open
5. Review any warnings displayed during import

The PCB import includes copper geometry, vias, component footprints, board outline, and in most cases, 3D models. Design rules do not transfer—you’ll need to recreate these in KiCad.

Linking Imported Files into a Project

After importing schematics and PCB separately:

1. Create a new KiCad project
2. Copy or move the imported schematic (.kicad_sch) and PCB (.kicad_pcb) files into the project folder
3. Add the files to your project through the Project Manager
4. Run Tools → Update PCB from Schematic to verify connectivity

Method 3: Using the altium2kicad Converter Tool

For legacy KiCad versions or when native import fails, the open-source altium2kicad tool provides an alternative conversion path.

Online Converter Option

The quickest approach for simple projects:

1. Visit www2.futureware.at/KiCad/
2. Create a ZIP file containing your .PcbDoc and .SchDoc files
3. Upload the ZIP (maximum 40MB file size)
4. Download the converted KiCad files
5. Open the resulting .pro file in KiCad

This online service handles basic conversions without requiring any local software installation.

Command-Line Tool Installation

For larger projects or offline use:

git clone https://github.com/thesourcerer8/altium2kicad/cd altium2kicadperl unpack.plperl convertschema.plperl convertpcb.pl

The command-line tool requires Perl and produces KiCad 5-compatible files. Results may need additional cleanup compared to KiCad’s native importer.

Importing Altium Libraries into KiCad

Component libraries often need separate handling, especially when planning ongoing KiCad use.

Direct Library Usage (Read-Only)

KiCad 8+ can use Altium libraries directly without conversion:

For Symbol Libraries (.SchLib):

1. Go to Preferences → Manage Symbol Libraries
2. Click the + icon to add a new library
3. Browse to your .SchLib file
4. Set Library Format to Altium
5. Assign a nickname and click OK

For Footprint Libraries (.PcbLib):

1. Go to Preferences → Manage Footprint Libraries
2. Click the + icon
3. Browse to your .PcbLib file
4. Set Library Format to Altium
5. Assign a nickname and click OK

Libraries loaded this way remain read-only. You can use the components but cannot edit them.

Converting Libraries to KiCad Format

For full editing capability:

1. Add the Altium library as described above
2. Select the library in the list
3. Click Migrate Libraries at the bottom of the dialog
4. Confirm the conversion
5. KiCad creates native .kicad_sym and .kicad_mod files

The migrated libraries are fully editable and no longer depend on the original Altium files.

Post-Import Verification Checklist

Never trust a conversion blindly. Always verify these critical elements before using an imported design.

Schematic Verification

• Component Count: Compare total component counts between Altium and KiCad
• Net Connectivity: Run ERC (Electrical Rule Check) and address all errors
• Symbol Appearance: Spot-check that symbols render correctly
• Pin Assignments: Verify critical component pin mappings
• Hierarchy: Confirm sheet-to-sheet connections for multi-page designs

PCB Layout Verification

• Board Outline: Ensure the board shape imported correctly
• Layer Count: Verify all copper layers exist and are properly ordered
• Component Placement: Check that components appear in correct positions
• Routing Integrity: Inspect critical traces, especially differential pairs
• Via Placement: Confirm vias transferred with correct sizes and positions
• Copper Pours: Re-pour all zones after import to ensure proper fill

Design Rule Check

Run KiCad’s DRC immediately after import:

1. Open the PCB Editor
2. Go to Inspect → Design Rules Checker
3. Click Run DRC
4. Address any violations—some may be false positives from conversion artifacts

Compare the violation count and types against DRC results from the original Altium project.

Common Altium to KiCad Conversion Issues

Based on community feedback and personal experience, these problems occur most frequently:

Missing 3D Models: While KiCad imports many 3D models successfully, some fail to transfer. STEP files generally work better than proprietary formats. Reassign missing models manually through the footprint properties.

Teardrop Artifacts: Altium’s teardrop feature sometimes creates DRC violations in KiCad. Consider removing teardrops in Altium before export, then re-adding them using KiCad’s teardrop extension after import.

Design Rules Not Imported: KiCad does not import Altium design rules. Recreate trace width rules, clearance constraints, and other DRC parameters manually. This is tedious but necessary for design integrity.

Flat Schematic Handling: KiCad versions before 9.0.3 don’t support flat (non-hierarchical) multi-sheet schematics. Each sheet must be imported individually and manually linked.

Mechanical Layer Mapping: Altium’s 16 mechanical layers don’t map directly to KiCad’s user layers. Verify critical mechanical information (assembly drawings, dimensions) transferred correctly.

Custom Pad Shapes: Complex pad geometries occasionally convert incorrectly. Inspect BGA footprints and connectors with unusual pad shapes carefully.

Useful Resources for Altium to KiCad Conversion

These resources provide additional help when tackling complex conversions:

Resource	URL	Description
KiCad Official Documentation	docs.kicad.org	Comprehensive import guides and troubleshooting
KiCad User Forum	forum.kicad.info	Community support for conversion issues
altium2kicad GitHub	github.com/thesourcerer8/altium2kicad	Open-source converter tool and issue tracking
Futureware Online Converter	www2.futureware.at/KiCad/	Web-based conversion service
NextPCB Conversion Guide	nextpcb.com/blog/how-to-convert-altium-to-kicad-vice-versa	Detailed tutorials with screenshots
KiCad Download Page	kicad.org/download	Latest stable and nightly builds

The KiCad forum is particularly valuable for unusual conversion problems. Many experienced users have encountered and solved obscure issues.

Best Practices for Ongoing Altium and KiCad Workflows

If your organization uses both tools, establishing consistent practices prevents ongoing conversion headaches.

Standardize Your Layer Usage: Document which Altium mechanical layers map to which KiCad user layers. Apply this mapping consistently across all projects.

Maintain Library Discipline: Keep a single source of truth for component libraries. Either convert Altium libraries to KiCad format and maintain only the KiCad versions, or use KiCad’s direct Altium library support for truly shared libraries.

Version Your Conversions: Store both original Altium files and converted KiCad files under version control. This creates an audit trail and enables re-conversion if needed.

Document Conversion Decisions: When manual fixes are required during conversion, document what was changed and why. This helps future engineers understand design decisions that may not be obvious.

Frequently Asked Questions

Does KiCad support Altium ASCII file formats?

Yes. KiCad 9 added support for Altium ASCII schematic file format import in addition to the standard binary format. For PCB files, both binary and ASCII formats import correctly. If you’re having trouble with binary files, ask your Altium users to export in ASCII format as a troubleshooting step.

Can I import Altium CircuitMaker or CircuitStudio files into KiCad?

Yes. KiCad’s Altium importer supports files from CircuitMaker and CircuitStudio, which use file formats compatible with Altium Designer. The import process is identical—simply select the appropriate .SchDoc or .PcbDoc file.

Will my Altium design rules transfer to KiCad?

No. Design rules (trace widths, clearances, via sizes, etc.) do not import from Altium to KiCad. You must recreate these rules manually in KiCad’s Board Setup dialog. This is one of the most time-consuming aspects of conversion for complex designs with many custom rules.

How do I handle multi-sheet flat schematics from Altium?

KiCad 9.0.3 introduced support for flat schematic import through the project import feature. For earlier KiCad versions, import each schematic sheet individually using the standalone Schematic Editor, then manually organize them into a project structure.

What’s the best KiCad version for Altium imports?

Use the latest stable release—currently KiCad 9. Each major version has significantly improved Altium import capability. KiCad 9.0.3 specifically added project file import which dramatically simplifies the workflow. Check the KiCad blog for release notes on import-related bug fixes in point releases.

Final Thoughts

Converting Altium files to KiCad is no longer the painful process it once was. KiCad’s native import support has matured to the point where most designs convert with minimal manual intervention. The key steps remain consistent: use the latest KiCad version, understand which files you need, map layers carefully, and always verify the converted design thoroughly.

For engineers transitioning permanently to KiCad, the investment in learning the conversion process pays dividends. You gain access to a powerful, free PCB design tool while preserving your existing design work. For those who need occasional access to Altium designs shared by clients or vendors, KiCad’s import capability eliminates the need for expensive software licenses.

Take your time with the first few conversions, document what works, and build a library of converted components. Each subsequent import becomes faster as you develop familiarity with both the process and the quirks of your specific design patterns.