How to Import Altium Files into EasyEDA: Complete Guide for PCB Engineers

Moving designs between EDA platforms is a reality most PCB engineers face at some point. Whether you’re collaborating with a team using different tools, working with reference designs from semiconductor vendors, or transitioning to a more cost-effective solution, knowing how to import Altium files into EasyEDA can save hours of manual recreation work.

Altium Designer is widely regarded as an industry-standard PCB design tool, and many engineers have years of designs locked in its proprietary format. EasyEDA offers a path to work with these designs in a free, browser-based environment with direct manufacturing integration. The catch? The import process requires specific file preparation that trips up many first-time users.

This guide covers everything you need to successfully import Altium Designer schematics, PCB layouts, and component libraries into EasyEDA, including the ASCII format requirement that causes most import failures.

Why Engineers Import Altium Designs into EasyEDA

Before diving into the technical process, understanding common migration scenarios helps frame the workflow decisions you’ll make.

Cost reduction motivates many transitions. Altium Designer subscriptions represent a significant investment, especially for freelancers, startups, or hobbyists. EasyEDA provides professional-grade features at no cost, making it attractive for those who can’t justify enterprise-level licensing.

Manufacturing integration appeals to production-focused engineers. EasyEDA connects directly to JLCPCB and LCSC, enabling one-click PCB ordering with pre-verified design rules. The integrated parts library shows real-time stock and pricing, streamlining the path from design to production.

Reference design utilization creates frequent import needs. Many semiconductor manufacturers publish reference designs in Altium format. Engineers using other tools need conversion paths to leverage this verified design data rather than recreating boards from scratch.

Team collaboration sometimes requires format flexibility. When project partners use different tools, the ability to exchange design files becomes critical. EasyEDA’s import capabilities enable engineers to receive Altium designs and continue development without purchasing additional licenses.

Understanding Altium File Types for EasyEDA Import

Altium Designer uses several file formats, and EasyEDA handles each differently. Understanding these distinctions prevents confusion during the import process.

Altium File Type	Extension	Description	EasyEDA Import Support
Schematic Document	.SchDoc	Circuit schematic	Supported (ASCII format only)
PCB Document	.PcbDoc	Board layout with routing	Supported (ASCII format only)
Schematic Library	.SchLib	Symbol definitions	Not directly supported*
PCB Library	.PcbLib	Footprint definitions	Not directly supported*
Integrated Library	.IntLib	Combined symbol/footprint	Not directly supported*
Project File	.PrjPcb	Project configuration	Not imported
Design Workspace	.DsnWrk	Multi-project container	Not imported

*Library files cannot be imported directly. You must place library components onto a schematic or PCB, save in ASCII format, then extract libraries during import.

Critical requirement: EasyEDA only imports Altium files saved in ASCII format. The standard binary format that Altium uses by default will not import. This is the single most common cause of import failures.

Preparing Altium Files for Import into EasyEDA

Proper preparation is essential for successful imports. Most problems stem from skipping these steps or not understanding the ASCII format requirement.

Converting Altium Files to ASCII Format

Altium Designer stores files in binary format by default. EasyEDA cannot read this format directly, so you must convert to ASCII before import.

For Schematic Files (.SchDoc):

1. Open the schematic in Altium Designer
2. Go to File → Save Copy As
3. In the “Save as type” dropdown, select Advanced Schematic ASCII (*.SchDoc)
4. Choose a destination and click Save

For PCB Files (.PcbDoc):

1. Open the PCB layout in Altium Designer
2. Go to File → Save Copy As
3. In the “Save as type” dropdown, select PCB ASCII File (*.PcbDoc)
4. Choose a destination and click Save

Important note: The ASCII conversion must happen within Altium Designer. There’s no reliable third-party tool to convert binary Altium files to ASCII. If you don’t have access to Altium, you’ll need someone with a license to perform this conversion.

Handling Library Files

EasyEDA doesn’t support direct import of Altium library files (.SchLib, .PcbLib, .IntLib). To get your libraries into EasyEDA, use this workaround:

1. Create a new schematic in Altium Designer
2. Place all the library components you need onto the schematic
3. Save the schematic in ASCII format
4. During import in EasyEDA, select “Extract library files”
5. The extracted symbols and footprints will be added to your EasyEDA library

For footprint libraries, the same process applies but using a PCB document instead of a schematic.

Pre-Import Checklist

Run through these items before attempting any import:

• Files saved in ASCII format (not binary)
• All required library components placed on schematics/PCBs if library extraction is needed
• File size under 100MB (larger files may fail or take very long)
• Units set to imperial mils in Altium (reduces grid alignment issues)
• Grid settings at 100mil for standard designs
• No non-ASCII characters in component names or net labels (can cause garbled text)
• Chinese or special characters removed or converted to standard ASCII

Reducing File Size for Large Designs

Files exceeding 100MB often fail to import or cause timeout errors. To reduce file size:

1. Open the PCB in Altium Designer
2. Select all polygon pours
3. Change copper fill type to “No Fill” temporarily
4. Save as ASCII
5. After import to EasyEDA, rebuild the copper pours

This technique removes the computed fill data, which is regenerated after import anyway.

Step-by-Step Process to Import Altium Files into EasyEDA

EasyEDA offers two editions: Standard and Professional. Both support Altium imports, but the process and capabilities differ slightly.

Importing Altium Files in EasyEDA Standard Edition

Method 1: Direct Import

1. Open EasyEDA Standard at easyeda.com
2. Navigate to File → Open → Altium
3. Select your ASCII-format .SchDoc or .PcbDoc file
4. Choose your import option:
   1. Import File: Imports the design only
   1. Import File and Extract Libs: Imports design plus extracts component libraries
5. Wait for processing to complete
6. Review the imported design

Method 2: Import Menu

1. Go to File → Import → Altium Designer
2. Browse to your ASCII file
3. Select import options
4. Click Import and wait for completion

Import Order Recommendation: When importing both schematic and PCB from the same project:

1. First, import the PCB and extract footprints
2. Then import the schematic
3. The schematic will automatically link to previously extracted footprints

This sequence ensures proper symbol-footprint associations.

Importing Altium Files in EasyEDA Pro Edition

EasyEDA Pro offers enhanced import capabilities and better handling of complex designs.

1. Open EasyEDA Pro at pro.easyeda.com
2. From the Start Page, click Import Altium
3. Select your ASCII files (you can import multiple files as a ZIP archive)
4. Configure import options:
   1. Via Solder Mask: Choose “All covered” or “Follow original setting”
   1. Board Outline Source: Select Keepout layer or Mechanical Layer 1
5. Click OK to begin import
6. Monitor progress and review results

ZIP Archive Import: For complex projects with multiple files, compress the ASCII schematic and PCB files together into a ZIP archive before import. This keeps related files linked during the import process.

Using the EasyEDA Pro Format Converter

For batch conversions or when direct import fails, the Format Converter tool provides an alternative path:

1. Download the Format Converter from the EasyEDA Pro documentation
2. Install and launch the converter
3. Select Altium Designer as the source format
4. Point to your source file directory
5. Specify the output directory
6. For binary files, provide the path to your Altium Designer executable
7. Select projects to convert and click Next
8. Import the converted files into EasyEDA Pro

The Format Converter handles both ASCII and binary formats when the original Altium software is available on the same machine.

Understanding EasyEDA Import Options

Several configuration options affect how your Altium design imports into EasyEDA.

Via Solder Mask Settings

Option	Description	When to Use
All covered with oil	Forces all vias to be tented (solder mask extension -1000)	When you want all vias covered regardless of original design
Follow original setting	Preserves the solder mask parameters from Altium	When original via settings are important to maintain

Board Outline Source

Option	Description	Result
From Keepout layer	Uses Keepout layer shapes as board outline	Closed shapes become board outline; keepout remains keepout
From Mechanical Layer 1	Uses Mechanical Layer 1 as board outline	Keepout layer converts to forbidden area

Most Altium designers use the Keepout layer for board outlines, so this is the default setting. Change it only if your design uses Mechanical Layer 1 for the board shape.

Component ID Reset

After import, schematic-to-PCB synchronization may not work correctly due to component ID mismatches. To fix this:

1. Open the imported schematic
2. Go to Design → Reset Component ID
3. Open the imported PCB
4. Go to Design → Reset Component ID
5. Try updating PCB from schematic again

Common Altium to EasyEDA Import Problems and Solutions

Even with proper preparation, issues arise. Here are the problems I encounter most frequently.

“File Not ASCII Format” Error

Symptom: Import fails with message indicating the file is not in ASCII format.

Cause: The file was saved in Altium’s default binary format.

Solution: Re-save the file from Altium Designer using “Save Copy As” and selecting the ASCII format option. There’s no workaround without access to Altium Designer.

Chinese Characters Appear as Garbled Text or Underscores

Symptom: Component names, net labels, or attributes show strange characters or underscores where text should be.

Cause: Character encoding mismatch. Altium versions below AD17 save ASCII files with GBK2312 encoding instead of UTF-8.

Solution:

1. Open the ASCII file in Notepad or another text editor
2. Save As with UTF-8 encoding
3. Retry the import

Alternatively, open the file in Notepad, find garbled text, and manually correct or remove problematic characters before import.

Wires and Pins Not Aligned to Grid

Symptom: After import, schematic wires don’t connect properly or pins appear offset from grid points.

Cause: The original Altium design used metric units or non-standard grid settings.

Solution:

1. Before exporting from Altium, set units to imperial mils (View → Switch Unit)
2. Set grid to 100mil
3. Select all (Ctrl+A)
4. Use Edit → Align → Snap to Grid
5. Save as ASCII and retry import

Missing Footprint Associations

Symptom: Schematic imports successfully but components show no footprint when converting to PCB.

Cause: Footprints weren’t extracted during import, or the import sequence was incorrect.

Solution:

1. Import the PCB file first, selecting “Extract library files”
2. Then import the schematic file
3. If associations are still broken, use Design → Reset Component ID on both documents

Import Timeout or Failure on Large Files

Symptom: Import hangs at progress indicator or fails with timeout error.

Cause: File size exceeds practical import limits (approximately 100MB).

Solution:

1. Open the design in Altium Designer
2. Select all polygon copper pours
3. Set fill type to “No Fill”
4. Save as ASCII (file size will be much smaller)
5. Import to EasyEDA
6. Rebuild copper pours in EasyEDA after import

Layer Mapping Issues

Symptom: PCB layers appear on wrong layers or are missing after import.

Cause: Altium and EasyEDA use different layer naming conventions and don’t have 1:1 mappings for all layers.

Altium Layer	EasyEDA Mapping	Notes
Top Layer	Top Layer	Direct mapping
Bottom Layer	Bottom Layer	Direct mapping
Mid Layer 1-30	Inner layers	Direct mapping
Top Overlay	Top Silk Screen	Direct mapping
Bottom Overlay	Bottom Silk Screen	Direct mapping
Keepout	Board Outline / Keep-out	Depends on import setting
Mechanical Layers	Document / Mechanical layers	May need manual adjustment
Multi-Layer	Multi-layer	Pad/via layers

Review all layers after import and manually reassign any that didn’t map correctly.

Verifying Your Imported Altium Design

Never assume an import succeeded without verification. Work through this checklist after every migration.

Schematic Verification

1. Component count: Compare total parts between Altium and EasyEDA
2. Net connectivity: Run ERC (Electrical Rules Check) in EasyEDA
3. Footprint assignments: Look for “NONE PACKAGE” warnings
4. Net names: Verify power, ground, and critical signal net names
5. Multi-sheet connectivity: Check that inter-sheet connections exist
6. Component values: Confirm resistor, capacitor, and other values transferred correctly

PCB Layout Verification

1. Board outline: Confirm board shape and dimensions match original
2. Layer stack: Verify all inner layers exist for multilayer boards
3. Copper pours: Rebuild all polygon pours after import
4. Via integrity: Check via sizes and net assignments
5. Track widths: Spot-check critical trace widths
6. Design rule check: Run DRC to catch violations

Synchronization Test

After importing both schematic and PCB:

1. Make a minor change to the schematic (add a component)
2. Try Update PCB from schematic
3. Verify the change propagates correctly
4. If synchronization fails, reset component IDs and retry

Tips for Successful Altium to EasyEDA Migration

Based on handling numerous migrations, these practices produce the best results.

Always work with copies: Never modify your original Altium files during the export process. Keep originals intact for reference and retry attempts.

Import in the correct sequence: PCB first (with footprint extraction), then schematic. This ensures proper library linkage.

Don’t round-trip files: Avoid exporting from EasyEDA back to Altium and re-importing. Each conversion can lose subtle details, and repeated conversions compound these losses.

Check encoding carefully: Character encoding issues cause more problems than any other single factor. When in doubt, open ASCII files in a text editor and look for garbled characters before importing.

Use EasyEDA Pro for complex designs: Pro handles edge cases better than Standard and offers the Format Converter for batch operations.

Document your layer mappings: Keep notes on which Altium layers map to which EasyEDA layers for your specific design. This speeds up troubleshooting and future imports.

Useful Resources for Altium to EasyEDA Migration

These resources provide additional help when standard import steps don’t solve your problem.

Official Documentation

• EasyEDA Standard Import Guide: https://docs.easyeda.com/en/Import/Import-Altium-Designer/
• EasyEDA Pro Import Guide: https://prodocs.easyeda.com/en/import-export/import-altium-designer/
• EasyEDA Pro Format Converter: https://prodocs.easyeda.com/en/import-export/easyeda-pro-format-converter/

Community Support

• EasyEDA Forums: https://easyeda.com/forum – Active community with searchable discussions of import problems
• OSHWLab Community: Discussion forum for open-source hardware projects using EasyEDA

Component Libraries

• LCSC Component Database: Integrated into EasyEDA with verified footprints linked to in-stock parts
• SnapEDA: https://www.snapeda.com – Download components in multiple formats including EasyEDA and Altium
• Ultra Librarian: https://www.ultralibrarian.com – Multi-format component downloads
• SamacSys: https://www.samacsys.com – Free component library tools

File Conversion Services

If you don’t have access to Altium Designer for ASCII conversion:

• Flex-ES: https://flex-es.com – Professional file conversion services for various EDA formats

FAQs About Importing Altium Files into EasyEDA

Can I import Altium binary files directly into EasyEDA without converting to ASCII?

No, EasyEDA requires Altium files in ASCII format. Binary format files will fail to import with an error message. You must use Altium Designer’s “Save Copy As” function to create ASCII versions of your schematic (.SchDoc) and PCB (.PcbDoc) files before importing. If you don’t have access to Altium Designer, you’ll need someone with a license to perform this conversion, or use a professional file conversion service.

How do I import Altium component libraries (.SchLib or .PcbLib) into EasyEDA?

EasyEDA doesn’t support direct import of Altium library files. The workaround is to place the library components onto a schematic or PCB document in Altium, save that document in ASCII format, then select “Extract library files” during the EasyEDA import process. The extracted symbols and footprints will be added to your EasyEDA personal library where you can reuse them in future projects.

What’s the maximum file size EasyEDA can import?

EasyEDA Standard supports files up to 100MB. EasyEDA Pro supports files up to 1GB, though very large files may experience long processing times or timeouts. For oversized files, reduce file size by temporarily removing copper pour fill data in Altium before saving to ASCII. The fill data regenerates when you rebuild copper pours in EasyEDA after import.

Why do special characters appear as underscores after import?

Unsupported characters, including Chinese text, non-ASCII symbols, and garbled encoding data, are automatically converted to underscores during import. This happens most often with files saved from Altium versions below AD17, which use GBK2312 encoding instead of UTF-8. To fix this, open the ASCII file in a text editor, convert encoding to UTF-8, correct any remaining garbled text manually, then retry the import.

Can I synchronize my imported schematic with the imported PCB?

Yes, but you must follow the correct import sequence and may need to reset component IDs. Import the PCB file first with footprint extraction enabled, then import the schematic. If synchronization still fails, use Design → Reset Component ID on both the schematic and PCB documents. This reassigns unique identifiers that enable EasyEDA to match schematic symbols with their PCB footprints.

Final Thoughts on Migrating from Altium to EasyEDA

Importing Altium files into EasyEDA requires more preparation than some engineers expect, primarily due to the ASCII format requirement. Once you understand this constraint and establish a reliable workflow, migrations become straightforward.

The key is treating the process as a deliberate conversion rather than a simple file open. Prepare your files properly in Altium, follow the correct import sequence, and verify results thoroughly before proceeding with design work.

For engineers without Altium Designer access, the ASCII requirement presents a real barrier. If you regularly receive Altium files from collaborators, establishing a relationship with someone who can perform the ASCII conversion—or using a conversion service—becomes necessary.

Once your designs are in EasyEDA, you gain access to a capable design environment with excellent manufacturing integration. The import effort pays off through streamlined PCB ordering and access to extensive, verified component libraries. For many engineers, this trade-off makes the migration worthwhile despite the initial learning curve.

Start with a simpler design to learn the import process before tackling your most complex projects. The experience you gain on a straightforward board will make migrating larger designs much smoother.