KB: Importing Zuken CR-8000 Schematic and Layout

Altium Designer does not officially support direct import of Zuken CR-8000 design files. However, users may need to migrate schematics and PCB layouts from CR-8000 into Altium for continued development or archival purposes.

Import Options

If you're working with CR-8000 data:

• You might consider exporting to intermediate formats (e.g., EDIF) and then importing those into Altium through CR-5000 Import Wizard.
• Alternatively, use Zuken’s own migration tools to convert CR-8000 data to CR-5000 format, then import into Altium.

Step-by-Step Instructions for Using Intermediate Formats

Step 1: Convert Schematics to EDIF Format

Use Zuken’s EDIF Writer to export schematic files:

\DesignGateway\zdg\bin\Win64\edifWriter.exe 

This generates .eds files compatible with Altium’s importer.

Step 2: Convert PCB Layout to ASCII Format

Use Zuken’s DFpcout tool to export the layout:

\Zuken\CR-8000\Design Force\bin\DFpcout.exe -r inputfile.dsgn -o outputfile.dsgf

Then rename the output file:

outputfile.dsgf → outputfile.pcf

Step 3: Import into Altium Designer

Use the CR-5000 Import Wizard in Altium Designer.

1. Ensure the CR-5000 Import Wizard is available

• If the CR-5000 Import Wizard is not listed in the Import Wizard options, install the Zuken CR5000 Importer extension via the Extensions and Updates page in Altium Designer.
• For guidance, refer to Extending Your Installation.

2. Launch the Import Wizard

• Go to File » Import Wizard and click Next.

3. Select the Import Type

• Choose Zuken CR-5000 Design Files and click Next.

4. Add Design Files

• For schematics, add the .eds file.
• For PCB layout, add the .pcf file to the Zuken CR-5000 Board Design File section.

5. Complete the Import

• Click Finish to start the import process.

⚠️ Note: This method does not include library data.

References

• CR-5000 Import Documentation