Importing a Design from CR-5000

Altium Designer includes the capability to import Zuken^® CR-5000^™ files through the Import Wizard. The Wizard is a quick and simple way to convert CR-5000 design files to Altium Designer files. The Wizard walks you through the import process and handles both the schematic and PCB parts of the project, as well as managing the relationship between them.

The CR-5000 importer is included in Altium Designer as a software extension, which when enabled, will add a Zuken CR-5000 Design Files import option to the Import Wizard.

Zuken CR5000 Importer Extension

To use the importer, first ensure the Zuken CR5000 Importer extension is included in the Software Extensions region on the Installed tab of the Extensions & Updates view (click the  control at the top-right of the design space then choose Extensions and Updates from the menu).

If the Zuken CR5000 Importer extension is not listed or is at anytime uninstalled, the extension will need to be installed. To do so, access the Extensions & Updates view then open the Purchased tab where the Zuken CR5000 Importer extension will be listed (the extensions are listed alphabetically). Click  to download the extension then restart Altium Designer when prompted. 

Preparing Zuken Binary Files for Import

The Zuken CR-5000 Importer requires ASCII files, so the native Zuken CR-5000 binary files will need to be converted to ASCII format before using the Import Wizard.

Use the following steps to convert the Zuken CR-5000 binary PCB database files to ASCII files:

1. Convert the binary file <basename>.ftp into an ASCII file: In the cdb directory, extract <basename>.ftf using the DOS (or command script) command: ftout.exe<basename>. For example, C:\cr5000\bin\ftout.exe basename.
2. Convert the binary file <jobname>.pcb into an ASCII file: In the pcb directory, extract <jobname>.pcf using the DOS (or command script) command: pcout.exe<jobname>. For example, C:\cr5000\bin\pcout.exe jobname. 

To convert the Zuken CR-5000 schematic binary file (*.sht) to ASCII format (*.eds), run the Zuken edifWriter.exe utility. This opens a GUI for creating the ASCII format file.

The Zuken CR-5000 Importer requires two ASCII files to import a Zuken CR-5000 PCB design, and an ASCII schematic file to import a schematic.

• An ASCII layout file which contains placement and layer symbols, layer count, units, etc. (*.pcf)
• An ASCII representation of the footprints used in the design (library) (*.ftf)
• An ASCII representation of the schematic (*.eds, *.edf)
• An ASCII representation of the symbol (*.laf)
• An ASCII representation of the symbol (*.smb)

Using the CR-5000 Importer

The Zuken CR-5000 design file importer is available through Altium Designer's Import Wizard  (File » Import Wizard) by selecting the Zuken CR-5000 Design Files option on the Wizard's Select Type of Files to Import page. The Wizard provides options for nominating design files (schematic and pcb) and library files, and also CR-5000 to Altium Designer layer mapping options for both footprints and PCB layouts.

 Zuken CR5000 files translate as follows:

• Zuken CR5000 ASCII PCB Layout (*.pcf) files translate to Altium Designer PCB files (*.PcbDoc).
• Zuken CR5000 ASCII representation of the footprints files (*.ftf, *.laf) translate into Altium Designer PCB library files (*.PcbLib).
• Zuken CR5000 ASCII representation of the schematic files (*.eds, *.edf, *.smb) translate to Altium Designer schematic files (*.SchDoc) and schematic library files (*.SchLib).