Importing a Design from CADSTAR

Supporting the potential need to work with PCB designs in the Zuken^® CADSTAR™ format, Altium NEXUS includes a CADSTAR Importer for translating CADSTAR Schematic, PCB and Library files to equivalent Altium NEXUS design files. The importer is included in Altium NEXUS as a platform extension, and the function is presented as an import file type option in the design file Import Wizard.

Version Support

The Altium NEXUS CADSTAR importer nominally supports CADSTAR versions 9 to 17 when the design files are converted into the ASCII-based CADSTAR archive format – binary CADSTAR file are not supported.

CADSTAR archive files have the extension .cpa or .csa for PCB and Schematic -based files, respectively. In practice, the importer supports the following CADSTAR file types:

• PCB designs
• Schematic designs
• Part libraries and schematic symbol libraries.
• PCB component libraries

Installing the Importer

The CADSTAR Importer can be installed alongside all other importers and exporters as part of initial installation of Altium NEXUS. Ensure that the Cadstar option - part of the Importers\Exporters functionality set - is enabled on the Select Design Functionality page of the Altium NEXUS Installer.

The CADSTAR Importer is selected for installation as part of the Importers\Exporters area of functionality.

If support has not already been added during initial installation of the software, it can be added from the Configure Platform page, when managing the extensions and updates for your installation through the Extensions & Updates view (click on the  control at the top-right of the workspace and choose Extensions and Updates from the menu):

1. From the Installed page of the view, click the Configure button at the top-right to access the Configure Platform page.

First access the Configure Platform page of the Extensions & Updates view.

2. Scroll down the page and enable the entry for Cadstar in the Importers\Exporters region of the page.

Then enable the Cadstar option under Importers\Exporters.

3. Click the Apply button at the top-right of the page. Altium NEXUS must be restarted for the changes to take effect; click Yes at the dialog prompt.

Preparing Files for Import

The following table describes the types of CADSTAR file the importer supports with a summary of how to convert the CADSTAR binary file format to an archive file format (where required) and the equivalent Altium NEXUS output.

PCB Design

The CADSTAR PCB layout file is equivalent to an Altium NEXUS PCB document. Given a CADSTAR pcb layout file (*.cpa), Altium NEXUS's CADSTAR importer will translate this to a native PCB document (*.PcbDoc). If the CADSTAR pcb layout is in binary file format, archive it to a *.cpa file format using CADSTAR File Export function. 

Schematic Designs

To import CADSTAR schematic binary files (*.scm) into Altium NEXUS, they must first be exported in the archive (*.csa) format using the File Export command in CADSTAR.

Schematic Library

The importer needs at least two CADSTAR source files to create an Altium NEXUS schematic library. The first is the CADSTAR Parts library, a plain text parts listing. Its name and location can be found through the CADSTAR Parts Library Manager (select Parts under the Libraries tab).

Part items in the Parts library are referenced by symbol definitions in a separate Symbol library file, which is the second file required by the importer when creating an Altium NEXUS schematic library.

The symbol library file must be in the CADSTAR Schematic archive (*.csa) file format, and can be converted in CADSTAR's Library Manager. Select Schematic Symbols under the Libraries tab to open the Library Manager, and use the Archive button to execute the conversion.

For example, where a Parts library file called 'parts.lib' uses the symbol definitions in a Symbol library file called 'symbol.lib', the latter is first converted to an ASCII 'symbol.csa' file using the CADSTAR's archive utility. The importer will then translate the parts.lib and symbol.csa files to an Altium NEXUS parts.schlib. If the parts.lib file references multiple 'symbol.csa' files. These can be added during the import/conversion process.

In Altium NEXUS terms, a part item definition in the parts.lib file and the symbol definition in the symbol.csa file are equivalent to an Altium NEXUS schematic library component definition.

PCB Library

A CADSTAR PCB component is equivalent to an Altium NEXUS PCB footprint. The CADSTAR PCB Library (*.lib) must first be converted to its archive (ASCII) format (*.cpa) via CADSTAR's Library Manager, and can then be translated to an Altium NEXUS PCB library (*.PcbLib) using the CADSTAR Importer.

Using the CADSTAR Importer

The CADSTAR design file importer is available through Altium NEXUS's Import Wizard  (File » Import Wizard) by selecting CADSTAR Designs and Libraries on the Wizard's Select Type of Files to Import page. The Wizard provides page options for nominating both design files (schematic and PCB) and library files (parts, symbol and footprint), and also CADSTAR to Altium NEXUS PCB layer mapping options.

Where the complete set of CADSTAR files are available (schematic design, PCB design, parts library, and schematic/pcb libraries), it is highly recommended that they are all imported during a single session of Altium NEXUS's Import Wizard. In this way, the Wizard can generate a complete Altium NEXUS project and its libraries where the component definitions in the resulting schematic library (*.SchLib) will correctly include both the related symbol and a link to the matching footprint (in the generated *.PcbLib file).

– See the CADSTAR Design and Libraries entry in the Import Wizard page for more information on the wizard's import steps.