Altium Designer Documentation

Importing a Design from CADSTAR into Altium Designer

Created: February 9, 2017 | Updated: February 20, 2017
Now reading version 17.1. For the latest, read: Importing a Design from CADSTAR for version 23
Applies to Altium Designer versions: 15.1, 16.0, 16.1, 17.0 and 17.1

Supporting the potential need to work with PCB designs in the Zuken® CADSTAR™ format, Altium Designer includes a CADSTAR Importer for translating CADSTAR Schematic, PCB and Library files to equivalent Altium Designer design files.

The importer is included in Altium Designer as a platform extension, and the function is presented as import file type option in the design file Import Wizard.

Version support

The Altium Designer 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

Enabling the Importer

If the Importer was not already added during Altium Designer’s initial installation, it can be enabled in the Configure Platform page in Altium Designer’s Extension & Updates view. Select DXP » Extensions and Updates, the Configure link under the view’s Installed tab and then check the Cadstar option in the Importers\Exporters section.

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 Designer output.


Export to CADSTAR Archive

Altium Designer Output

PCB design (*.pcb)

Use the CADSTAR File » File Export option to convert the binary pcb design (*.pcb) to a CADSTAR PCB archive (*.cpa)

Altium Design PCB document (*.pcbdoc)

Schematic design (*.scm)

Use the CADSTAR File » File Export option to convert the binary schematic design (*.scm) to a CADSTAR schematic archive (*.csa)

Altium Design schematic document (*.schdoc)

PCB Library (*.lib)

Use the CADSTAR Library Manager (Library – PCB Components) to convert the binary pcb library (*.lib) to a CADSTAR PCB archive (*.cpa)

Altium Designer PCB library (*.pcblib)

Parts Library (*.lib) and Schematic Symbol Library (*.lib)

The Parts library (*.lib) file should already be in an ASCII file format and does not need conversion. As with the PCB Library, use the CADSTAR Library Manager (Library – Schematic Symbols) to convert the binary symbol library (*.lib) to a CADSTAR schematic archive (*.csa)

The importer uses both the Parts library and the symbol schematic archive to output an Altium Designer schematic library (*.schlib)

PCB Design

The CADSTAR PCB layout file is equivalent to an Altium Designer PCB document.  Given a CADSTAR pcb layout file (*.cpa), Altium Designer'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 *.cps file format using CADSTAR File Export function. 

Schematic Designs

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

Schematic Library

The importer needs to at least two CADSTAR source files to create an Altium Designer 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 Designer 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 Designer parts.schlib. If the parts.lib file references multiple 'symbol.csa' files, these can be added during the import/conversion process.

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

PCB Library

A CADSTAR PCB component is equivalent to an Altium Designer 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 Designer PCB library (*.PcbLib) using the CADSTAR Importer.

A CADSTAR Parts library file is not strictly required when importing a CADSTAR pcb library, however if its pcb components are linked to schematic symbols via part definitions, it is good practice to supply the Parts library file during the import process. Doing so will allow Altium Designer's CADSTAR importer to correctly map the pin names from schematic component to pcb footprint by using the pin names in the part definition.

Using the CADSTAR Importer

The CADSTAR design file importer is available through Altium Designer's Import Wizard  (File » Import Wizard), where the option is selected in 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 Designer PCB layer mapping options.

Note that the Import Wizard offers a default Layer Mapping setup, which can be modified and saved as a *.ini file. The mapping is used by the Import Wizard to build the layer mapping for each PCB in the imported design, so during the import of several PCB files, a saved mapping configuration file can be loaded and applied to individual (or all) PCB files.

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 Designer's Import Wizard. In this way the wizard can generate a complete Altium Designer 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.

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
You are reporting an issue with the following selected text
and/or image within the active document: