Altium Designer Documentation

Importing a Design from OrCAD into Altium Designer

Created: March 6, 2019 | Updated: March 17, 2020
Now reading version 19.0. For the latest, read: Importing a Design from OrCAD for version 24
Applies to Altium Designer versions: 19.0 and 19.1

Translating complete OrCAD® designs, including Capture schematics, Layout PCB files, and library files can all be handled by Altium Designer's Import Wizard (to OrCAD version 16.xx). The Import Wizard removes much of the headache normally found with design translation by analyzing the imported files and offering defaults and suggested settings for the project structure, layer mapping, PCB footprint naming, and more. The flexibility provided through the Wizard steps gives you as little or as much control as you like over the file translation settings, before committing to the actual translation process.

Installing the Importer

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

The OrCAD Importer/Exporter 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.

Access the Configure Platform page of the Extensions & Updates view.

  1. Scroll down the page and enable the entry for OrCAD in the Importers\Exporters region of the page.

Enable the OrCAD option under Importers\Exporters.

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

Importing OrCAD Files

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

Directly opening an OrCAD file (*.dsn, *.max, *.olb, *.llb) in Altium Designer (File » Open) will activate the Import Wizard with that file already specified for import.
See the OrCAD Design and Libraries Files entry on the Import Wizard page for more information on the Wizard's import steps.

File Translation

Imported OrCAD files translate as follows:

  • OrCAD Layout (*.MAX) files translate to Altium Designer PCB files (*.PcbDoc).
  • OrCAD Capture (*.DSN) files translate to Altium Designer schematic files. Each page within a .DSN file will be imported as a single Altium Designer schematic file (*.SchDoc). Design caches within a .DSN file will be imported as a schematic library (*.SchLib). Design hierarchy is maintained, including complex hierarchy.
  • OrCAD .OLB (schematic library) files will be translated into Altium Designer schematic library files (*.SchLib).
  • OrCAD .LLB (PCB library) files will be translated into Altium Designer PCB library files (*.PcbLib).
  • Translated OrCAD libraries are automatically grouped into one PCB project.
Migration from one tool to another is subject to the limitations of converting objects from the first tool to the importing tool. It is sometimes not possible to translate all object types. Altium regularly improves the Import Wizard's design file converters, so if difficulty is encountered during an import, ensure that Altium Designer has been updated to the most current build. This may result in better version compatibility and more accurate imports.

PCB Layer Mapping

It is worth noting how layers are mapped between the imported PCB design and the resulting PCB layout in Altium Designer. Layer mapping is the relationship between the names of the 'foreign' PCB layers and the Altium Designer PCB layers.

To support the batch import process of multiple designs, the Import Wizard offers a default Layer Mapping setup, which can be modified and saved as a text-based *.ini file. The mapping is used by the 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.

The Wizard's default Layer Mapping setup can be modified and saved to a configuration file.
The Wizard's default Layer Mapping setup can be modified and saved to a configuration file.

A previously saved Layer Mapping configuration can be loaded and applied to any or all imported PCB files.
A previously saved Layer Mapping configuration can be loaded and applied to any or all imported PCB files.

The rationale here is that if you want to import ten PCB designs and want to map the layer Assembly 1 to Mechanical Layer 1, each of the ten imported PCB designs would not have to be customized in order to achieve the desired layer mapping.

Working with Imported Documents

In OrCAD Capture all design work begins on the page, which is the logical working area of the design, and there can be multiple schematic pages within a single OrCAD schematic design file (*.DSN file). In Altium Designer, the logical design area begins with a document, and for each document, there is a file stored on the hard drive.

This means that each Altium Designer schematic sheet (page) is represented by is schematic document file, which is a key conceptual difference to keep in mind. Note that Altium Designer can also include multiple documents of varying types (beyond just schematic and PCB design documents), depending on the nature of the design project.

Workspace Panels

Many elements of the Altium Designer environment will appear familiar to OrCAD users, such as the Projects panel which is similar to the OrCAD Project Manager. Since the Projects panel is not limited to schematic design data, it can include the PCB, all libraries, output files, as well as other project documents, such as non-native files (PDFs, text files, spreadsheets, etc.).

Project Structure

OrCAD Capture, like Altium Designer, supports flat and hierarchical designs.

Capture presents a schematic, shown as a folder icon in Capture's Project Manager, and this contains pages shown as schematic sheet icons. Each Capture schematic can be made up of one or more pages, and a typical flat Capture design is one schematic (folder), with the design being drawn on as many pages as required in that schematic.

The schematic folder at the top of a hierarchy, which directly or indirectly refers to all other modules in the design, is called the root module. In the OrCAD Project Manager, the root module has a backslash on its folder icon.

Altium Designer presents a hierarchical of related schematics, where the sheet-to-sheet structure is typically defined by Sheet Symbols. The equivalent Capture construct is a Hierarchical Block symbol, which references the lower level schematic.

See the Projects panel for information on managing project structures in Altium Designer.
Note that the OrCAD importer will convert the cached components contained in an imported *.DSN schematic file into an Altium Designer Schematic library (*.SchLib). The library's component entries will include any footprint references and parameters that are available from the source file. This function is not unlike Altium Designer's Make Schematic Library feature for native projects.

Net Connectivity

In OrCAD Capture, net connectivity is made using net aliases, off-page connectors, hierarchical blocks and ports, and globals. Nets between schematic pages within a single schematic folder are connected through the off-page connectors while the hierarchical blocks and ports connect the nets between the schematic folders. Globals are used to connect power/ground nets throughout the design.

Altium Designer uses a similar set of net identifiers to create net connectivity. Within a schematic sheet you can use Wires and Net Labels. Between schematic sheets, nets in a flat design are typically connected using Ports, but Off-Sheet Connectors are also available. Nets in a hierarchical design are connected from a Port on the lower sheet to a Sheet Entry of the same name in the sheet symbol that represents the lower sheet. Power/ground nets are connected using Power Ports.

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: