OrCAD からのインポート

Translation is available for Altium Designer 18.0: Go to the page

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 17.2). 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.

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.

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.

Enable the OrCAD option under Importers\Exporters.

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

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.

The OrCAD importer can import PCB files created in OrCAD Layout. If the PCB was created in the product called OrCAD PCB Editor (OrCAD PCB Designer Professional), use the Allegro importer to import the PCB and PCB library files into Altium Designer.

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.
  • OrCAD PCB Editor (*.BRD & *.ALG) files can be imported into Altium Designer using the Allegro importer.
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.

Importing Orcad and PADS Designs and Libraries Files

Many PADS users use a combination of PADS Layout for their PCB layout and OrCAD Capture for their schematic capture. This section assumes this combination.

All used PADS PCB layers must be mapped to an Altium Designer layer prior to import. There are additional options through the pages of the Wizard to control the automatic creation of design rules, missing vias, and keep-out conversions.

It should be noted about how the layers are mapped on import for PCB designs. Layer Mapping is simply a mapping between the names of the PADS PCB layers and Altium Designer PCB layers. Of course, you can change as many mappings as you want as only suggested default mappings are given. This mapping is used by the Import Wizard to build the layer mapping for each PCB that can then be individually customized. The rationale here is that should you wish to import ten PCB designs and you want to map the layer Assembly 1 to Mechanical Layer 1, you would not have to customize each of the ten PCB designs in order to get the right layer mapping.

The advantage to importing in this manner is that batch management of layer mapping can save a lot of time when importing multiple designs. In this instance, the default layer mapping will be saved to your Preferences. The disadvantage to using this is that Default Layer Mapping is not always intelligent with differing structures in designs, and so some manual changes may be needed afterward.

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.).

See the Altium Designer Documentation sections to learn more about Altium Designer's functionality.

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 hierarchy 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 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.
  • Parameters defined in the title block of an OrCAD schematic are treated/behave as schematic document parameters.
The Convert Orcad Off-Page connectors as Altium Ports (instead of defaults Off-sheet connectors) option on the Schematics General Options page option can be used when converting a flat design to a hierarchical design when ports are required. See image in the Net Connectivity section below

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.

The generated schematic document supports customized port connectors and bi-directional off-sheet connectors.

If desired, you can enable the Convert Orcad Off-Page connectors as Altium Ports (instead of defaults Off-sheet connectors) option on the Schematics General Options page to eliminate the manual process needed to convert off-page connectors to ports.


利用できる機能は、Altium Designer ソフトウェア サブスクリプション のレベルによって異なります。