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.
The OrCAD Importer/Exporter can be installed alongside all other importers and exporters as part of 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.
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).
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.
Imported OrCAD files translate as follows:
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.
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.).
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.
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.
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.
Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.