EAGLE からのインポート

Supporting your need to work with design files in other formats and from other tools, Altium Designer provides an importer for Autodesk® EAGLE™ (Easily Applicable Graphical Layout Editor) design files and libraries (*.sch, *.brd, *.lbr).

Version Support

The EAGLE Importer is able to import XML-format EAGLE design files saved with EAGLE versions 6.4 through to 9.4. These are XML-format in nature; EAGLE binary-format design files cannot be imported directly using the EAGLE Importer. For these older, binary version design files, it is advised to save them in this later (XML) format through your EAGLE software before attempting to import into the software.

Installing the EAGLE Importer

The EAGLE Importer can be installed alongside all other importers and exporters as part of the initial installation of Altium Designer. Ensure that the EAGLE 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 the  control at the top-right of the workspace then 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.

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

Enable the EAGLE option under Importers\Exporters.

3. 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 in the dialog prompt to restart.

Accessing and Running the EAGLE Importer

Import is performed using the Import Wizard (File » Import Wizard). Select the EAGLE Projects and Designs entry to gain access to the EAGLE Import Wizard then click Next.

Access the EAGLE Import Wizard  through the Import Wizard dialog.

The EAGLE Import Wizard will guide you through the steps involved when importing these types of files including:

• Specifying which EAGLE design archives (*.BRD, *.SCH) to include in the process.
• Specifying which EAGLE library files (*.LBR) to include in the process.
• Setting options to control the reports manager.
• Setting options related to project structure.
• Specifying the location of the output directory in which to import the files

You have full control over where the generated Altium Designer project(s) and associated documents are to be located by specifying an output directory.

The proposed output structure is also displayed so you can see exactly what you will be getting with the import. If all is as required, proceed with the import by clicking Next. If you need to change anything, click the Back button. If you want to cancel out of the import, click Cancel.

Specify which EAGLE design files and/or libraries are to be imported and other options as required.
Check the output directory and proposed structure, before proceeding with the import process.

Once the import process completes, click Finish in the Import Wizard dialog to close it. The result of the import can be seen in the Projects panel and can be summarized as follows:

• An Altium Designer PCB Project (*.PrjPcb) is created per EAGLE .sch, .brd and .lbr involved in the import.
• An EAGLE schematic design archive (*.sch) is imported into an Altium Designer Schematic document (*.SchDoc).
• An EAGLE PCB design archive (*.brd) is imported into an Altium Designer PCB document (*.PcbDoc).
• An EAGLE library (*.lbr) is imported as Altium Designer Schematic Library (*.SchLib) and PCB Library (*.PcbLib) documents. In addition, an integrated Library (*.IntLib) is compiled based on these source libraries.
• A Log file (*.log) is generated for each imported file, which shows the results of analysis on the original EAGLE file, as well as any errors and warnings (if enabled for inclusion).

Resulting PCB projects, with opened schematic and PCB documents after importing EAGLE .pcb and .sch design files.

Post-Import Considerations

After importing your EAGLE design files, it is fairly common to check and possibly change a few things. The following is an example of a post-import procedure that may be undertaken. This is by no means an exhaustive, or indeed mandatory requirement, but more of a thought-provoking aid for possible items to consider post-import:

• When schematic and PCB files are present and imported into separate projects, move (or copy) the imported design files into a single Altium Designer PCB project.
• Check component links (again, when both schematic source and PCB board have been imported). From the imported PCB for the design, use the Project » Component Links command. Use the subsequent Edit Component Links dialog to match (link) schematic and PCB components.
• Check the Design Rules using the PCB Rules and Constraints Editor dialog (Design » Rules) fixing any that are not quite targeting the intended objects, and simplifying where ever possible (especially Clearance and Width rules).
• If not already present on import, make a PCB Library from the PCB design (Design » Make PCB Library), fix any parts as needed to the required standard for your company, and also add 3D models.
• Update the PCB Design from the update PCB Library (if applicable).
• Run a DRC (Tools » Design Rule Check) using the Design Rule Checker dialog and fix any errors.
• Clean up any imported polygons into larger pours with associated rules.
• Add a keepout boundary to the board.