Altium Designer Documentation

Generating IPC-2581 Fabrication Data from a PCB in Altium Designer

Created: December 19, 2018 | Updated: August 13, 2019
All Contents

Parent page: More about Outputs

As part of Altium Designer’s ability to export a wide range of PCB design fabrication and assembly file formats, the IPC-2581 Standard format is available for both individual and output job file generation.

The IPC-2581-compliant export generator is available as an Altium Designer software extension – see Extension Access for more detail.

Related to the existing ODB++ format, IPC-2581 is an open-source standard developed by the Institute for Printed Circuits IPC-2581 Consortium some years ago (2004), but since refined to the most recent Revision A and B releases (IPC-2581A/B).

The standard has progressively gained wider acceptance as an alternative to the traditional fabrication output data composed of, typically, a collection of Gerber, Drill, BOM, and text files, etc. The previous need for a complex mix of fabrication files is due to the inherent limitations of the traditional RS-274x Gerber format, which lacks definitions for the layer stack, drill information, netlist data (electrical connectivity), and BOM information.

The IPC-2581 standard is officially titled ‘Generic Requirements for Printed Board Assembly Products Manufacturing Description Data and Transfer Methodology’ and offers an XML-based single file format that incorporates a rich range of board fabrication data - from layer stackup details though to full pad/routing/component information, and the Bill Of Materials (BOM).

A single IPC-2581 XML file can include:

  • Copper image information for etching PCB layers.
  • Board layer stack information (including rigid and flexible sections).
  • Netlist for bare board and in-circuit testing.
  • Components Bill-of-Materials for purchasing and assembly (pick-and-place).
  • Fabrication and Assembly notes and parameters.

The potential advantage of adopting the IPC-2581 format for transferring board design data to fabrication and assembly houses is centered on the highly-defined, detailed single file format that is fully understood at both ends of the chain. With a working system of CAD-CAM data exchange established, the risks associated with data misinterpretation, file errors, and variable Gerber interpretation, are largely eliminated. In short, both the IPC-2581 and Gerber X2 formats represent a new generation of board design to manufacture data transfer.

Useful links:

Functionality is provided courtesy of the IPC2581 extension (a Software Extension).

The IPC2581 extensionThe IPC2581 extension

The IPC-2581 functionality can only be accessed provided the IPC2581 extension is installed as part of your Altium Designer installation. This extension is installed by default when installing the software, but in case of inadvertent uninstall can be found on the Purchased tab of the Extensions & Updates page (click on the  control at the top-right of the workspace then choose Extensions and Updates from the menu). If reinstalling, remember to restart Altium Designer once the extension has been successfully downloaded and installed.

IPC-2581 Direct Output

With a project PCB file loaded as the active document, an IPC-2581 file can be generated by selecting File » Fabrication Outputs » IPC-2581 from the main menu. This opens an initial IPC-2581 Configuration dialog in which you can specify the revision of the IPC-2581 standard to be used (A or B), as well as the measurement units and floating point number precision applied during the export process.

Define export settings in the IPC-2581 Configuration dialog.
Define export settings in the IPC-2581 Configuration dialog.

The precision setting determines the positional and sizing accuracy of the data within the generated IPC-2581 compliant file as illustrated in the image below.

The same section of an IPC-2581 file with the precision set to 2 (left) and 6 (right).The same section of an IPC-2581 file with the precision set to 2 (left) and 6 (right).

The XML-based IPC-2581 file will be exported to the location defined in the Output Path field on the Options tab of the Project Options dialog. It will be named using the format <PCBDocumentName>.cvg.

The generated file will be added to the project and appear in the Projects panel under the Generated\Text Documents folder.

IPC-2581 Output Through an Output Job File

Related page: Preparing Multiple Outputs in an OutputJob

To include IPC-2581 file output in a project's Output Job Configuration file, click on [Add New Fabrication Output] under the Fabrication Outputs section then select IPC-2581 from the menu, and the desired data source from the associated sub-menu.

Configure an IPC-2581 output as part of an Output Job file's Fabrication Outputs.Configure an IPC-2581 output as part of an Output Job file's Fabrication Outputs.

As with other Fabrication outputs, when the OutJob is run - either manually or part of the project release system - the IPC-2581 file will be generated in accordance with settings defined for the applicable Output Container.

Prepping an IPC-2581 output as part of a configured OutJobPrepping an IPC-2581 output as part of a configured OutJob

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: