Generating Fabrication Data

This documentation page references Altium NEXUS/NEXUS Client (part of the deployed NEXUS solution), which has been discontinued. All your PCB design, data management and collaboration needs can now be delivered by Altium Designer and a connected Altium 365 Workspace. Check out the FAQs page for more information.

 

Parent page: Streamlining Generation of Manufacturing Data with Output Jobs

A wide range of PCB design fabrication file formats is available for both individual and output job file generation, including:

  • Gerber RS-274X and Gerber X2
  • ODB++
  • IPC-2581

Generating Gerber Fabrication Data

Each file of the Gerber RS274X format (also known as Extended Gerber, or GerberX) corresponds to one layer in the physical board – the component overlay, top signal layer, bottom signal layer, the solder masking layers, etc. This file format includes aperture definitions, XY coordinate locations for draw and flash commands, and other information needed for PCB fabrication.

Gerber X2 is a direct, and much advanced, evolution of the Gerber RS-274X standard and adds a large range of additional data for PCB fabrication and assembly. Compared to the RS-274X standard, the Gerber X2 format includes critical information, such as:

  • Layer stack definitions
  • Pad and via attributes
  • Impedance controlled tracks

A prime advantage of the Gerber X2 format is backward compatibility with the old Gerber RS-274X standard. Being a multi-file standard, a target fab/assembly house that has not moved to the new standard can extract the traditional Gerber file elements as needed. This may be a significant advantage for those unwilling to tackle a major shift in fabrication file formats, or for fabrication houses with inflexible equipment and software.

The overall benefit of adopting the Gerber X2 format for transferring board design data to fabrication and assembly houses is the rich set of manufacturing data included in the file set and the backward compatibility to the previous standard for a low-risk upgrade path. With a full implementation at both ends of the CAD-CAM chain, the risks associated with data misinterpretation, file errors and variable data interpretation can be largely eliminated. In short, both the Gerber X2 and IPC-2581 formats represent a new generation of board design to manufacture data transfer.

Useful links:

With a project PCB file as the active document, the Gerber file set can be generated by selecting File » Fabrication Outputs » Gerber Files or File » Fabrication Outputs » Gerber X2 Files from the main menus. This opens an appropriate Gerber Setup or Gerber X2 Setup dialog in which you can define the plot layers and general configuration applied during the export process. See the collapsible sections below for detailed information on options and controls provided by these dialogs.

This page looks at Gerber file generation using the Gerber Setup and Gerber X2 Setup dialogs available when the UI.Unification.GerberDialog option is enabled in the Advanced Settings dialog. The Advanced Settings dialog is accessed by clicking the Advanced button on the System – General page of the Preferences dialog. If any changes are made in the Advanced Settings dialog, the software must be restarted in order for the changes to take effect.

When the UI.Unification.GerberDialog option is disabled in the Advanced Settings dialog, Gerber file generation is performed using the previous iterations of the Gerber Setup and Gerber X2 Setup dialogs.

Gerber Setup and Gerber X2 Setup  dialogs
Gerber Setup and Gerber X2 Setup dialogs

Output is generated in the location defined in the Output Path field on the Options tab of the Project Options dialog. Generated file names will include the name of the PCB document.

Generated files will be added to the project and appear in the Projects panel under Generated\CAMtastic! Documents and Generated\Text Documents folders.

The generated Gerber output is also opened as a composite CAM document that can be edited and/or saved into the current project and managed via the CAMtastic panel.

To specify if the generated CAM output is automatically opened in Altium NEXUS, enable the Open outputs after compile option on the Options tab of the Project Options dialog (Project » Project Options).

Generating ODB++ Fabrication Data

ODB++ is a CAD-to-CAM data exchange format used in the design and manufacture of printed circuit boards. The format was originally developed by Valor Computerized Systems, Ltd., as an open database that could provide a more information-rich data exchange between PCB design software and Valor CAD-CAM software used by PCB fabricators.

With a project PCB file as the active document, the ODB++ file set can be generated by selecting File » Fabrication Outputs » ODB++ Files from the main menus. This opens the ODB++ Setup dialog that provides controls to completely configure ODB++ file output options.

 
 
 
 
 

Define export settings in the ODB++ Setup dialog.
Define export settings in the ODB++ Setup dialog.

Generating IPC-2581 Fabrication Data

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 NEXUS 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 design space then choose Extensions and Updates from the menu). If reinstalling, remember to restart Altium NEXUS once the extension has been successfully downloaded and installed.

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.

Fabrication File Output through an Output Job File

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


Configure fabrication outputs as part of an Output Job file's Fabrication Outputs. Shown here is an example for Gerber X2 files.

When the OutJob is run – either manually, or as part of the project release process – the fabrication outputs will be generated in accordance with settings defined for the applicable Output Container.

Prepping fabrication outputs as part of a configured OutJob.
Prepping fabrication outputs as part of a configured OutJob.

The settings defined in related dialogs when generating fabrication outputs directly from the PCB are distinct and separate from those defined for the same output type in an OutputJob Configuration file. In the case of the former, the settings are stored in the project file, whereas for the latter, they are stored in the OutputJob Configuration file.
If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.
Content