Generating Gerber Fabrication Data

This document is no longer available beyond version 22. Information can now be found here: Generating Gerber Fabrication Data for version 24


As part of Altium Designer’s ability to export a wide range of PCB design fabrication and assembly file formats, the Gerber RS-274X and Gerber X2 formats are available for both individual and output job file generation.

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:

Gerber Direct Output

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 Designer, enable the Open outputs after compile option on the Options tab of the Project Options dialog (Project » Project Options).

Gerber Output through an Output Job File

To include Gerber file output in a project's Output Job Configuration file, click on [Add New Fabrication Output] under the Fabrication Outputs section then select Gerber Files or Gerber X2 Files from the menu, and the desired data source from the associated sub-menu.

Configure Gerber outputs as part of an Output Job file's Fabrication Outputs. Shown here is an example for Gerber files. Hover the cursor over the image to see an example for Gerber X2 files.
Configure Gerber outputs as part of an Output Job file's Fabrication Outputs. Shown here is an example for Gerber files. Hover the cursor over the image to see an example for Gerber X2 files.

As with other Fabrication outputs, when the OutJob is run – either manually, or as part of the project release process – the Gerber file set will be generated in accordance with settings defined for the applicable Output Container.

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

The settings defined in the Gerber Setup and Gerber X2 Setup dialogs when generating output 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.

The features available depend on your Altium product access level. Compare features included in the various levels of Altium Designer Software Subscription and functionality delivered through applications provided by the Altium 365 platform.

If you don’t see a discussed feature in your software, contact Altium Sales to find out more.