RS-274D and RS-274X are two generations of the Gerber PCB image format. They can look similar when rendered, but they are very different as manufacturing handoff files. RS-274D is the old, now-deprecated Standard Gerber format. RS-274X is Extended Gerber, the modern format that embeds the information needed to interpret the layer image.
The short version is that RS-274D files were incomplete by themselves. They contained draw and flash commands, but the aperture definitions lived in a separate external aperture list. RS-274X moved those definitions into the file with parameter commands such as %AD, %FS, and %MO. That made each Gerber layer much more portable and much less dependent on CAM operator guesswork.
If you are new to the overall file set, start with what a Gerber file is. If you already have a ZIP, inspect it in the Gerber viewer and confirm that the layers render without missing shapes.
Quick answer
RS-274D is legacy Standard Gerber and depends on a separate aperture list, so the file alone is incomplete. RS-274X is Extended Gerber and embeds apertures, units, and coordinate format inside the file. Ucamco has deprecated RS-274D, and modern PCB tools should output RS-274X or Gerber X2.
What RS-274D was
RS-274D is the older Gerber format used in early photoplotter and CAM workflows. It describes image operations such as moving, drawing, and flashing an aperture at specified coordinates. The problem is that the file refers to apertures by codes, but it does not define what those apertures are. The round, rectangular, thermal, or custom shape assigned to a code had to be supplied in a separate aperture list, aperture table, or wheel file.
That separation was workable in controlled internal workflows, but it was fragile as a data exchange format. If the aperture list was missing, outdated, renamed, or interpreted differently, the CAM system could not reproduce the layer correctly. Pads could render at the wrong size. Traces could use the wrong width. Custom apertures could disappear or become placeholders. Those errors were not minor formatting issues; they changed the board image.
Ucamco, the current owner and maintainer of the Gerber specification, has deprecated RS-274D. If a manufacturer asks for an aperture list today, that is a sign that the export flow is old or configured for Standard Gerber instead of Extended Gerber.
What RS-274X changed
RS-274X, also called Extended Gerber, made Gerber files self-contained. The file can define its own coordinate format, units, apertures, layer polarity, and image parameters. The most recognizable commands are parameter blocks wrapped in percent signs. %FS defines coordinate format. %MO defines units. %AD defines apertures. Other commands describe polarity, step-and-repeat, regions, and related image details.
With RS-274X, a top copper file can travel as a complete layer image. A CAM system does not need a separate aperture wheel to know that D10 is a 0.2 mm circular aperture or that another code is a rectangular SMD pad shape. This does not mean a single Gerber contains the whole board. It means each Gerber layer contains the image information needed to render that layer without an external aperture definition file.
RS-274D vs RS-274X reference
| Topic | RS-274D | RS-274X |
|---|---|---|
| Common name | Standard Gerber | Extended Gerber |
| Aperture definitions | External aperture list or wheel file. | Embedded in the Gerber with commands such as %AD. |
| Self-contained layer image | No, not without the matching aperture data. | Yes, for the Gerber layer image. |
| Status | Deprecated legacy format. | Current baseline for normal Gerber output. |
| When you might see it | Old archives, old CAM jobs, or misconfigured exports. | Modern EDA exports and manufacturer ZIP packages. |
| Practical risk | Missing or mismatched apertures can alter the image. | Lower handoff risk because aperture data travels inside. |
Why missing apertures mattered
In a PCB layer, apertures are not cosmetic. They define the drawing tools that create pads, tracks, and other image features. A flash places an aperture shape at a coordinate. A draw moves an aperture along a path to create a trace or line. A region fills an area. If the aperture definitions are absent or wrong, the same coordinate commands can produce a physically different board.
This is why RS-274X became the practical baseline. It reduced the number of separate files needed to interpret a layer and removed a class of avoidable CAM intake errors. Modern manufacturers may still request a readme or layer map, but they should not need a separate aperture list for a normal RS-274X export.
Where Gerber X2 fits
Gerber X2 does not replace RS-274X with an unrelated format. It extends it. The image commands remain RS-274X-compatible, and additional attributes describe what the data means. A file can say it is top copper instead of relying only on a filename such as .gtl. An aperture can be tagged as an SMD pad or via pad. Object attributes can carry net or component-related metadata when exported by the design tool.
That attribute model is covered in the Gerber X2 guide. The key point here is that RS-274X solved self-contained image transfer, while X2 adds structured meaning on top of that image.
Check old files in the viewer
If you receive old Gerbers and they do not render correctly, inspect the file headers and ask whether a separate aperture list exists. Load the complete package in the Gerber viewer first. If shapes are missing, pads look wrong, or layers fail to parse, regenerate RS-274X or X2 files from the original PCB project rather than trying to repair a partial RS-274D handoff.
FAQ
- Is RS-274D still a valid format?
- RS-274D is a legacy Gerber format, but Ucamco has deprecated it. Modern PCB workflows should export RS-274X or Gerber X2 instead.
- Why did RS-274D need an aperture list?
- RS-274D files did not embed aperture definitions. The CAM operator needed a separate aperture list or wheel file to know the shapes and sizes used by the drawing commands.
- How can I tell if a file is RS-274X?
- RS-274X files usually contain parameter blocks such as %FS, %MO, and %AD near the top of the file. Those commands define format, units, and apertures inside the Gerber itself.
- Is Gerber X2 different from RS-274X?
- Gerber X2 is an extension of RS-274X. It keeps the embedded image data and adds attributes that describe layer function, apertures, objects, nets, and components.