Gerber format

The Gerber file format is used by printed circuit board (PCB) industry software to describe the printed circuit board images copper layers, solder mask, legend, drill holes, etc.). The Gerber file format is the de facto industry standard for printed circuit board image transfer.

The Gerber file format was developed by Gerber Systems Corp. founded by Joseph Gerber. The Gerber file format is now owned by Ucamco through its acquisition of Barco ETS, a company that previously acquired Gerber Systems Corp. Ucamco brings out revisions of the specification from time to time.

The current Gerber file format specification is revision I1 from December 2012. It can be freely downloaded from the Ucamco download page.

There are two versions:

• Extended Gerber, or RS-274X, is commonly used today.
• Standard Gerber, the previous version, was a subset of the EIA RS-274-D NC standard; it is deprecated and is superseded by RS-274X.

Introduction

Inside many electronic devices is a PCB onto which components are connected. These PCBs may be designed using a computer-aided design (CAD) system. One way to physically realize a design is to transfer the computerized design information to a photolithographic computer-aided manufacturing (CAM) system. Gerber is a widely used file format for performing this transfer. Once the bare board is fabricated the Gerber file plays no role in the final assembly of components onto the board.

RS-274X extended Gerber

The RS-274X Gerber format, also known as extended Gerber or X-Gerber, is a 2D bi-level vector image description format. It is a superset of RS-274-D standard Gerber, which is itself a subset of the EIA RS-274-D format for numerically controlled machines.

It is a human readable ASCII format. It consists of a sequence of commands and coordinates. Its imaging primitives are line draw, flash (display) predefined shapes at a given location and outline fill. Positive and negative graphics objects can be combined.

An example of a RS-274X file:

G04 Film Name:    paste_top*
G04 Origin Date:  Thu Sep 20 15:54:22 2007*
G04 Layer:  PIN/PASTEMASK_TOP*
%FSLAX26Y26*MOIN*%
%IPPOS*%
%ADD28R,.11X.043*%
%ADD39O,.07X.022*%
...
%AMMACRO19*
21,1,.0512,.0512,0.0,0.0,45.*%
%ADD19MACRO19*%
%LPD*%
G75*
D10*
X1762513Y1175000D03*
Y1374634D03*
Y1637506D03*
...
D39*
X4962513Y1425000D02*
Y1375000D01*
Y1325000D01*
Y1275000D01*
M02*

An RS-274X file contains the complete description of a PCB layer image without requiring any external files. It has all the imaging operators needed for a PCB image. Any aperture shape can be defined. Positive and negative objects can be combined. Planes can be specified without the need to "paint" or "vector-fill" as in RS-274-D.

RS-274X is a complete, powerful and unambiguous standard to describe a PCB layer. It can be input and processed fully automatically. This makes it well suited for fast and secure data transfer and for reliable and automated workflows.

The format specification is published.

Usage

Gerber files are typically produced by PCB designers using specialized Electronic Design Automation (EDA) or PCB CAD software. These files are sent to PCB fabricators where they are loaded into a CAM system to prepare data for each step of the PCB production process. In this workflow they transfer the layer information from CAD to CAM. They are also used to specify drilled hole information, which can be viewed as image layers; however, the Excellon Format is used more often to transfer drilling information. Gerber files are also used to drive quality control machines, such as automated optical inspection.

The RS-274X format does not specify which PCB layer the file represents. Extensions have been proposed to specify this. In any case, it is sufficient to specify the function in the file name and to specify the format in the extension - e.g. ".GER" for Gerber. Some designers, however, use cryptic file names and document them in a free-format text file. This means that the manufacturer has to browse all the files in the dataset to find the necessary production information. In other cases the function is indicated by misusing the file extension - e.g. .BOT for Bottom Layer. In this case the manufacturer has to open the file to find out the format.

Supplementary data

An RS-274X file specifies a single conductor or mask layer image. PCB fabrication and testing requires additional information. RS-274X can specify the drill data; however, drill data is often specified in IPC-NC-349 or Excellon format. RS-274X cannot represent the netlist; if needed, the netlist is usually specified using IPC-D-356. Layer names and material stack up are typically provided in informal text files or drawings. However, Ucamco recommends using a subset of IPC-2581 for these. Typically, all these files are "zipped" into a single archive that is sent to the PCB fabrication shop.

RS-274-D standard Gerber

Standard Gerber, is largely superseded by extended Gerber. It was created from a subset of the Electronic Industries Association RS-274-D specification, a format to drive mechanical NC machines in a wide range of industries. Be aware that the term RS-274-D is often used incorrectly (with the qualifying "Gerber" postfix omitted) to refer to the standard Gerber subset, rather than the original RS-274-D superset itself. Standard Gerber is used to drive vector photoplotters, which indeed were 2D NC machines. It is a simple ASCII format consisting of commands and X, Y coordinates. An example of a Gerber RS-274-D file:

D11*
X1785250Y2173980D02*
X1796650Y2177730D01*
X1785250Y2181480D01*
X1796650Y2184580D01*
D12*
X3421095Y1407208D03*
X1785250Y2173980D03*
M02*

RS-274-D was designed in the 1960s and 1970s to drive numerical controlled machines such as vector photoplotters, machines now all replaced by raster-photoplotters. An RS-274-D file on its own is not an image description because it does not contain all information: the coordinate unit and the definitions of the apertures are not defined in the RS-274-D file. (Apertures are the basic shapes, similar to fonts in a PDF file.) The coordinate units and apertures were supposed to be set manually by the plotter operator. They were typically described in a free-format text file, called an aperture file or a wheel file (because the apertures were mounted on a wheel and rotated into the light beam), intended for human reading. There are no standards for wheel files in RS-274-D, so the designer and the plotter operator had to agree on these on a case-by-case basis.

It only supports a few simple imaging operators. To work around this limitation constructions such as "stroking," also known as "painting" or "vector-fill" are needed. Standard Gerber was well-suited to drive vector plotters and was constrained by the technology then available. It was designed for a manual workflow. It is not suitable for fully automated data transfer between PCB designers and manufacturers. PCB manufacturers have to enter coordinate units and aperture definitions manually.

RS-274-D has been deprecated by Ucamco.

History

• On 27-Aug-1980 the first edition of the Gerber Format: a subset of EIA RS-274-D; plot data format reference book was published by Gerber Systems Corporation as a specification to drive their range of photoplotters.
• In 1986 the Gerber format was extended to support apertures with variable sizes to produce rectangles of arbitrary sizes within a given range and tapered lines. This functionality is not in practical use any more.
• In the 1980s the Gerber format was adopted by several other photoplotter vendors and also CAM systems for PCB manufacturing. It had by now become the de facto standard.
• On 26-Apr-1991 with the availability of raster scan capability the Gerber format was extended for polygon areas and Extended Mass Parameters. These allow the user to dynamically define apertures of different shapes and sizes as well as defining polygon area fills without the need for "painting". The impetus to develop the Extended Mass Parameters was provided by AT&T.
• On 16-Aug-1994 the last edition of the Gerber Format Guide was published by Gerber Systems Corporation.
• In April 1998 Gerber Systems Corporation was taken over by and integrated in Barco, Belgium. Barco's PCB division is now called Ucamco (former Barco ETS).
• On 21-Sep-1998 the RS-274X Format User's Guide was published by Barco - Gerber Systems Corporation.
• In February 2010 the Gerber Format Specification was updated to revision F.
• In December 2010 the Gerber Format Specification was updated to revision G.
• In January 2012 the Gerber Format Specification was updated to revision H.
• In February 2013 the Gerber Format Specification was updated to revision I1.
• In April 2013 the Gerber Format Specification was updated to revision I2.

Related formats

Over the years there have been several attempts to replace Gerber by formats containing more information than just the layer image, e.g. netlist or component information. None of these attempts have been widely accepted within the electronics manufacturing industry, probably because the formats are complex. Gerber remains the most widely used data transfer format.

• IPC-D-350 C Printed Board Description in Digital Format, 1989. This specification was standardized as IEC 61182-1 in 1992 and withdrawn in 2001. Rarely, if ever, used.
• DXF Sometimes used. These are typically constructed as drawings, PCB objects (tracks and pads) are lost, which makes them very difficult to use in CAM.
• PDF Rarely used. Very impractical to work with because PCB objects (tracks and pads) are lost.
• DPF Format, now at v7, a CAM format from Ucamco. Sometimes used.
• The Electronic Design Interchange Format, EDIF. Rarely, if ever, used.
• ODB++, a CAM format from Mentor Graphics. Sometimes used, the prevalent non-Gerber format.
• GenCAM: IPC-2511A Generic Requirements for Implementation of Product Manufacturing Description Data and Transfer Methodology, 2000. Rarely, if ever, used.
• GenCAM: IPC-2511B Generic Requirements for Implementation of Product Manufacturing Description Data and Transfer XML Schema Methodology, 2002. Rarely, if ever, used.
• Offspring: IPC-2581 Generic Requirements for Printed Board Assembly Products Manufacturing Description Data and Transfer Methodology, 2004. Rarely, if ever, used, but receiving more attention recently.
• STEP AP210: ISO 10303-210, Electronic assembly interconnect and packaging design, first edition 2001, second edition 2008 (to be published)
• Fujiko: JPCA-EB02, based on work by Prof. Tomokage of Fukuoka University. A new standard in Japan. Rarely, if ever used.^{[citation needed]}

External links

• The Gerber File Format Specification, and diverse articles about the format