The Gerber format is an open 2D bi-level vector image file format. It is the de facto standard 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 was originally developed by the Gerber Systems Corp., a division of Gerber Scientific, 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 Gerber file format specification is currently J1 from February 2014, extending the format with attributes conveying PCB meta-information such as the layer the file represents. The specification can be freely downloaded from the Ucamco download page.
There are two versions:
- Extended Gerber, or RS-274X, is commonly used today.
- Standard Gerber, or RS-274-D, is deprecated; it is superseded by RS-274X.
The standard file extension is .GBR.
One usage is the transfer of PCB design data from design to manufacturing. PCBs are typically designed on a specialized Electronic Design Automation (EDA) or a computer-aided design (CAD) system. The CAD systems output Gerber files which are sent to PCB fabricators to transfer the design information. The fabricator loads them into his computer-aided manufacturing (CAM) system to prepare data for each step of the PCB production process. Gerber files are also used to transfer drilled hole information, however, for historic reasons Excellon files are used more often for this. 
Another usage is to transfer a single image. An example is where a CAM system outputs a Gerber file to drive a photo plotter. Another is the use of Gerber viewers to visualize PCB layers.
Once the bare board is fabricated the Gerber file plays no role in the final assembly of components onto the board.
Exchanging PCB design information
A PCB design is described by a number of Gerber files and files in other formats. Typically, all these files are "zipped" into a single archive that is sent to the PCB fabrication shop.
A Gerber file defines a single conductor or mask layer image. It does not specify which PCB layer the file represents. A simple method to specify the file function is to express it clearly in the file name. Sometimes, however, cryptic file names are used and then documented in a free-format text file. This means that the manufacturer has to browse all the files in the data set to find the file function. Sometimes the function is even indicated by abusing the file extension - e.g. instead of using the standard extension .GBR using .BOT to express the file is the bottom layer; the manufacturer then cannot even know which format a file is in without opening it.
Pads are sometimes represented by painting them with small strokes rather than by a single flash. This technique is known as painting or stroking. Painting produces the desired image but the location and shape of the pads is lost. The fabricator needs pad locations, e.g. to perform an electrical test. When the fabricator receives painted files he must laboriously recover the pads from the mass of painted strokes, a time-consuming and error-prone process. Use flashed pads rather than painted pads in design to fabrication data transfer. Some claim painting is somehow intrinsic to the Gerber format. This is a fallacy. Painting is simply poor implementation of the Gerber output.
Drill data can be viewed as an image. Gerber files can therefore specify the drill data. However, for historic reasons, IPC-NC-349 or Excellon format is more often used for this although the use of another format often leads to registration problems.
Layer functions, the material stack up, components and meta-information are typically provided in informal text files or drawings. Ucamco recommends using a subset of IPC-2581 for this non-image information.
In December 2013 Ucamco published a draft specification extending the Gerber format with attributes transferring meta-information. Ucamco requests feedback from the PCB community before committing this to the specification.
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 and pads can be specified without the need to "paint" or "vector-fill".
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.
RS-274-D standard Gerber
Standard Gerber is superseded by extended Gerber. It is a subset of the Electronic Industries Association RS-274-D specification, a format to drive mechanical NC machines in a wide range of industries. Standard Gerber was used to drive vector photoplotters, which indeed were 2D NC machines. The term RS-274-D, without the qualifying "Gerber" postfix, is sometimes used informally for the standard Gerber subset rather than full RS-274-D.
RS-274-D standard Gerber is a simple ASCII format consisting of commands and XY coordinates. An example:
D11* X1785250Y2173980D02* X1796650Y2177730D01* X1785250Y2181480D01* X1796650Y2184580D01* D12* X3421095Y1407208D03* X1785250Y2173980D03* M02*
Standard Gerber was designed in the 1960s and 1970s to drive numerical controlled machines such as vector photoplotters, machines now all replaced by raster-photoplotters. Standard Gerber was well-suited to drive vector plotters but 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.
An Standard Gerber 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 set manually by the operator of the plotter. They were described in a free-format text file, called an aperture file or a wheel file, intended for human reading. It was called a wheel file because the apertures were mounted on a rotating wheel and the operator defined the apertures by selecting a wheel and mounting it on the plotter. There are no standards for wheel files. The designer and the plotter operator had to agree on these a case-by-case. Therefore standard Gerber is an NC standard but not an image definition standard.
Standard Gerber supports only the few simple imaging operators supported by vector plotters. To work around this limitation all but the simplest shapes were created by stroking the shape with a large number of small vectors. This method is known as stroking, painting of vector-fill. This does create the desired image, but such file are very hard to work with in PCB CAM because the original shape is lost.
- 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.
- In June 2013 the Gerber Format Specification was updated to revision I3.
- In June 2013 a proposal to extend the Gerber format with attributes is published.
- In November 2013 the Gerber Format Specification was updated to revision I4.
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.
- "Gerber File Format Specification.pdf". Ucamco. February 2013. Retrieved 21 December 2012.
- Williams, Al (2004). Build your own printed circuit board. McGraw-Hill Professional. p. 121. ISBN 978-0-07-142783-8. Retrieved April 2, 2011.
- Schroeder, Chris (1998). Printed circuit board design using AutoCAD. Newnes. p. 283. ISBN 978-0-7506-9834-4. Retrieved April 2, 2011.
- Blackwell, Glenn R. (2000). The electronic packaging handbook. 5.18: CRC Press. ISBN 978-0-8493-8591-9. Retrieved April 2, 2011.
- "Gerber Scientific Instrument Company Records, 1911-1998".
- Tanghe, Jean-Pierre. "Barco acquires Gerber Systems Corp". Barco.com. Barco NV. Retrieved 26 November 2011.
- "A short History of Electronic Data Formats". Printed Circuits Design and Fab. 28 June 2011. Retrieved 15 October 2011.
- "Ucamco announce a revision of the industry standard RS-274X Format Specification". ucamco.com. December 9, 2010. Retrieved February 15, 2013.
- "New Gerber Format Specification free at www.ucamco.com". ucamco.com. January 27, 2012. Retrieved February 15, 2013.
- "Ucamco Offers Latest Gerber Format Specification". ucamco.com. February 19, 2013. Retrieved February 15, 2013.
- "Gerber Grows Attributes". Printed Circuit Design & Fab. August 2013. Retrieved 5 September 2012.
- Karel Tavernier (2011/2Q). "Improving CAD to CAM Data Transfer: A Practical Approach". Journal of the HKPCA (40). Retrieved 2 October 2011. "Use of RS-274-D: Do not use it."
- "EDA: Where Electronics Begins". edac.org. Electronic Design Automation Consortium. Retrieved December 18, 2011.
- "PCBexpress Printed Circuit Board Tutorial". PCBexpress.com. Retrieved December 18, 2011.
- Mike Buetow (28 June 2011). A Short History of Electronic Data Formats. Printed Circuit Design and Fab magazine. Retrieved December 18, 2011.
- "PCB Layout Data". Eurocircuits. Retrieved 26 November 2011.
- "RS-274X Painting Considered Harmful.pdf". Ucamco. June 2011. Retrieved 5 March 2012.
- Karel Tavernier (November 2013). "Painting Pads". PCB Design Magazine (November 2013). Retrieved 23 November 2013.
- "PCB Layout Data". Eurocircuits. Retrieved 26 November 2011.
- "Using IPC-D-356 for Importing Net and Node". Retrieved 16 October 2011.
- IPC-2524 PWB Fabrication Data Quality Rating System, February 1999.
- Karel Tavernier (January 2013). "IPC-2581 meets Gerber". PCB Design Magazine (January 2013). Retrieved 19 February 2013.
- Sinclair, Ian Robertson; Dunton, John (January 11, 2007). Practical electronics handbook. Elsevier. p. 543. ISBN 978-0-7506-8071-4. Retrieved April 2, 2011.
- EIA Standard RS-274-D Interchangeable Variable Block Data Format for Positioning, Contouring, and Contouring/Positioning Numerically Controlled Machines. Electronic Industries Association, Engineering Department, 2001 Eye Street, NW, Washington, D.C. 200006. February 1979.
- Steve DiBartolomeo (1991). "D-codes, Apertures and Gerber Files". Artwork Conversion Software, Inc. Retrieved 16 October 2011.
- Google book entry on Gerber format: a subset of EIA RS-274-D ; plot data format reference book.
- Coombs, Clyde F. (September 2, 2007). Printed circuits handbook. McGraw-Hill Professional. p. 18.11. ISBN 978-0-07-146734-6. Retrieved April 3, 2011.
- "Ucamco's Revised Gerber Format Specification Now Online". ucamco.com. February 19, 2013. Retrieved February 15, 2013.
- "Ucamco Enhances Gerber File Format Specification". ucamco.com. November 22, 2013. Retrieved November 22, 2013.
- Mike Santarini (1/22/2002 2:33 PM EST). "ODB++ spec tapped for CAD-to-CAM data exchange". EE Times. Retrieved 29 September 2011.
- IPC-2581 Panel: A Spirited Discussion on PCB Data Transfer Formats, Richard Goering, Cadence Design Systems blog, October 2, 2011
- "JPCA Standards".