The Gerber Layer Format Specification 2021.02

The Gerber Layer Format

Specification

A format developed by Ucamco

Revision 2021.02

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Contents

Contents ........................................................................................................................ 2

Preface ........................................................................................................................... 7

1 Introduction .............................................................................................................. 8

1.1 Scope and Target Audience ................................................................................ 8

1.2 Further Resources .............................................................................................. 8

1.3 Reference Gerber Viewer ................................................................................... 8

1.4 Copyright and Intellectual Property ..................................................................... 9

2 Overview ................................................................................................................. 10

2.1 File Structure ..................................................................................................... 10

2.2 Apertures ........................................................................................................... 10

2.3 Graphical objects .............................................................................................. 11

2.4 Draws and Arcs ................................................................................................. 12

2.5 Operations (D01, D02, D03) ............................................................................. 13

2.6 Graphics State .................................................................................................. 14

2.7 Polarity .............................................................................................................. 16

2.8 Blocks ................................................................................................................ 17

2.9 Attributes ........................................................................................................... 17

2.10 Commands Overview ..................................................................................... 18

2.11 Processing a Gerber File ................................................................................ 19

2.12 Glossary .......................................................................................................... 21

2.13 Annotated Example Files ................................................................................ 24

Example: Two Square Boxes ................................................................... 24

Example: Polarities and Apertures ........................................................... 26

2.14

Conformance .................................................................................................. 30

3 Syntax ..................................................................................................................... 31

3.1 Character Set .................................................................................................... 31

3.2 Grammar Syntax ............................................................................................... 31

3.3 Commands ........................................................................................................ 33

3.4 Data Types ........................................................................................................ 35

Integers ...................................................................................................... 35

Decimals ..................................................................................................... 35

Strings ........................................................................................................ 35

Fields .......................................................................................................... 36

Names ........................................................................................................ 36

3.5

Full Grammar of the Gerber Format .................................................................. 37

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

3.6 File Extension, MIME Type and UTI ................................................................. 43

4 Graphics.................................................................................................................. 44

4.1 Comment (G04) ................................................................................................ 44

4.2 Coordinate Commands ..................................................................................... 45

Unit (MO) .................................................................................................... 45

Format Specification (FS) ........................................................................... 46

4.3

Aperture Definition (AD) .................................................................................... 47

AD Command ............................................................................................. 47

Zero-size Apertures .................................................................................... 48

Examples .................................................................................................... 48

4.4

Standard Aperture Templates ........................................................................... 49

Overview..................................................................................................... 49

Circle .......................................................................................................... 49

Rectangle ................................................................................................... 51

Obround ..................................................................................................... 52

Polygon ...................................................................................................... 53

Transparency of Holes ............................................................................... 54

4.5

Aperture Macro (AM) ......................................................................................... 55

Primitives .................................................................................................... 57

Exposure Parameter................................................................................... 66

Rotation Parameter .................................................................................... 67

Macro Variables and Expressions .............................................................. 68

Examples .................................................................................................... 69

4.6

Set Current Aperture (Dnn) ............................................................................... 73

4.7 Interpolation State Commands (G01,G02,G03,G75) ........................................ 74

Linear Interpolation (G01)........................................................................... 74

Circular Interpolation (G02, G03, G75) ....................................................... 75

4.8

Operations (D01/D02/D03) ............................................................................... 79

Overview..................................................................................................... 79

Interpolate (D01)......................................................................................... 81

Move (D02) ................................................................................................. 81

Flash (D03) ................................................................................................. 81

Example ..................................................................................................... 82

4.9

Aperture Transformations (LP, LM, LR, LS) ...................................................... 83

Overview..................................................................................................... 83

Load Polarity (LP) ....................................................................................... 85

Load Mirroring (LM) .................................................................................... 85

Load Rotation (LR) ..................................................................................... 85

Load Scaling (LS) ....................................................................................... 86

Examples .................................................................................................... 86

4.10

Region Statement (G36/G37) ......................................................................... 89

Region Overview ...................................................................................... 89

Region Statement Syntax ......................................................................... 90

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Valid Contours .......................................................................................... 90

Examples .................................................................................................. 92

Power and Ground Planes ..................................................................... 108

4.11

Block Aperture (AB) ...................................................................................... 111

Overview of block apertures ................................................................... 111

AB Statement Syntax ............................................................................. 111

Usage of Block Apertures ....................................................................... 112

Example ................................................................................................. 113

4.12

Step and Repeat (SR) .................................................................................. 115

4.13 End-of-file (M02) ........................................................................................... 118

4.14 Numerical Accuracy ...................................................................................... 119

Visualization ........................................................................................... 119

Image Processing ................................................................................... 119

5 A

ttributes .............................................................................................................. 121

5.1 Attributes Overview ......................................................................................... 121

5.2 File Attributes (TF) .......................................................................................... 123

5.3 Aperture Attributes (TA) .................................................................................. 123

Aperture Attributes on Regions ................................................................ 124

5.4

Object Attributes (TO) ..................................................................................... 124

5.5 Delete Attribute (TD) ....................................................................................... 125

5.6 Standard Attributes ......................................................................................... 126

Overview................................................................................................... 126

.Part .......................................................................................................... 128

.FileFunction ............................................................................................. 129

.FilePolarity ............................................................................................... 133

.SameCoordinates .................................................................................... 134

.CreationDate ........................................................................................... 134

.GenerationSoftware................................................................................. 135

.ProjectId .................................................................................................. 135

.MD5 ......................................................................................................... 136

.AperFunction ......................................................................................... 138

.DrillTolerance ........................................................................................ 148

.FlashText ............................................................................................... 148

.N (Net) ................................................................................................... 149

.P (Pin) ................................................................................................... 151

.C (Component) ...................................................................................... 153

5.7

Text in the Image ............................................................................................ 154

5.8 Examples ........................................................................................................ 155

6 PCB Fabrication and Assembly Data ................................................................. 157

6.1 Structure .......................................................................................................... 157

6.2 Mandatory Attributes ....................................................................................... 157

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

6.3 Alignment ........................................................................................................ 157

6.4 Pads ................................................................................................................ 157

6.5 The Profile ....................................................................................................... 157

6.6 Drill/rout files ................................................................................................... 158

6.7 Drawings and Data .......................................................................................... 162

6.8 The CAD Netlist .............................................................................................. 162

6.9 PCB Assembly Data .................................................. 165

7 Errors and Bad Practices .................................................................................... 168

7.1 Errors .............................................................................................................. 168

7.2 Bad Practices .................................................................................................. 171

8 Deprecated Format Elements ............................................................................. 173

8.1 Deprecated Commands .................................................................................. 173

Overview................................................................................................... 173

Axis Select (AS)........................................................................................ 174

Image Name (IN) ...................................................................................... 175

Image Polarity (IP) .................................................................................... 175

Image Rotation (IR) .................................................................................. 176

Load Name (LN) ....................................................................................... 177

Mirror Image (MI) ...................................................................................... 177

Offset (OF) ............................................................................................... 178

Scale Factor (SF) ..................................................................................... 179

Single-quadrant arc mode (G74) ............................................................ 181

8.2 D

eprecated Command Options ....................................................................... 185

Format Specification (FS) Options ........................................................... 185

Rectangular Hole in Standard Apertures .................................................. 186

Draws and Arcs with Rectangular Apertures ............................................ 187

Macro Primitive Code 2, Vector Line ........................................................ 188

Macro Primitive Code 22, Lower Left Line ................................................ 188

Macro Primitive Code 6, Moiré ................................................................. 189

8.3 D

eprecated Syntax Variations ......................................................................... 190

Combining G01/G02/G03 and D01 in a single command. ....................... 190

Coordinate Data without Operation Code ................................................. 191

Style Variations in Command Codes ........................................................ 191

Deprecated usage of SR .......................................................................... 191

8.4 D

eprecated Attribute Values ........................................................................... 191

8.5 Standard Gerber (RS-274-D) .......................................................................... 193

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

9 References ............................................................................................................ 194

10 History ................................................................................................................... 195

11 Revisions .............................................................................................................. 197

11.1 Revision 2021.02 .......................................................................................... 197

11.2 Revision 2020.09 – X3 .................................................................................. 197

11.3 Revision 2019.09 .......................................................................................... 197

11.4 Revision 2019.06 .......................................................................................... 197

11.5 Revision 2018.11 .......................................................................................... 198

11.6 Revision 2018.09 .......................................................................................... 198

11.7 Revision 2018.06 .......................................................................................... 198

11.8 Revision 2018.05 .......................................................................................... 198

11.9 Revision 2017.11 .......................................................................................... 198

11.10 Revision 2017.05 .......................................................................................... 199

11.11 Revision 2017.03 .......................................................................................... 199

11.12 Revision 2016.12 – Nested step and repeat ................................................. 199

11.13 Revision 2016.11 .......................................................................................... 199

11.14 Revision 2016.09 .......................................................................................... 200

11.15 Revision 2016.06 .......................................................................................... 200

11.16 Revision 2016.04 .......................................................................................... 200

11.17 Revision 2016.01 .......................................................................................... 200

11.18 Revision 2015.10 .......................................................................................... 201

11.19 Revision 2015.07 .......................................................................................... 201

11.20 Revision 2015.06 .......................................................................................... 201

11.21 Revision J3 (2014 10) ................................................................................... 201

11.22 Revision J4 (2015 02) ................................................................................... 201

11.23 Revision J2 (2014 07) ................................................................................... 201

11.24 Revision J1 (2014 02) – X2 .......................................................................... 202

11.25 Revision I4 (2013 10) .................................................................................... 202

11.26

Revision I3 (2013 06) .................................................................................... 202

11.27 Revision I2 (2013 04) .................................................................................... 202

11.28 Revision I1 (2012 12) .................................................................................... 202

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Preface

The Gerber format is the de facto open standard for printed circuit board (PCB) design data

transfer. As an UTF-8 human-readable format Gerber is portable and easy to debug. It is

compact and unequivocal, and simple - there are just 27 commands. Every PCB design system

outputs Gerber files and every PCB fabrication software inputs them. Implementations are

thoroughly field-tested. Gerber's widespread availability allows PCB professionals to exchange

PCB design data securely and efficiently. It has been called “the backbone of the electronics

fabrication industry”.

Gerber is at its core is an open vector format for 2D binary images specifying PCB copper

layers, solder mask, legend, etc. Attributes transfer meta-information with the images. Attributes

are akin to labels expressing, for example, that an image represents the top solder mask, or that

a pad stack is a via or component stack, and which components are positioned where.

Attributes transfer the meta-information necessary for fabrication and assembly. A set of well-

constructed Gerber files reliably and productively transfers PCB fabrication from design to

fabrication, and component information to assembly.

Although other data formats have appeared, they have not displaced Gerber. The reason is

simple. Any problems in PCB fabrication data transfer are not due to limitations in the Gerber

format but are due to poor practices and poor implementations. The new formats are more

complicated and less transparent. To quote Günther Schindler: "“There are no superfluous,

production-specific attributes like in other CAM formats. Gerber X2 is simple and tidy.” Poor

practices and poor implementations in unfamiliar, new and complicated formats are more

damaging than in a well-known, well-tested and simple format. The industry has not adopted

new formats. Gerber remains the standard.

Ucamco continuously clarifies this document and adapts it to current needs based on input from

the user community. Ucamco thanks the individuals that help us with comments, criticism, and

suggestions.

The Gerber format was named after Joseph Gerber, who fled his native Austria from the Nazis,

and arrived in the USA as a teenager, alone and penniless. With his technical genius and work

ethic he became a very successful inventor and technical entrepreneur. The American dream

come true. Mr. Gerber pioneered photoplotting in PCB fabrication, which is the link with the

format. Ucamco is honored to look after a format called after this brilliant man.

The emergence of Gerber as a standard for PCB fabrication data is the result of efforts by many

individuals who developed outstanding software for Gerber files. Without their dedication there

would be no standard format in the electronics fabrication industry. Ucamco thanks these

dedicated individuals.

Karel Tavernier

Managing Director,

Ucamco

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

1 Introduction

1.1 Scope and Target Audience

This document specifies the Gerber layer format, an UTF-8 format for representing PCB

fabrication data. The Gerber format is the de facto standard in the printed circuit board (PCB).

This specification is intended for developers and users of Gerber software. A basic knowledge

of PCB design or fabrication is assumed, and knowledge about PCB CAD/CAM is helpful.

1.2 Further Resources

The Ucamco website contains articles about the use of the Gerber format as well as sample

files. For more information about Gerber or Ucamco see www.ucamco.com

, or mail to

[email protected]

Ucamco strives to make this specification easy to read and unequivocal. If you find a part of this

specification unclear, please ask. Your question will be answered, and it will be considered to

improve this document. We are grateful for any suggestion for improvement.

1.3 Reference Gerber Viewer

Ucamco provides a reference Gerber file viewer - free of charge – at gerber-viewer.ucamco.com.

The Reference Gerber Viewer provides an easy-to-use reference for both X1 and X2 Gerber

files. - the utmost care was taken to display valid Gerber files correctly. It gives a clear warning

on risky errors. It is a convenient complement to the written specification. (The specification has

precedence if it conflicts with the viewer.)

The Reference Gerber Viewer is an easy tool to review PCB fabrication data. For completeness,

it also displays drill files in NC format and netlists in IPC-D-356 files. If X2 is used the layer

structure is displayed, and the function of all objects can be checked – e.g. whether a drill hole is

a via or a component hole.

As the Reference Gerber Viewer is a cloud-based on-line web service there is no software to

download, install and maintain –it is always up to date. It is simple and easy to learn. It offers the

following benefits:

• For developers, it provides an easy way to test their Gerber output and to answer

questions about the interpretation of the specification.

• For users of Gerber files, it provides an easy way to check the file they have received or

are about to send, and to settle discussions about the interpretation of a file.

It is allowed to integrate a link to the online reference viewer in your website. Email us a

[email protected]

for more information.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

1.4 Copyright and Intellectual Property

content may be re-distributed, reproduced or published, modified or not, translated or not, in any

form or in any way, electronically, mechanically, by print or any other means without prior written

permission from Ucamco. One reason Ucamco must retain its copyrights in the Gerber Format®

specification is to maintain the integrity of the standard.

The information contained herein is subject to change without prior notice. Revisions may be

issued from time to time. This document supersedes all previous versions. Users of the Gerber

Format

, especially software developers, must consult www.ucamco.com to determine whether

new revisions were issued.

Ucamco developed the Gerber Format

. All intellectual property contained in it is solely owned

by Ucamco. By publishing this document Ucamco has not granted any license or alienated any

rights to the intellectual property contained in it. To use this intellectual property, developers of

software interfaces based on this format specification must make a reasonable effort to comply

with the latest revision of the specification; this is necessary to maintain the integrity of the

standard.

Gerber Format

is a Ucamco registered trademark. By using this document, developing

software interfaces based on this format or with the name Gerber Format

, users agree not to (i)

rename the Gerber Format

; (ii) associate the Gerber Format

with data that does not conform

to the Gerber format specification; (iii) develop derivative versions, modifications or extensions

without prior written approval by Ucamco; (iv) make alternative interpretations of the data; (v)

communicate that the Gerber Format

is not owned by Ucamco, explicitly or implied.

The material, information and instructions are provided AS IS without warranty of any kind,

either express or implied. Ucamco does not warrant, or makes any representations regarding,

the use of the information contained herein, the results of its use, non-infringement,

merchantability, or fitness for a particular purpose . Ucamco shall not be liable for any direct,

indirect, consequential, or incidental damages arising out of the use or inability to use the

information contained herein. You are solely responsible for determining the appropriateness of

using this information and assume any risks associated with it.

All product names cited are trademarks or registered trademarks of their respective owners.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

2 Overview

2.1 File Structure

The Gerber layer format is a 2D bi-level vector image format: the image is defined by resolution-

independent graphical objects. Bi-level or binary images in each point take one of two possible

values, typically labeled black and white.

A single Gerber file specifies a single image. A Gerber file is complete: it does not need sidecar

files or external parameters to be interpreted. One Gerber file represents one image. One image

needs one file only.

A Gerber file is a stream of commands. The commands create a stream of graphical objects

(see 2.2) that are put on the image plane in order to create the final image. Other commands

add attributes to those objects or to the overall file. Attributes are akin to label that add meta

information to the objects without affecting the image.

The commands are ordered. A Gerber file can be processed in a single pass. Names,

parameters and objects must be defined before they are used.

A Gerber file uses printable 7-bit ASCII characters for all commands and names defined in the

specification – this fully covers image generation. For attribute values the complete UTF-8

encoding is allowed, as they can be human defined. This makes the files printable and human

readable.

Below is a small example Gerber file that creates a circle of 1.5 mm diameter centered on the

origin. There is one command per line.

%FSLAX26Y26*%

%MOMM*%

%ADD100C,1.5*%

D100*

X0Y0D03*

M02*

2.2 Apertures

An aperture is a 2D plane figure. Aperture typically have simple shapes, as in the examples

below, but complex shapes can be created.

Apertures are the basic tools to create graphic images in the plane. They can be replicated in

the plane, optionally rotated, mirrored, and scaled. This replication is called flashing, from the

days when these things were done with NC optical equipment. Flashes are used to create pads.

Apertures can also be used as a pen to draw lines in the plane. This is called interpolating or

stroking. Stroking creates traces on the PCB.

There are several methods to define apertures: via standard apertures, macro apertures and

block apertures. Apertures are identified by a unique aperture number.

The AD (Aperture Define) command creates an aperture based on an aperture template and

parameter values giving it a unique D code or aperture number for later reference.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

There are two kinds of apertures templates:

 Standard apertures. They are pre-defined: the circle (C), rectangle (R), obround (O) and

regular polygon (P). See 4.4.

 Macro apertures. They are created with the AM (Aperture Macro) command. Any shape

and parametrization can be created. They are identified by their given name. (See 4.4.6).

Standard apertures can be considered as built-in macro apertures. The example AD command

below creates an aperture. The aperture number is 123. It uses the standard aperture R with

parameters 2.5 and 1.5 mm to creates a rectangle of 2.5 by 1.5 mm.

%ADD123R,2.5X1.5%

Macros are a powerful feature of the Gerber format. Templates of any shape and parameters

can be created. A file writer can easily define the apertures it needs. A file reader can handle

any such aperture by implementing a single macro function. This single flexible mechanism

replaces the need for a large - but always insufficient - set of built-in apertures. New apertures

can be created without extending the format.

Block apertures are an ordered set of graphical objects. Block apertures are not created with

templates. They are created by an AB statement, which creates a block aperture with the

standard flashes and strokes of the Gerber format, and assigns an aperture number to it (see

2.8).

An aperture has an origin. When an aperture is flashed, its origin is positioned at the

coordinates in the flash command (see 4.1). The origin of a standard aperture is its geometric

center. The origin of a macro aperture is the origin used in the AM command defining the

macro. The origin of a block aperture is the origin used in the AB command defining the block.

2.3 Graphical objects

A Gerber file creates an ordered stream of graphical objects. A graphical object represents a

plane figure. It has a shape, a size, a position and a polarity (dark or clear). The stream of the

graphical objects creates the final image by superimposing the objects on the plane in the order

of the stream, with dark polarity objects darkening the plane and clear ones erasing all dark

areas under them.

There are four types of graphical objects:

 Draws are straight-line segments, stroked with the current aperture, which must be a solid

circular one.

 Arcs are circular segments, stroked with the current aperture, which must be a solid

circular one.

 Flashes are replications of the current aperture in the image plane. Any valid aperture can

be flashed (see 4.8.4). An aperture is typically flashed many times.

 Regions are defined by its contour (see 4.10.1). A contour is a closed sequence of

connected linear or circular segments.

In PCB copper layers, tracks are typically represented by draws and arcs, pads by flashes and

copper pours by regions. Tracks is then a generic name for draws and arcs.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

2.4 Draws and Arcs

A draw object is created by a command with D01 code in linear interpolation mode. The

command strokes the straight-line segment with a solid circle standard aperture resulting in a

line with thickness equal to the diameter of the circle and round endings.

An arc object is created by a command with D01 code in circular interpolation mode. In this

case the command results in stroking an arc segment with a solid circle standard aperture. The

arc has round endings, and its thickness is equal to the diameter of the circle. An arc object

cannot be created using a rectangle or any other aperture.

The solid circle standard aperture is the only aperture allowed for creating draw or arc objects.

Other standard apertures or macro apertures that fortuitously have a circular shape are not

allowed.

A circle aperture with diameter zero can be used for creating a draw or an arc. It creates

graphical objects without image which can be used to transfer non-image information, e.g. an

outline.

"Zero-length draws and arcs are allowed. As an image, the resulting image is identical to a flash

of the same aperture. However the resulting graphical object is a draw/arc object and not a flash

object, which affects the meaning. Do not use zero-length draws to represent pads. Pads must

be represented by flashes."

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

2.5 Operations (D01, D02, D03)

D01, D02 and D03 are the operations. An operation is a command consisting of coordinate data

followed by an operation code. Operations create the graphical objects and/or change the

current point by operating on the coordinate data.

Example:

X100Y100D01*

X200Y200D02*

X300Y-400D03*

The operations have the following effect.

 D02 moves the current point (see 2.5) to the coordinate pair. No graphical object is created.

 D01 creates a linear or circular line segment by interpolating from the current point to the

coordinate pair. Outside a region statement (see 2.5) these segments are converted to

draw or arc objects by stroking them with the current aperture (see 2.4). Within a region

statement these segments form a contour defining a region (see 4.10). The effect of D01,

e.g. whether a straight or circular segment is created, depends on the graphics state (see

2.5).

 D03 creates a flash object by flashing (replicating) the current aperture. The origin of the

current aperture is positioned at the specified coordinate pair.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

2.6 Graphics State

The graphics state is a set of parameters affecting the result of the operation codes (see 2.5).

Before an operation code is issued all graphics state parameters affecting it must be defined.

The most important graphics state parameter is the current point. This is a point in the image

plane set implicitly by each operation command (D01, D02, D03) to the coordinates contained in

that operation command after finishing.

All other graphics state parameters are set explicitly by corresponding commands. Their values

remain constant until explicitly changed.

The table below lists the graphics state parameters. The column ‘Constant or variable’ indicates

whether a parameter remains fixed during the processing of a file or whether it can be changed.

The column ‘Initial value’ is the default value at the beginning of each file; if the default is

undefined the parameter value must be explicitly set by a command in the file before it is first

used.

Graphics state

parameter

Value range

Constant or

variable during

file processing

Initial

value

Coordinate Parameters

Coordinate format

Coordinate resolution. See the FS command in 4.1

Constant

Undefined

Unit

mm or inch. See MO command in 4.2.1

Constant

Undefined

Generation state

Current point

Point in plane

Variable

Undefined

Current aperture

Used for interpolating and flashing.

See D01 and D03 commands in 4.7

Variable

Undefined

Interpolation state

Linear, clockwise circular, counterclockwise circular

See G01, G02, G03 commands in 4.7

Variable

Undefined

Aperture transformation state

Polarity

Dark or clear. See the LP command in 4.9.2

Variable

Dark

Mirroring

See the LM command in 4.9.3

Variable

No mirror

Rotation

See the LR command in 4.9.4

Variable

No rotation

Scaling

See the LS command in 4.9.5

Variable

No scaling

Graphics state parameters

The graphics state determines the effect of an operation. If a parameter that is required to

perform an operation is undefined at the time of the operation the Gerber file is invalid. A

graphics state parameter that is not needed can remain undefined.

The relevance of the graphics state parameters for the operations is represented in the table

below.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Graphics state

Operation codes

D01

D02

D03

Coordinate format

Yes

Unit

Yes

Current point Yes (interpolation

starting point)

No No

Current aperture Yes in a region

statement.

No outside a region

statement

No Yes

Interpolation mode

Yes

Polarity

Yes

Mirroring

Yes

Rotation

Yes

Scaling

Yes

Relevance of graphics state parameters for operation codes

If a table cell contains ‘Yes’ it means the graphics state parameter is relevant for the

corresponding operation. Thus the graphics state parameter must be defined before the

operation code is used in the file. If the parameter does not have an automatically assigned

initial value it must be explicitly set by the corresponding command.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

2.7 Polarity

The final image of the Gerber file is created by superimposing the objects in the order of their

creation. Objects have a polarity, either clear or dark. Objects can overlap. A dark polarity object

darkens its image in the plane. A clear polarity object clears its image in all objects beneath it

(generated before). Subsequent dark objects may again darken the cleared area. See

illustration below. Another example is in 4.10.4.6.

1. Superimposing objects with dark and clear polarities

An object is totally dark or totally clear. It cannot be partially dark and partially clear.

The order of superimposed objects with different polarities affects the final image.

The LP command sets the polarity mode, a graphics state parameter (see 4.9). Objects that are

created when the polarity mode is dark are dark; when the mode is clear the objects are clear.

Dark polarity

Clear polarity

Dark polarity

Image plane Graphics objects

[Not supported by viewer]

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

2.8 Blocks

A block is a substream of graphical objects that can be added one or more times to the final

graphical objects stream. Blocks can be mirrored, rotated, scaled, shifted and its polarity can be

toggled. By using blocks sub-images that occur multiple times must only be defined once, thus

slashing file size, boosting processing speed and preserving the information that these sub-

images are identical.

A block is not a macro of commands called repeatedly in the command stream. The command

stream is processed sequentially, in one pass, without procedure or macro calls. Gerber is not a

programming language.

Blocks can contain objects with different polarities (LPD and LPC). Blocks can overlap.

The origin of the block is the (0, 0) point of the file coordinate space.

Once a block is added to the graphical objects stream its objects become part of the overall

stream. Their appearance does not depend on whether they were part of a block or not. Only the

order is important. A clear object in a block clears all objects beneath it, not only the objects

contained in the block.

There are two commands to create a block: SR and AB.

2.9 Attributes

Attributes add meta-information to a Gerber file. These are akin to labels providing additional

information about the file or features within. Examples of such meta-information are:

 The function of the file: is it the top solder mask, or the bottom copper layer etc.

 The function of a pad: is the pad a component pad, or a via pad, or a fiducial, etc.

Example:

This command defines an attribute indicating the file represents the top solder mask.

%TF.FileFunction,Soldermask,Top*%

Attributes can be attached to objects, apertures or to the complete file.

Attributes do not affect the image itself, they only add meta-information to the data. A Gerber

reader will generate the correct image even if it ignores some or all attributes.

The attribute syntax provides a flexible and standardized way to add meta-information to the

images, independent of the specific semantics or application.

Attributes are needed when PCB data is transferred from design to fabrication. The PCB

fabricator needs more than just the image. For example, the solder mask around via pads

needs dedicated clearances to achieve the specified via protection. Without these attributes, the

fabricator has to guess which objects represent a via; figuring this out manually is a time

consuming and error-prone process. The attributes transfer the design intent from CAD to CAM

in an unequivocal and standardized manner. This is sometimes rather grandly called “adding

intelligence to the image”.

Gerber files containing attribute commands (TF, TA, TO, TD) are called Gerber X2 files, files

without attributes Gerber X1 files.

Attributes are described in detail in the chapter 5.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

2.10 Commands Overview

Command

Long name

Description

Ref.

G04

Comment

A human readable comment, does not affect the image.

4.1

Mode

Sets the unit to mm or inch.

4.2.1

Format specification

Sets the coordinate format, e.g. the number of decimals.

4.2.2

Aperture define

Defines a template-based aperture, assigns a D code to it.

4.3

Aperture macro

Defines a macro aperture template.

4.5

Dnn (nn≥10)

Sets the current aperture to D code nn.

4.6

D01

Interpolate operation

Outside a region statement D01 creates a draw or arc

object with the current aperture. Inside it adds a draw/arc

segment to the contour under construction. The current

point is moved to draw/arc end point after the creation of

the draw/arc.

4.8.2

D02

Move operation

D02 moves the current point to the coordinate in the

command. It does not create an object.

4.8.3

D03

Flash operation

Creates a flash object with the current aperture. The

current point is moved to the flash point.

4.8.4

G01

Sets linear/circular mode to linear.

4.7.1

G02

Sets linear/circular mode to clockwise circular.

4.7.2

G03

Sets linear/circular mode to counterclockwise circular.

4.7.2

G75

A G75 must be called before creating the first arc.

4.7.2

Load polarity

Loads the polarity object transformation parameter.

4.9.2

Load mirroring

Loads the mirror object transformation parameter.

4.9.3

Load rotation

Loads the rotation object transformation parameter.

4.9.4

Load scaling

Loads the scale object transformation parameter.

4.9.5

G36

Starts a region statement which creates a region by

defining its contours.

4.10.

G37

Ends the region statement.

4.10

Aperture block

Opens a block aperture statement and assigns its aperture

number or closes a block aperture statement.

4.11

Step and repeat

Open or closes a step and repeat statement.

4.11

Attribute on file

Set a file attribute.

5.2

Attribute on aperture

Add an aperture attribute to the dictionary or modify it.

5.3

Attribute on object

Add an object attribute to the dictionary or modify it.

5.4

Attribute delete

Delete one or all attributes in the dictionary.

5.5

M02

End of file.

4.13

Command Overview

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

2.11 Processing a Gerber File

2. Gerber file processing diagram

The syntax parser reads the Gerber file and produces the stream of commands for the

commands processor. The commands processor is responsible for handling the stream of

Syntax parser

Gerber file

Image plane

Stream of

commands

Stream of

graphics objects

Aperture templates

dictionary

AM command

M02 command

Graphics state

Graphics

object

Commands processor

Apertures dictionary

AD command

Legend

A B

Command

As the result of Command execution A

forces B to change or perform a task

A affects B

A B

A passes stream of data to B

A B

A processes B

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

commands and as the result it generates the stream of graphical objects. All the created objects

are superimposed on the image plane in order of their creation.

The graphics state is a core part of the command processor. How the processor creates

graphical objects from the operation codes (see 2.5) depends on the graphics state.

Conversely, the processor modifies the graphics state when processing certain commands (see

2.5).

The aperture template dictionary holds all the templates available. The AD command (see 4.3)

instantiates the templates to apertures and adds them to the aperture library. Standard, or built-

in, aperture templates are automatically added to the dictionary when file processing is started.

Macro aperture templates are created with an AM command (see 4.5); they are added when the

AM command is processed.

The current aperture is a graphics state parameter that is maintained by Dnn command (see

4.6). When the processor executes a Dnn command a referenced aperture from apertures

dictionary is set as the current aperture.

The graphics state also affects the generation of aperture templates and apertures: the

templates and apertures depend on ‘coordinate format’ and ‘unit’ graphics state parameters

(see 2.5).

The graphical object stream is without state. Objects are superimposed as they are, in their

order of appearance.

After processing the M02 command (see 4.13) the processor interrupts the syntax parser and

stops the graphical objects generation.

The image from above illustrates the processing of a Gerber file without attributes.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

2.12 Glossary

AB statement: A statement defining a block aperture.

Aperture: A 2D shape that is used for stroking or flashing. (The name is historic; vector

photoplotters exposed images on lithographic film by shining light through an opening,

called aperture.) They are identified by an aperture number.

Aperture macro: The content of an Aperture Macro (AM) command. Defines a custom

aperture template by combining built-in primitives.

Aperture template: A template is used to create the specific apertures used in the file.

The AD command defines the parameters to instantiate the template to a defined

aperture. There are three types of templates: standard or built-in apertures, macro

apertures and block apertures.

Aperture templates dictionary: The object that holds all the aperture templates.

Apertures dictionary: The object that holds all the apertures.

Arc: A graphical object created by a D01 command in a circular interpolation mode.

Attribute: Metadata that is attached to the file or to objects in it; it provides extra

information without affecting the image.

Attributes dictionary: The object that holds all the current attributes during the

processing of a Gerber file.

Bi-level image: A two-dimensional (2D) image represented by two colors, usually

black and white.

Block: A substream of graphical objects that can be added to the final objects stream.

Circular interpolation: Creating a circular segment (circular arc) that is either an arc

graphical object or used as a circular contour segment.

Clear: Clearing or erasing part of the image in the image plane. When a graphical

object with clear polarity is added to the stream it erases its shape from any image that

was already there.

Command: Commands are the basic unit of a Gerber file. Commands create graphical

objects, define apertures, manage attributes, modify the graphics state and so on. For

historic reasons, there are two syntax styles for commands: word commands and

extended commands.

Command code: A code that identifies the command.

Contour: A closed sequence of connected linear or circular segments. Contours are

used to create regions or outline primitives in macro apertures.

Coordinate data: A number whose interpretation is determined by the FS command. It

is used to specify the X and Y coordinates of a point in the image plane and a distance

or offset in the X and Y direction.

Coordinate format: The specification of how to convert coordinate data to

coordinates. It is file-dependent and is defined by an FS command.

Current aperture: The graphics state parameter that specifies the last aperture

selected by a Dnn command. The current aperture is always used to create flashes,

draws and arcs.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Current point: The graphics state parameter that specifies the point in the plane used

as a begin point of a circular or linear interpolation or as the location flash.

Darken: Darken the shape of a graphical object on the image plane; this happens

when a graphical object with dark polarity added to the image.

Draw: A graphical object created by D01 command in linear interpolation mode.

File image: The bi-level image that is the visual representation of a Gerber file. It is

created by superimposing the graphical objects in the plane.

Flash: A graphical object created by D03 or flash command.

Gerber file: A file in the Gerber format.

Gerber format: The vector image format defined by the current specification and used

for representing a bi-level image.

Graphical object: A graphical object is a 2D object with a shape, a size, a position in

the plane and a polarity (dark or clear). It is of one of the following types: flash, draw,

arc or region. The file image is created by superimposing graphical objects on the

image plane. Attributes can optionally be attached to a graphical object.

Graphics state: The set of parameters that at each moment determine how the

operation codes create graphical objects. For example, it determines whether a D01

operation code creates a draw or an arc.

Header: The part of the file from the file beginning to the point where the first operation

code is encountered. The header typically holds the definitions of file attributes,

aperture definitions, scale and unit.

Image plane: The 2D plane in which the image defined by the file is created.

Interpolation mode: The graphics state parameter defining how the D01 operation

behaves.

Linear interpolation: Creating a straight segment that is either converted to a draw

graphical object or used as a linear contour segment.

Macro aperture: An aperture template defined using AM command.

Operation: A command containing one of the operation codes D01, D02 or D03 and

coordinate data. The operation code defines the type of the operation that is performed

with the coordinate data. Operations may create graphical objects, create contours,

and change the current point of the graphics state.

Polarity: A graphics state parameter that can take the value dark or clear. It

determines the polarity of the graphical objects generated. Dark means that the object

marks the image plane in dark and clear means that the object clears or erases

everything underneath it. See also ‘Darken’ and ‘Clear’.

Region: A graphical object with an arbitrary shape defined by its contour.

Region statement: A statement creating a region by defining its contour.

Resolution: The distance expressed by the least significant digit of coordinate data.

Thus, the resolution is the step size of the grid on which all coordinates are defined.

SR statement: A statement defining a block and step & repeating it.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Standard aperture: A built-in aperture template.

Standard attribute: A built-in attribute with a pre-defined semantics. See also user

attribute.

Statement: A coherent sequence of commands delimited by an open and close

command defining a higher-level structure.

Stroke: To create a draw or an arc graphical object with the current aperture.

Track: Either a draw or an arc. Typically used for conductive traces on a PCB.

Unit: The measurement unit ‘mm’ or ‘inch’ used to interpret the coordinate data. The

effective unit is stored as the value of the corresponding graphics state parameter.

User attribute: A third-party defined attribute to extend the format with proprietary

meta-information.

Word: A sequence of characters ending with the ‘*’ delimiter character. It is the low-

level syntactical element of a Gerber file used to build commands.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

2.13 Annotated Example Files

These annotated sample files illustrate the Gerber layer format to make the formal specification

easier to read.

Example: Two Square Boxes

This example represents a single polarity image with two square boxes.

3. Example: two square boxes

Syntax Annotation

G04 Ucamco ex. 1: Two

square boxes*

A comment

%MOMM*%

Unit set to mm

%FSLAX25Y25*%

Format specification:

Leading zero’s omitted

Absolute coordinates

Coordinates in 3 integer and.6 fractional digits.

%TF.Part,Other,example*%

Attribute: the file does not describe a PCB part - it is just an

example

%LPD*%

Set the polarity to dark

%ADD10C,0.010*%

Define aperture number 10 as a 0.01 mm circle

D10*

Select aperture 10 as current aperture

X0Y0D02*

Set current point to (0, 0)

G01*

Set linear interpolation mode

X500000Y0D01*

Create draw graphical object with the current aperture (10): start point

is the current point (0,0), end point is (5, 0)

Y500000D01*

Create draw with the current aperture: (5, 0) to (5, 5)

X0D01*

Create draw with the current aperture: (5, 5) to (0, 5)

Y0D01*

Create draw with the current aperture: (0, 5) to (0, 0)

X600000D02*

Set current point to (6, 0)

X1100000D01*

Create draw with the current aperture: (6, 0) to (11, 0)

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Syntax Annotation

Y500000D01*

Create draw with the current aperture: (11, 0) to (11, 5)

X600000D01*

Create draw with the current aperture: (11, 5) to (6, 5)

Y0D01*

Create draw with the current aperture: (6, 5) to (6, 0)

M02*

End of file

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Example: Polarities and Apertures

This example illustrates the use of polarities and various apertures.

4. Example: various shapes

Syntax Annotation

G04 Ucamco ex. 2: Shapes*

A comment

G04 Ucamco ex. 2: Shapes*

Comment

%MOMM*%

Units are mm

%FSLAX36Y36*%

Format specification:

Leading zero’s omitted

Absolute coordinates

Coordinates in 3 integer and.6 fractional digits.

%TF.FileFunction,Other,Sample*

Attribute: the is not a PCB layer, it is just an

example

G04 Define Apertures*

Comment

%AMTARGET125*

Define the aperture macro ‘TARGET125’

6,0,0,1.25,.1,0.1,3,0.03,1.50,0*%

Use moiré primitive in the macro

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Syntax Annotation

%AMTHERMAL80*

Define the aperture macro ‘THERMAL80’

7,0,0,0.800,0.550,0.125,45*%

Use thermal primitive in the macro

%ADD10C,0.1*%

Define aperture 10 as a circle with diameter 0.1 mm

%ADD11C,0.6*%

Define aperture 11 as a circle with diameter 0.6 mm

%ADD12R,0.6X0.6*%

Define aperture 12 as a rectangle with size 0.6 x 0.6 mm

%ADD13R,0.4X1.00*%

Define aperture 13 as a rectangle with size 0.4 x 1 mm

%ADD14R,1.00X0.4*%

Define aperture 14 as a rectangle with size 1 x 0.4 mm

%ADD15O,0.4X01.00*%

Define aperture 15 as an obround with size 0.4 x 1 mm

%ADD16P,1.00X3*%

Define aperture 16 as a polygon with 3 vertices and

circumscribed circle with diameter 1 mm

%ADD18TARGET125*%

Define aperture 18 as an instance of macro aperture

‘TARGET125’ defined earlier

%ADD19THERMAL80*%

Define aperture 19 as an instance of macro aperture

‘THERMAL80’ defined earlier

G04 Start image generation*

A comment

D10*

Select aperture 10 as current aperture

X0Y2500000D02*

Set the current point to (0, 2.5) mm

G01*

Set linear interpolation mode

X0Y0D01*

Create draw with the current aperture

X2500000Y0D01*

Create draw with the current aperture

X10000000Y10000000D02*

Set the current point

X15000000D01*

Create draw with the current aperture

X20000000Y15000000D01*

Create draw with the current aperture

X25000000D02*

Set the current point.

Y10000000D01*

Create draw with the current aperture

D11*

Select aperture 11 as current aperture

X10000000Y10000000D03*

Create flash with the current aperture (11) at (10, 10).

X20000000D03*

Create a flash with the current aperture at (20, 10).

Y is modal.

X25000000D03*

Create a flash with the current aperture at (25, 10).

Y is modal.

Y15000000D03*

Create a flash with the current aperture at (25, 15).

X is modal.

X20000000D03*

Create a flash with the current aperture at (20, 15).

Y is modal.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Syntax Annotation

D12*

Select aperture 12 as current aperture

X10000000Y15000000D03*

Create a flash with the current aperture at (10, 15)

D13*

Select aperture 13 as current aperture

X30000000Y15000000D03*

Create a flash with the current aperture at (30, 15)

D14*

Select aperture 14 as current aperture

Y12500000D03*

Create a flash with the current aperture at (30, 125)

D15*

Select aperture 14 as current aperture

Y10000000D03*

Create a flash with the current aperture at (30, 10)

D10*

Select aperture 10 as current aperture

X37500000Y10000000D02*

Set the current pointt

G75*

Must be called before an arc is created

G03*

Set counterclockwise circular interpolation mode

X37500000Y10000000I2500000J0D01*

Create full circular arc with the current aperture (10).

D16*

Set the current aperture: use aperture 16

X34000000Y10000000D03*

Create a flash with the current aperture 16

X35000000Y9000000D03*

Create a flash with the current aperture 16 again

G36*

Start a region statement

X5000000Y20000000D02*

Set the current point to (5, 20)

G01*

Set linear interpolation mode

Y37500000D01*

Create linear segment of the contour

X37500000D01*

Create linear segment of the contour

Y20000000D01*

Create linear segment of the contour

X5000000D01*

Create linear segment of the contour

G37*

Close the region statement

This creates the region by filling the created contour

D18*

Select aperture 18 as current aperture

X0Y38750000D03*

Create a flash with the current aperture (18)

X38750000Y38750000D03*

Create a flash with the current aperture

%LPC*%

Set the polarity to clear

G36*

Start the region statement

X10000000Y25000000D02*

Set the current point to (10, 25)

Y30000000D01*

Create linear segment

G02*

Set clockwise circular interpolation mode

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Syntax Annotation

X12500000Y32500000I2500000J0D01*

Create clockwise circular segment with radius 2.5

G01*

Set linear interpolation mode

X30000000D01*

Create linear segment

G02*

Set clockwise circular interpolation mode

X30000000Y25000000I0J-3750000D01*

Create clockwise circular segment with radius 3.75

G01*

Set linear interpolation mode

X10000000D01*

Create linear segment

G37*

Close the region statement, creates region object

%LPD*%

Set the polarity to dark

D10*

Select aperture 10 as current aperture

X15000000Y28750000D02*

Set the current point

X20000000D01*

Create draw with the current aperture

D11*

Select aperture 11 as current aperture

X15000000Y28750000D03*

Create a flash with the current aperture (11)

X20000000D03*

Create a flash with the current aperture

D19*

Select aperture 19 as current aperture

X28750000Y28750000D03*

Create a flash with the current aperture (19)

M02*

End of file

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

2.14 Conformance

A file violating any requirement of the specification or with constructs not defined in it is wholly

invalid. An invalid Gerber file is meaningless and does not represent an image.

A conforming Gerber file writer must write files according to this specification. A current

conforming Gerber file writer cannot use deprecated constructs. A writer is not required to

consider limitations or errors in particular readers but may assume that a valid file will be

processed correctly.

A conforming Gerber file reader must render a valid Gerber file according to this specification. A

current reader may support deprecated format elements as they can be present in legacy files.

To prepare for future extensions of the format, a Gerber file reader must give a warning when

encountering an unknown command; it must then continue processing after otherwise ignoring

the unknown construct. Otherwise there is no mandatory behavior on reading an invalid Gerber

file. It is not mandatory to report any other errors – this would impose an unreasonable burden

on readers and may result in useless messages in some applications. A reader is allowed to

attempt to reverse engineer the intended image and display it; note that if reverse engineering

fails this is the responsibility of the writer of the file, not the reader, as the invalid file is

meaningless – it is the file that is wrong, not the reader.

The responsibilities are obvious and plain. Writers must write valid and numerically robust files

and readers must process such files correctly. Writers are not responsible to navigate around

problems in the readers, nor are readers responsible to solve problems in the writers. Keep in

mind Postel’s rule: “Be conservative in what you send, be liberal in what you accept.”

Standard Gerber (RS-274-D) is revoked and therefore non-conforming. The responsibility for

misunderstandings of its non-standardized wheel file rests solely with the party that decided to

use Standard Gerber rather than Extended Gerber. See 8.5.

This document is the sole specification of the Gerber format. Gerber viewers, however useful,

do not overrule this document.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

3 Syntax

3.1 Character Set

A Gerber file is expressed in UTF-8 Unicode. The line separators CR and LF can be ignored

when processing the file, their sole purpose is human readability. The Gerber file is therefore

human-readable and transferrable between systems.

The characters '*' and '%' are delimiters and can only be used as prescribed in the syntax.

Space characters are only allowed inside strings (see 3.4.3).

Gerber files are case-sensitive. Command codes must be in upper case.

Actually, all characters in a Gerber file are taken form the readable ASCII characters, ASCII

codes 32 to 126 - regex [ -~] - and new line characters, except for attributes values with user-

defined metadata'. Metadata can require special characters and other languages than English,

and full UTF-8 is allowed.

3.2 Grammar Syntax

The formal grammar used in this specification is the parsing expression grammar (PEG), similar

in formalism to context-free grammars, with a slightly different interpretation. See

https://en.wikipedia.org/wiki/Parsing_expression_grammar for more information. The grammar of

is expressed in the variant of the Extended Backus-Naur Form used by the TatSu PEG parser

generator.

https://tatsu.readthedocs.io/en/stable/ for more information. Only a subset of the

rules in the very powerful TatSu grammar is needed – after all Gerber is a simple format. Below

is a description of that subset, taken from the TatSu documentation.

A grammar consists of a sequence of one or more rules of the form:

name = <expression> ;

The expressions are constructed from the following operators, in reverse order of precedence.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Grammar Syntax Rules

Rule

Name

Description

Comment

Comments have no effect on the grammar.

e1 | e2

Choice Match either e1 or e2

A | can be used before the first option as a layout aid:

rule =

| option1

| option2

| option3

;

(e)

Grouping

Match e, making it a node in the syntax tree

[e]

Option

Optionally match e

{e} or {e}*

Closure

Match e zero or more times.

{e}+

Positive

closure

Match e one or more times.

Positive

lookahead

Succeeds if e can be parsed. Does not consume input

Negative

lookahead

Fails if e can be parsed. Does not consume input

'text'

Token Match the token text.

Note that if text is alphanumeric it will only parse if the

character following the token is not alphanumeric. This is

done to prevent tokens like IN matching when the text

ahead is INITIALIZE. This feature can be turned setting

the grammar directive @@nameguard=False

/regexp/

Regex The pattern expression.

Match the regular expression regexp at the current text

position.

Python style regex is used, and it is interpreted as a

Python raw string.

End-of-text

Verify that the end of the input text has been reached.

Cut

Commit to the current option and prevent other options

from being considered even if what follows fails to parse.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Grammar Directives

Directive

Description

@@grammar :: <word

Specifies the name of the grammar.

@@nameguard :: <bool>

When set to True, avoids matching tokens

when the next character in the input

sequence is alphanumeric. Defaults to True.

See the ‘text’ expression for an explanation.

@@nameguard :: False

@@whitespace :: <regexp>

Provides a regular expression for the

whitespace to be ignored by the parser. It

defaults to /(?s)\s+/

@@whitespace :: /[\t ]+

3.3 Commands

Commands are the core syntactic element of the Gerber format. A Gerber file is a stream of

commands. Commands define the graphics state, create graphical objects, defines apertures,

manage attributes and so on.

Commands are built with words, the basic syntactic building block of a Gerber file. A word is a

non-empty character string, excluding the reserved characters '*' and '%', terminated with an '*'

free_character = /[^%*]/; # All characters but * and %

word = {free_character}+ '*';

For historic reasons, there are two command syntax styles: word commands and extended

commands.

command =

| extended_command

| word_command

;

word_command = word;

extended_command = '%' {word}+ '%';

Word commands are identified by a command code, the letter G, D or M followed by a positive

integer, e.g.

G02. Most word commands only consist of the command code, some also contain

coordinates.

Extended commands are identified by a two-character command code that is followed by

parameters specific to the code. An extended command is enclosed by a pair of ‘%’ delimiters.

An overview of all commands is in section 2.10, a full description in chapters 3.5 and 5.

The example below shows a stream of Gerber commands. Word commands are in yellow,

extended commands in green.

Example:

G04 Different command styles*

%FSLAX26Y26*%

%MOMM*%

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

%AMDonut*

1,1,$1,$2,$3*

$4=$1x0.75*

1,0,$4,$2,$3*

%ADD11Donut,0.30X0X0*%

%ADD10C,0.1*%

D10*

G75*

G02*

X0Y0D02*

X2000000Y0I0Y1000000D01*

G01*

D11*

D03*

M02*

One of the strengths of the Gerber format is its human readability. Use line breaks to enhance

readability; put one word or command per line; do not put a new line within a word, except after

a comma in long words.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

3.4 Data Types

All data types are tokens in the Gerber syntax, expressed a regex.

Integers

unsigned_integer = /[0-9]+/;

positive_integer = /[0-9]*[1-9][0-9]*/;

integer = /[+-]?[0-9]+/;

Integers must fit in a 32-bit signed integer. Examples:

-1024

+16

Decimals

unsigned_decimal = /((([0-9]+)(\.[0-9]*)?)|(\.[0-9]+))/;

decimal = /[+-]?((([0-9]+)(\.[0-9]*)?)|(\.[0-9]+))/;

Decimals must fit in an IEEE double. Examples:

-200

5000

1234.56

.123

-0.128

Note that a comma ',' is not valid as a decimal point.

Strings

Strings are used for communication between humans and can contain any non-Unicode

character. These are expressed as UTF-8 literal characters, or by a Unicode escape - reserved

characters must be escaped.

string = /[^%*]*/; # All characters except *%

Note that UTF-8 is identical to ASCII for any character that can be represented by ASCII.

The Unicode escape for the copyright symbol '©' is as follows:

• With lower case u for a 16-bit hex value: \u00A9

• With upper case U for a 32-bit hex value: \U000000A9

Zero-fill if needed to reach the required 4 or 8 hex digits

• The reserved characters '%' (\u0025 ) and '*' (\u002A) must always be escaped as they

are the delimiters of the Gerber syntax.

• '\' (\u005C) must be escaped as it is the escape character.

• ',' (\u002C) separates fields, and therefore must be escaped by a in any string that does

not end the word.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

If you want to keep the Gerber file printable ASCII-only use escape sequences for any character

in strings or fields. This may increase compatibility with legacy software but defeats human

readability of the meta-data.

Fields

The fields follow the string syntax in section 3.4.3 with the additional restriction that a field must

not contain commas. Fields are intended to represent comma-separated items in strings. If a

field must contain a comma it can be escaped with \u002C.

field = /[^%*,]*/; # All characters except *%,

Names

Names identify something, such as an attribute. They are for use only within the Gerber format

and are therefore limited to printable ASCII.

Names consist of upper- or lower-case ASCII letters, underscores (‘_’), dots (‘.’), a dollar sign

(‘$’) and digits. The first character cannot be a digit. Names are from 1 to 127 characters long.

Names beginning with a dot ‘.’ are reserved for standard names defined in the specification.

User defined names cannot begin with a dot.

Name = [._$a-zA-Z][._$a-zA-Z0-9]{0,126}

StandardName = \.[._$a-zA-Z][._$a-zA-Z0-9]{0,125}

UserDefinedName = [_$a-zA-Z][_.$a-zA-Z0-9]{0,126}

The scope of a name is from its definition till the end of the file. Names are case-sensitive:

Name ≠ name

Names for macro variables used in AM commands are more restrictive. They are of the form $n,

with n a positive integer, for example $3.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

3.5 Full Grammar of the Gerber Format

@@grammar :: Gerber_2021_02

@@nameguard :: False

@@whitespace :: /\n/

start = {statement}* M02 $;

statement =

| single_statement

| compound_statement

;

single_statement =

| operation

| interpolation_state_command

| Dnn

| G04

| attribute_command

| AD

| AM

| coordinate_command

| transformation_state_command

;

compound_statement =

| region_statement

| SR_statement

| AB_statement

;

coordinate_command =

|FS

|MO

;

operation =

|D01

|D02

|D03

;

interpolation_state_command =

|G01

|G02

|G03

|G75

;

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

transformation_state_command =

|LP

|LM

|LR

|LS

;

attribute_command =

|TO

|TD

|TA

|TF

;

# Graphics commands

#------------------

FS = '%' ('FS' 'LA' 'X' coordinate_digits 'Y' coordinate_digits) '*%';

coordinate_digits = /[1-6][56]/;

MO = '%' ('MO' ('MM'|'IN')) '*%';

D01 = (['X' integer] ['Y' integer] ['I' integer 'J' integer] 'D01') '*';

D02 = (['X' integer] ['Y' integer] 'D02') '*';

D03 = (['X' integer] ['Y' integer] 'D03') '*';

G01 = ('G01') '*';

G02 = ('G02') '*';

G03 = ('G03') '*';

G75 = ('G75') '*';

Dnn = (aperture_ident) '*';

G04 = ('G04' string) '*';

M02 = ('M02') '*';

LP = '%' ('LP' ('C'|'D')) '*%';

LM = '%' ('LM' ('N'|'XY'|'Y'|'X')) '*%';

LR = '%' ('LR' decimal) '*%';

LS = '%' ('LS' decimal) '*%';

AD = '%' ('AD' aperture_ident template_call) '*%';

#aperture_shape = name [',' decimal {'X' decimal}*];

template_call =

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

|'C' fst_par [nxt_par]

|'R' fst_par nxt_par [nxt_par]

|'O' fst_par nxt_par [nxt_par]

|'P' fst_par nxt_par [nxt_par [nxt_par]]

|!(('C'|'R'|'O'|'P')(','|'*')) name [fst_par {nxt_par}*]

;

fst_par = ',' (decimal);

nxt_par = 'X' (decimal);

AM = '%' ('AM' macro_name macro_body) '%';

macro_name = name '*';

macro_body = {in_macro_block}+;

in_macro_block =

|primitive

|variable_definition

;

variable_definition = (macro_variable '=' expression) '*';

macro_variable = '$' positive_integer;

primitive =

|('0' string) '*'

|('1' par par par par [par]) '*'

|('20' par par par par par par par) '*'

|('21' par par par par par par) '*'

|('4' par par par par {par par}+ par) '*'

|('5' par par par par par par) '*'

|('7' par par par par par par) '*'

;

par = ',' (expression);

# Compound statements

region_statement = G36 {contour}+ G37;

contour = D02 {D01|interpolation_state_command}*;

G36 = ('G36') '*';

G37 = ('G37') '*';

AB_statement = AB_open {in_block_statement}* AB_close;

AB_open = '%' ('AB' aperture_ident) '*%';

AB_close = '%' ('AB') '*%';

SR_statement = SR_open {in_block_statement}* SR_close;

SR_open = '%' ('SR' 'X' positive_integer 'Y' positive_integer 'I' decimal 'J'

decimal) '*%';

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

SR_close = '%' ('SR') '*%';

in_block_statement =

|single_statement

|region_statement

|AB_statement

;

# Attribute commands

#-------------------

TF = '%' ('TF' TF_atts) '*%';

TA = '%' ('TA' TA_atts) '*%';

TO = '%' ('TO' TO_atts) '*%';

TD = '%' ('TD' [all_atts]) '*%';

TF_atts =

|'.Part' nxt_field

|'.FileFunction' {nxt_field}*

|'.FilePolarity' nxt_field

|'.SameCoordinates' [nxt_field]

|'.CreationDate' nxt_field

|'.GenerationSoftware' nxt_field nxt_field [nxt_field]

|'.ProjectId' nxt_field nxt_field nxt_field

|'.MD5' nxt_field

|user_name

;

TA_atts =

|'.AperFunction' {nxt_field}*

|'.DrillTolerance' nxt_field nxt_field

|'.FlashText' {nxt_field}*

|user_name {nxt_field}*

;

TO_atts =

|'.N' nxt_field {nxt_field}*

|'.P' nxt_field nxt_field [nxt_field]

|'.C' nxt_field

|'.CRot' nxt_field

|'.CMfr' nxt_field

|'.CMPN' nxt_field

|'.CVal' nxt_field

|'.CMnt' nxt_field

|'.CFtp' nxt_field

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

|'.CPgN' nxt_field

|'.CPgD' nxt_field

|'.CHgt' nxt_field

|'.CLbN' nxt_field

|'.CLbD' nxt_field

|'.CSup' nxt_field nxt_field {nxt_field nxt_field}*

|user_name {nxt_field}*

;

all_atts =

|TF_atts

|TA_atts

|TO_atts

;

nxt_field = ',' field;

# Expressions

#------------

expression =

|{addsub_operator term}+

|expression addsub_operator term

|term

;

term =

|term muldiv_operator factor

|factor

;

factor =

| '(' ~ expression ')'

|macro_variable

|unsigned_decimal

;

# Tokens, by regex

#-----------------

addsub_operator = /[+-]/;

muldiv_operator = /[x\/]/;

unsigned_integer = /[0-9]+/;

positive_integer = /[0-9]*[1-9][0-9]*/;

integer = /[+-]?[0-9]+/;

unsigned_decimal = /((([0-9]+)(\.[0-9]*)?)|(\.[0-9]+))/;

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

decimal = /[+-]?((([0-9]+)(\.[0-9]*)?)|(\.[0-9]+))/;

aperture_ident = /D[0-9]{2,}/;

name = /[._a-zA-Z$][._a-zA-Z0-9]*/;

user_name = /[_a-zA-Z$][._a-zA-Z0-9]*/; # Cannot start with a dot

string = /[^%*]*/; # All characters except * %

field = /[^%*,]*/; # All characters except * % ,

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

3.6 File Extension, MIME Type and UTI

The Gerber Format has a standard file name extension, a registered mime type and a UTI

definition.

Standard file extension: .gbr or .GBR

Mime type: application/vnd.gerber

(see http://www.iana.org/assignments/media-types/application/vnd.gerber)

Mac OS X UTI:

<key>UTExportedTypeDeclarations</key>

<array>

<dict>

<key>UTTypeIdentifier</key>

<string>com.ucamco.gerber.image</string>

<key>UTTypeReferenceURL</key>

<string>http://www.ucamco.com/gerber</string>

<key>UTTypeDescription</key>

<string>Gerber image</string>

<key>UTTypeConformsTo</key>

<array>

<string>public.plain-text</string>

<string>public.image</string>

</array>

<key>UTTypeTagSpecification</key>

<dict>

<key>public.filename-extension</key>

<array>

</array>

<key>public.mime-type</key>

<string>application/vnd.gerber</string>

</dict>

</array>

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4 Graphics

4.1 Comment (G04)

The G04 command is used for human readable comments. It does not affect the image.

The syntax for G04 is as follows.

G04 = ('G04' string) '*';

The string must follow the string syntax in 3.4.3.

Example:

G04 This is a comment*

G04 The space characters as well as ‘,’ and ‘;’ are allowed here.*

Content starting with ” #@! “ is reserved for standard comments. They can only be used if

defined in the specification. Their future purpose is to allow to add information about the file

without affecting image generation. Gerber readers must ignore such comments when

generating the image.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.2 Coordinate Commands

Unit (MO)

The MO (Mode) command sets the file unit to either metric (mm) or imperial (in).

The MO command must be used once and only once, in the header of the file, before the first

operation command. The syntax is:

MO = '%' ('MO' ('MM'|'IN')) '*%';

Syntax

Comments

MO for Mode

MM|IN MM – metric (millimeter)

IN – imperial (inch)

Example:

Syntax

Comments

%MOMM*%

Specify the file is in metric units.

Parameters specifying distances or coordinates are expressed in the file unit.

Example:

G04 Defines a aperture 10 as a circle with diameter 0.25mm*

%MOMM*%

…

%ADD10C,0.25*%

Coordinates in operations have their own unit, see 4.2.2

It is recommended only to use metric. Imperial is there only for historic reasons and will be

deprecated at a future date.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Format Specification (FS)

The coordinates and distances in operations - the X,Y,I and J – are integers, not decimals. This

simplifies image processing. However, the file unit, mm or inch, is far too big when only integer

coordinates can be used. Coordinates have their own, much smaller, coordinate unit. The FS

(Format Specification) command sets the coordinate unit as a decimal fraction of file unit.

The FS command must be used once and only once, in the header, before the first operation

command. The syntax is:

FS = '%' ('FS' 'LA' 'X' coord_digits 'Y' coord_digits) '*%';

coord_digits = /[1-6][56]/;

Syntax

Comments

FS for Format Specification

LA These fixed characters are necessary for backwards

compatibility. (They pertain to deprecated format options,

see 8.2.1.)

X coord_digits

Y coord_digits

Specifies the number of integer and decimal file unit digits in

the X and Y coordinate data. The format of X and Y

coordinate must be the same; it is specified in both X and Y

for backwards compatibility.

coord_digits The first digit sets the maximum number of integer digits in

the coordinate data. The number of integer digits can be 1

up to 6; use a number that is sufficient for the size of the

image; 3 integer digits is typical.

The second digit sets the number of decimal digits. For

example, if the MO command sets the file to metric, the

base unit is mm, and the FS commands sets 6 decimal

digits 6, then the coordinate unit is 10

-6

mm, or nm. The

number of decimal digits must be 5 or 6, with 6

recommended.

Example:

%MOMM*%

%FSLAX36Y36*%

The file is metric. The file unit is mm, the coordinate unit is 10

-6

mm in nm.

Coordinate Units

%MOMM*% %MOIN*%

%FSLAXn3Yn3*%

μm (10

-3

mm)

mil (10

-3

inch) = 25.4 μm

%FSLAXn4Yn4*%

100 nm (10

-4

mm)

0.1 mil (10

-4

inch) = 2.54 μm

%FSLAXn5Yn5*%

10 nm (10

-5

mm)

0.01 mil (10

-5

inch) = 254.0 nm

%FSLAXn5Yn6*%

nm (10

-6

mm)

0.001 mil (10

-6

inch) = 25.4 nm

Red is deprecated, green is current,

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Always use metric, with 6 decimals.

It is sometimes argued that 6 decimals is overkill as the PCB design grid is much coarser. This

is not a valid argument. Many points in a Gerber file are calculated; intersections, certainly with

circles, have rational or even irrational coordinates, resulting in rounding errors. Even small

perturbations can turn an otherwise perfect arc into an invalid one or turn an impeccable contour

in an invalid self-intersecting one. Most errors such as missing clearances have low resolution

as root cause and are solved when metric 6 mm is set. There only downside to high resolution

is that the file becomes about 5% bigger, which is not a reason to throw away precision and risk

scrap. There is no reason to use antiquated imperial units. An underlying component or design

grid may be imperial, but a nm unit expresses any imperial value of 1/100 mil or larger without

rounding error – amply sufficient for PCBs. By using inch, which is 25.4 times larger than mm,

one gives up precision for no gain.

4.3 Aperture Definition (AD)

AD Command

The AD command creates an aperture, attaches the aperture attributes at that moment in the

attribute dictionary to it and adds it to the apertures dictionary.

The syntax for the AD command is as follows:

AD = '%' ('AD' aperture_ident template_call) '*%';

template_call = template_name [',' parameter {'X' parameter}*];

Syntax

Comments

‘AD’ is the command code

aperture_ident

The aperture identification being defined (≥10).

The

aperture numbers can range from 10 up to

2.147.483.647 (max int 32). The D00 to D09 are

reserved and cannot be used for apertures. Once an

aperture number is assigned it cannot be re-assigned

– thus apertures are uniquely identified by their

number.

template_call Set the shape of the aperture by calling a template

with actual parameters

template_name The name of the template, either a standard aperture

or macro (see 2.2

). It follows the syntax of names

(see 3.4.5).

[',' parameter {'X' parameters}*]; The number and meaning of the actual parameters

depend on the template. Parameters are decimals.

All sizes are in the unit of the MO command.

The AD command must precede the first use of the aperture. It is recommended to put all AD

commands in the file header.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Example:

%ADD10C,.025*%

%ADD10C,0.5X0.25*%

Section 5.8 has examples to illustrate how to attach aperture attributes to an aperture.

Zero-size Apertures

Generally, apertures with size zero are not valid, and so are objects created with them.

There is one exception. The C (circular) standard aperture with zero diameter is allowed, and so

are objects created with it. Attributes can be attached to them. For the avoidance of doubt, it is

only the C aperture where zero-size is valid, not another aperture type whose shape is

fortuitously circular.

Zero-size objects do not affect the image. They can be used to provide meta-information to

locations in the image plane.

Allowed does not mean recommended, quite in the contrary. If you are tempted to use a zero-

size object, consider whether it is useful, and whether there is no proper way to convey the

meta-information. Do not abuse a zero-size object to indicate the absence of an object, e.g. by

flashing a zero-size aperture to indicate the absence of a flash. This is just confusing. If there is

nothing, put nothing.

Examples

Syntax

Comments

%ADD10C,.025*%

Create aperture with number 10: a solid circle with

diameter 0.025

%ADD22R,.050X.050X.027*%

Creates aperture 22: a rectangle with sides of 0.05

– therefore forming a square - and with a 0.027

diameter round hole

%ADD57O,.030X.040X.015*%

Creates aperture 57: an obround with sizes 0.03 x

0.04 with 0.015 diameter round hole

%ADD30P,.016X6*%

Creates aperture 30: a solid polygon with 0.016

outer diameter and 6 vertices

%ADD15CIRC*%

Creates aperture 15: instantiate the macro aperture

template CIRC defined previously witg an aperture

macro (AM) command

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.4 Standard Aperture Templates

Overview

Standard Aperture Templates

Name

Shape

Parameters

Ref.

Circle

Diameter[, Hole diameter]

4.4.2

Rectangle

X size, Y size[, Hole diameter]

4.4.3

Obround

X size, Y size[, Hole diameter]

4.4.4

Polygon

Outer diameter, # vertices[, Rotation[, Hole diameter]]

4.4.5

Table with standard aperture templates

Circle

The syntax of the circle standard template call is:

template_call = 'C' ',' diameter 'X' hole_diameter

Syntax

Comments

Indicates the circle aperture template.

diameter

Diameter. A decimal ≥0.

hole_diameter

Diameter of a round hole.

A decimal

If omitted the aperture

is solid. See also section 4.4.6.

Examples:

%ADD10C,0.5*%

%ADD10C,0.5X0.25*%

These commands define the following apertures:

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

5. Circles

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Rectangle

The syntax of the rectangle or square standard template call is:

template_call = 'R' ',' x_size 'X' y_size 'X' hole_diameter

Syntax

Comments

Indicates the rectangle aperture template.

x_size

y_size

X and Y sizes of the rectangle. Decimals >0.

If x_size = y_size the effective shape is a square.

hole_diameter

Diameter of a round hole.

A decimal

If omitted the aperture is

solid.

See also section 4.4.6.

Examples:

%ADD17P,.040X6*%

%ADD17P,.040X6X0.0X0.019*%

These commands define the following apertures:

8. Polygons

Outer diameter

Out er diameter

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Transparency of Holes

Standard apertures may have a round hole in them. When an aperture is flashed only the solid

part affects the image, the hole does not. Objects under a hole remain visible through the hole.

For image generation the area of the hole behaves exactly as the area outside the aperture. The

hole is not part of the aperture.

Warning: Make no mistake: holes do not clear the objects under them.

For all standard apertures the round hole is defined by specifying its diameter as the last

parameter: <Hole diameter>. If <Hole diameter> is omitted the aperture is solid. If present the

diameter must be ≥ 0. The hole must strictly fit within the standard aperture. It is centered on the

aperture.

Example:

%FSLAX26Y26*%

%MOMM*%

%ADD10C,10X5*%

%ADD11C,1*%

G01*

%LPD*%

D11*

X-25000000Y-1000000D02*

X25000000Y1000000D01*

D10*

X0Y0D03*

M02*

9. Standard (circle) aperture with a hole above a draw

Note that the draw is visible through the hole.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.5 Aperture Macro (AM)

The AM command creates a macro aperture template and adds it to the aperture template

dictionary (see 2.2). A template is a parametrized shape. The AD command instantiates a

template into an aperture by suppling values to the template parameters.

Templates of any shape or parametrization can be created. Multiple simple shapes called

primitives can be combined in a single template. An aperture macro can contain variables

whose actual values are defined by:

 Values provided by the AD command

 Arithmetic expressions with other variables

The template is created by positioning primitives in a coordinate space. The origin of that

coordinate space will be the origin of all apertures created with the state.

A template must be defined before the first AD that refers to it. The AM command can be used

multiple times in a file.

Attributes are not attached to templates. They are attached to the aperture at the time of its

creation with the AD command.

An AM command contains the following words:

 The AM declaration with the macro name

 Primitives with their comma-separated parameters

 Macro variables, defined by an arithmetic expression

The syntax for the AM command is:

AM = '%' ('AM' macro_name macro_body) '%';

macro_name = name '*';

macro_body = {in_macro_block}+;

in_macro_block =

|primitive

|variable_definition

;

variable_definition = (macro_variable '=' expression) '*';

macro_variable = '$' positive_integer;

primitive = primitive_code {',' par}*

par = ',' (expression);

Syntax

Comments

AM for Aperture Macro

<Macro name> Name of the aperture macro. The name must be unique, it

cannot be reused for another macro. See 3.4.5

for the syntax

rules.

<Macro body> The macro body contains the primitives generating the image

and the calculation of their parameters.

<Variable definition> $n=<Arithmetic expression>. An arithmetic expression may

use arithmetic operators (described later), constants and

variables $m defined previously.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Syntax

Comments

<Primitive> A primitive is a basic shape to create the macro. It includes

primitive code identifying the primitive and primitive-specific

parameters (e.g. center of a circle). See 4.5.1

. The primitives

are positioned in a coordinates system whose origin is the

origin of the resulting apertures.

A code specifying the primitive (e.g. polygon).

<Parameter> Parameter can be a decimal number (e.g. 0.050), a variable

(e.g. $1) or an arithmetic expression based on numbers and

variables. The actual value is calculated as explained in

4.5.4.3.

Coordinates and sizes are expressed in the unit set by the MO command.

A parameter can be either:

 A decimal number

 A macro variable

 An arithmetic expression

A macro variable name must be a ‘$’ character followed by an integer >0, for example $12.

(This is a subset of names allowed in 3.4.3.)

Note: New lines can be added between words of a single command to enhance

readability. They do not affect the macro definition.

Example:

The following AM command defines an aperture macro named ‘Triangle_30’.

%AMTriangle_30*

4,1,3,

1,-1,

1,1,

2,1,

1,-1,

30*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Primitives

4.5.1.1 Overview

Macro Primitives

Code

Name

Parameters

Ref.

Comment

A comment string

4.5.1.2

Circle

Exposure, Diameter, Center X, Center Y, Rotation

4.5.1.3

Vector Line

Exposure, Width, Start X, Start Y, End X, End Y, Rotation

4.5.1.4

Center Line

Exposure, Width, Hight, Center X, Center Y, Rotation

4.5.1.5

Outline

Exposure, # vertices, Start X, Start Y, Subsequent points..., Rotation

4.5.1.6

Polygon

Exposure, # vertices, Center X, Center Y, Diameter, Rotation

4.5.1.7

7 Thermal Center X, Center Y, Outer diameter, Inner diameter, Gap, Rotation

4.5.1.8

Table with macro primitives

Except for the comment all the parameters can be a decimal, integer, macro variables or am

arithmetic expression.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.5.1.2 Comment, Code 0

The comment primitive has no effect on the image but adds human-readable comments in an

AM command. The comment primitive starts with the ‘0’ code followed by a space and then a

single-line text string. The text string follows the syntax for strings in section 3.4.3.

Example:

%AMBox*

0 Rectangle with rounded corners, with rotation*

0 The origin of the aperture is its center*

0 $1 X-size*

0 $2 Y-size*

0 $3 Rounding radius*

0 $4 Rotation angle, in degrees counterclockwise*

0 Add two overlapping rectangle primitives as box body*

21,1,$1,$2-$3-$3,0,0,$4*

21,1,$2-$3-$3,$2,0,0,$4*

0 Add four circle primitives for the rounded corners*

$5=$1/2*

$6=$2/2*

$7=2X$3*

1,1,$7,$5-$3,$6-$3,$4*

1,1,$7,-$5+$3,$6-$3,$4*

1,1,$7,-$5+$3,-$6+$3,$4*

1,1,$7,$5-$3,-$6+$3,$4*%

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.5.1.3 Circle, Code 1

A circle primitive is defined by its center point and diameter.

Parameter

number

Description

Exposure off/on (0/1)

Diameter ≥ 0

Center X coordinate.

Center Y coordinate.

5 Rotation angle of the center, in degrees counterclockwise. The primitive

is rotated around the origin of the macro definition, i.e. the (0, 0) point of

macro coordinates.

The rotation parameter is optional. The default is no rotation.

10. Circle primitive

Below there is the example of the AM command that uses the circle primitive.

Example:

%AMCircle*

1,1,1.5,0,0,0*%

3, 4

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.5.1.4 Vector Line, Code 20.

A vector line is a rectangle defined by its line width, start and end points. The line ends are

rectangular.

Parameter

number

Description

Exposure off/on. (0/1)

Width of the line

≥ 0.

Start point X coordinate.

Start point Y coordinate.

End point X coordinate.

End point Y coordinate.

7 Rotation angle, in degrees counterclockwise. The primitive is rotated

around the origin of the macro definition, i.e. the (0, 0) point of macro

coordinates

11. Vector line primitive

Below there is the example of the AM command that uses the vector line primitive.

Example:

%AMLine*

20,1,0.9,0,0.45,12,0.45,0*

3, 4

5, 6

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.5.1.5 Center Line, Code 21

A center line primitive is a rectangle defined by its width, height, and center point.

Parameter

number

Description

Exposure off/on. (0/1)

Width

≥ 0.

Height

≥ 0.

Center point X coordinate.

Center point Y coordinate.

6 Rotation angle, in degrees counterclockwise. The primitive is rotated

around the origin of the macro definition, i.e. (0, 0) point of macro

coordinates.

Warning: The rotation is not around the center point. (Unless the

center point happens to be the macro origin.)

12. Center line primitive

Below there is the example of the AM command that uses the center line primitive.

Example:

%AMRECTANGLE*

21,1,6.8,1.2,3.4,0.6,30*%

4, 5

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.5.1.6 Outline, Code 4

An outline primitive is an area defined by its outline or contour. The outline is a polygon,

consisting of linear segments only, defined by its start vertex and n subsequent vertices. The

outline must be closed, i.e. the last vertex must be equal to the start vertex. The outline must

comply with all the requirements of a contour according to 4.10.3.

Parameter

number

Description

Exposure off/on (0/1)

2 The number of vertices of the outline = the number of coordinate

pairs minus one. An integer ≥3.

3, 4

Start point X and Y coordinates.

5, 6

First subsequent X and Y coordinates.

... Further subsequent X and Y coordinates.

The X and Y coordinates are not modal: both X and Y must be

specified for all points.

3+2n, 4+2n Last subsequent X and Y coordinates. As the outline must be closed

the last coordinates must be equal to the start coordinates.

5+2n Rotation angle, in degrees counterclockwise, a decimal. The primitive is

rotated around the origin of the macro definition, i.e. the (0, 0) point of

macro coordinates.

13. Outline primitive

The maximum number of vertices is 5000. The purpose of this primitive is to create apertures to

flash pads with special shapes. The purpose is not to create copper pours. Use the region

statement for copper pours; see 4.10.

3, 4

5, 6

7, 8

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Example:

The following AM command defines an aperture macro named ‘Triangle_30’. The macro is a

triangle rotated 30 degrees around the origin of the macro definition:

%AMTriangle_30*

4,1,3,

1,-1,

1,1,

2,1,

1,-1,

30*

Syntax

Comments

AM Triangle _30

Aperture macro name is ‘Triangle _30’

4,1,3 4 – Outline

1 – Exposure on

3 – The outline has three subsequent points

1,-1 1 – X coordinate of the start point

-1 – Y coordinate of the start point

1,1,

2,1,

1,-1,

Coordinates (X, Y) of the subsequent points: (1,1), (2,1), (1,-1).

Note that the last point is the same as the start point

Rotation angle is 30 degrees counterclockwise

14. Rotated triangle

(0, 0)

Rotation center

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.5.1.7 Polygon, Code 5

A polygon primitive is a regular polygon defined by the number of vertices n, the center point

and the diameter of the circumscribed circle.

Parameter

number

Description

Exposure off/on (0/1)

2 Number of vertices n, 3 ≤ n ≤ 12. An integer. The first vertex is on the

positive X-axis through the center point when the rotation angle is

zero.

Center point X coordinate. A

Center point Y coordinate.

Diameter of the circumscribed circle

≥ 0.

6 Rotation angle, in degrees counterclockwise.

With rotation angle zero

there is a vertex on the positive X-axis through the aperture center.

The primitive is rotated around the origin of the macro definition, i.e. the

(0, 0) point of macro coordinates.

15. Polygon primitive

Example:

%AMPolygon*

5,1,8,0,0,8,0*%

3, 4

First

vertex

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.5.1.8 Thermal, Code 7

The thermal primitive is a ring (annulus) interrupted by four gaps. Exposure is always on.

Parameter

number

Description

Center point X coordinate.

Center point Y coordinate.

Outer diameter > inner diameter

Inner diameter ≥ 0

Gap thickness < (outer diameter)/√2. Note that if the (gap

thickness)*√2 ≥ (inner diameter) the inner circle disappears. This is

not invalid.

The gaps are on the X and Y axes through the center without

rotation. They rotate with the primitive.

Rotation angle, in degrees counterclockwise. A decimal.

The primitive is

rotated around the origin of the macro definition, i.e. (0, 0) point of

macro coordinates.

16. Thermal primitive

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Exposure Parameter

The exposure parameter that can take two values:

 0 means exposure is ‘off’

 1 means exposure is ‘on’

Primitives with exposure ‘on’ create the solid part of the macro aperture. Primitives with

exposure ‘off’ erase the solid part created earlier in the same macro. Exposure off is used to

create a hole in the aperture – see also 4.4.6.

The erasing action of exposure off only acts on other primitives within the same macro

definition. When a macro is flashed the hole does not clear objects in the final image – the hole

is transparent. Another way of expressing it is that the macro definition is flattened before it is

used, and the result is a positive image.

Warning: When the macro aperture is flashed, the erased area does not clear the

underlying graphical objects. Objects under removed parts remain visible.

Example:

%FSLAX26Y26*%

%MOMM*%

%AMSquareWithHole*

21,1,10,10,0,0,0*

1,0,5,0,0*%

%ADD10SquareWithHole*%

%ADD11C,1*%

G01*

%LPD*%

D11*

X-25000000Y-2000000D02*

X25000000Y1000000D01*

D10*

X0Y0D03*

M02*

17. Macro aperture with a hole above a draw

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Note that the draw is still visible through the hole.

Rotation Parameter

All primitives can be rotated around the origin of the macro definition, i.e. its point (0, 0). (Make

no mistake: rotation is not around the geometric center of the primitive, unless of course it

coincides with the origin.)

A rotation angle is expressed by a decimal number, in degrees counterclockwise. A positive

angle means counterclockwise rotation, a negative angle clockwise. The rotation angle is

defined by the rotation parameter, the last in the list of the primitive parameters.

To rotate a macro composed of several primitives it is sufficient to rotate all primitives by the

same angle. See illustration below.

18. Rotation of an aperture macro composed of several primitives

Warning: Rotation is around the origin of the macro definition, not around the geometric

center of the primitive – unless the two coincide of course. The reason is obvious: if rotation

were about the center of each primitive a composite aperture like the one above would fall apart

under rotation.

(0, 0)

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Macro Variables and Expressions

4.5.4.1 Variable Values from the AD Command

An AM command can use variables whose actual values are provided by the AD command

calling the macro. Such variables are identified by ‘$n’ where n indicates the index in the list of

the variable values provided by the AD command. Thus $1 means the first value in the list, $2

the second, and so on.

Example:

%AMDONUTVAR*1,1,$1,$2,$3*1,0,$4,$2,$3*%

$1, $2, $3 and $4 are macro variables. With the following calling AD

%ADD34DONUTVAR,0.100X0X0X0.080*%

the variables take the following values:

$1 = 0.100

$2 = 0

$3 = 0

$4 = 0.080

4.5.4.2 Arithmetic Expressions

A parameter value can also be defined by an arithmetic expression consisting of integer and

decimal constants, other variables, arithmetic operators and the brackets ‘(‘ and ‘)’. The

standard arithmetic precedence rules apply. The following arithmetic operators are available:

Operator

Function

Unary plus (expressions without the unary

sign are positive)

Unary minus

Add

Subtract

x (lower case)

Multiply

Divide. The result is a decimal; it is not

rounded or truncated to an integer.

Arithmetic operators

Example:

%AMRect*

21,1,$1,$2-2*$3,-$4,-$5+$2,0*%

The corresponding AD command could be:

%ADD146Rect,0.0807087X0.1023622X0.0118110X0.5000000X0.3000000*%

4.5.4.3 Definition of a New Variable

New variables can be defined by an assign statement as follows: $4=$1x1.25-$3. The

right-hand side is any arithmetic expression as in the previous section.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Example:

%AMDONUTCAL*

1,1,$1,$2,$3*

$4=$1x1.25*

1,0,$4,$2,$3*%

The variable values are determined as follows:

 $1, $2, ..., $n take the values of the n parameters of the calling AD command.

 New variables get their value by evaluating their defining expression.

 Undefined variables are 0.

Macro variables cannot be redefined.

Example:

%AMDONUTCAL*

1,1,$1,$2,$3*

$5=$1x0.75*

1,0,$5,$2,$3*%

%ADD35DONUTCAL,0.020X0X0X0.03*%

The AD command contains 4 parameters. The first four macro variables take the values: $1 =

0.02, $2 = 0, $3 = 0, $4 = 0.03. $5 is defined later and becomes $5 = 0.02 x

0.75 = 0.015.

Below are some more examples to illustrate the syntax to define macro variables. ues.

Examples:

%AMTEST1*

1,1,$1,$2,$3*

$4=$1x0.75*

$5=($2+100)x1.75*

1,0,$4,$5,$3*%

%AMTEST2*

$4=$1x0.75*

$5=100+$3*

1,1,$1,$2,$3*

1,0,$4,$2,$5*

$6=$4x0.5*

1,0,$6,$2,$5*%

Examples

4.5.5.1 Fixed Parameter Values

The following AM command defines an aperture macro named ‘DONUTFIX’ consisting of two

concentric circles with fixed diameter sizes:

%AMDONUTFIX*

1,1,0.100,0,0*

1,0,0.080,0,0*%

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Syntax

Comments

AMDONUTFIX

Aperture macro name is ‘DONUTFIX’

1,1,0.100,0,0 1 – Circle

1 – Exposure on

0.100 – Diameter

0 – X coordinate of the center

0 – Y coordinate of the center

1,0,0.080,0,0 1 – Circle

0 – Exposure off

0.080 – Diameter

0 – X coordinate of the center

0 – Y coordinate of the center

An example of an AD command using this aperture macro:

%ADD33DONUTFIX*%

4.5.5.2 Variable Parameter Values

The following AM command defines an aperture macro named ‘DONUTVAR’ consisting of two

concentric circles with variable diameter sizes:

%AMDONUTVAR*

1,1,$1,$2,$3*

1,0,$4,$2,$3*%

Syntax

Comments

AMDONUTVAR

Aperture macro name is ‘DONUTVAR’

1,1,$1,$2,$3 1 – Circle

1 – Exposure on

$1 – Diameter is provided by AD command

$2 – X coordinate of the center is provided by AD command

$3 – Y coordinate of the center is provided by AD command

1,0,$4,$2,$3 1 – Circle

0 – Exposure off

$4 – Diameter is provided by AD command

$2 – X coordinate of the center is provided by AD command (same

as in first circle)

$3 – Y coordinate of the center is provided by AD command (same

as in first circle)

The AD command using this aperture macro can look like the following:

%ADD34DONUTVAR,0.100X0X0X0.080*%

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

In this case the variable parameters get the following values: $1 = 0.100, $2 = 0, $3 = 0, $4 =

0.080.

4.5.5.3 Definition of a New Variable

The following AM command defines an aperture macro named ‘DONUTCAL’ consisting of two

concentric circles with the diameter of the second circle defined as a function of the diameter of

the first:

%AMDONUTCAL*

1,1,$1,$2,$3*

$4=$1x0.75*

1,0,$4,$2,$3*%

Syntax

Comments

AMDONUTCAL

Aperture macro name is ‘DONUTCAL’

1,1,$1,$2,$3 1 – Circle

1 – Exposure on

$1 – Diameter is provided by AD command

$2 – X coordinate of the center is provided by AD command

$3 – Y coordinate of the center is provided by AD command

$4=$1x0.75 Defines variable $4 to be used as the diameter of the inner circle;

the diameter of this circle is 0.75 times the diameter of the outer

circle

1,0,$4,$2,$3 1 – Circle

0 – Exposure off

$4 – Diameter is calculated with the previous definition of this

variable

$2 – X coordinate of the center is provided by AD command (same

as in first circle)

$3 – Y coordinate of the center is provided by AD command (same

as in first circle)

The AD command using this aperture macro can look like the following:

%ADD35DONUTCAL,0.020X0X0*%

This defines a donut with outer circle diameter equal to 0.02 and inner circle diameter equal to

0.015.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.5.5.4 A useful macro

The following example creates a rectangle with rounded corners, useful as SMD pad.

It uses the following construction:

19. Construction of the Box macro

%AMBox*

0 Rectangle with rounded corners, with rotation*

0 The origin of the aperture is its center*

0 $1 X-size*

0 $2 Y-size*

0 $3 Rounding radius*

0 $4 Rotation angle, in degrees counterclockwise*

0 Add two overlapping rectangle primitives as box body*

21,1,$1,$2-$3-$3,0,0,$4*

21,1,$2-$3-$3,$2,0,0,$4*

0 Add four circle primitives for the rounded corners*

$5=$1/2*

$6=$2/2*

$7=2x$3*

1,1,$7,$5-$3,$6-$3,$4*

1,1,$7,-$5+$3,$6-$3,$4*

1,1,$7,-$5+$3,-$6+$3,$4*

1,1,$7,$5-$3,-$6+$3,$4*%

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.6 Set Current Aperture (Dnn)

The command Dnn (nn

≥10)

sets the current aperture graphics state parameter. The syntax is:

Dnn = 'D unsigned_integer '*';

Syntax

Comments

Command code

<aperture number> The aperture number (integer ≥10). An aperture with

that number must be in the apertures dictionary.

D-commands 0 to 9 are reserved and cannot be used for apertures. The D01 and D03

commands use the current aperture to create track and flash graphical objects.

Example:

D10*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.7 Interpolation State Commands (G01,G02,G03,G75)

Linear Interpolation (G01)

G01 sets linear interpolation mode. In linear interpolation mode a D01 operation generates a

linear segment, from the current point to the (X, Y) coordinates in the command. The current

point is then set to the (X, Y) coordinates.

The segment is stroked with the current aperture to create a draw graphical object, except in a

region statement where the segment is added to the contour under construction.

The G01 command sets linear operation. The syntax is as follows:

G01 = ('G01') '*';

Syntax

Comments

G01 Sets interpolation mode graphics state parameter to ‘linear

interpolation’

D01 = (['X' x_coordinate] ['Y' y_coordinate] 'D01') '*';

Syntax

Comments

x_coordinate An integer specifying the X coordinate of the end point of the straight

segment. The default is the X coordinate of the current point.

y_coordinate

As above, but for the Y axis.

D01

Interpolate operation code

The coordinates are interpreted as specified by the FS and MO command.

Example:

G01*

X250000Y155000D01*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Circular Interpolation (G02, G03, G75)

G02 sets clockwise circular interpolation mode, G03 counterclockwise. In circular interpolation

mode a D01 operation generates an arc segment, from the current point to the (X, Y)

coordinates in the command. The current point is then set to the (X, Y) coordinates.

The segment is stroked with the current aperture to create an arc graphical object, except in a

region statement where the segment is added to the contour under construction.

For compatibility with older versions of the Gerber format, a G75* must be issued before the first

D01 in circular mode.

The syntax of these commands is:

G02 = ('G02') '*';

G03 = ('G03') '*';

G75 = ('G75') '*';

Syntax

Comments

G02 Sets interpolation mode graphics state parameter to

‘clockwise circular interpolation’

G03 Sets interpolation mode graphics state parameter to

‘counterclockwise circular interpolation’

G75 This command must be issued before the first circular interpolation

operation, for compatibility with older Gerber versions

Examples:

G02*

G75*

The syntax of the D01 command in circular interpolation mode is:

D01 = (['X' x_coordinate] ['Y' y_coordinate] 'D01' 'I' x_offset 'J' y-offset ) '*';

Syntax

Comments

x_coordinate

As above, but for the Y axis.

i_offset Add the I offset to the X coordinate of the start point of the arc to

calculate the X of the center of the arcs. <Offset> is an integer.

j_offset

As above, but for the Y axis.

D01

Interpolate operation code

The coordinates and offsets are interpreted according as specified by the FS and MO

command.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

20. Circular interpolation example

Example:

G75*

G03*

X75000Y50000I40000J0D01*

When start point and end point coincide the result is a full 360° arc. An example:

Syntax

Comments

D10*

G01*

X0Y600D02*

G75*

G02*

X0Y600I500J0D01*

Select aperture 10 as current aperture

Set linear interpolation mode

Set the current point to (0, 6)

Must be called before an arc is created.

Set clockwise circular interpolation mode

Create arc object to (0, 6) with center (5,6)

The resulting image is a full circle.

Note that arcs where the start point and end point of an arc very close together are unstable: a

small change in their relative position can turn a large arc in a small one and vice versa,

dramatically changing the image. A typical case is very small arcs: start and end point are close

together; if due to rounding the end point is slightly moved to coincide with the start point the

small arc becomes a full arc.

Rounding must be done carefully. Using high resolution is an obvious prerequisite. See 4.14.

The Gerber writer must also consider that the reader unavoidably has rounding errors. Perfectly

exact numerical calculation cannot be assumed. It is the responsibility of the writer to avoid

unstable arcs. Arcs shorter than say 2μm must be replaced with a draw - draws are intrinsically

Y axis

0,0

X axis

End point

Start point

(current

point)

Arc center

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

stable and the error is negligible. Near full arcs must be cut in two big arcs, which too are

intrinsically stable.

Warning: A Gerber file that attempts to create an arc without a preceding G75 is invalid.

4.7.2.1 Example

Syntax

Comments

X3000000Y-2000000D02*

G75*

G03*

X-3000000Y-2000000I-

3000000J4000000D01*

Set the current point to (3, -2) mm

Must be called before an arc is created

Set counterclockwise interpolation mode

Create arc object counterclockwise to (-3,-2). The

offsets from the start point to the center point are

3 for X and 4 for Y, i.e. the center point is (0, 2)

21. Arc example

4.7.2.2 Valid Arcs

Mathematically, the distance from the center to the start point must be exactly equal to the

distance to the end point. However, a Gerber file has a finite resolution. It is therefore generally

not possible to position the center point exactly so that both distances – radii - are indeed

exactly equal. Furthermore, the software generating the Gerber file unavoidably adds rounding

errors of its own. In real files the center is unavoidably not positioned exactly, and the two radii

are not equal. We will call the difference between the start and end radius the arc deviation.

End point (-3, -2)

Start point (3, -2)

(0, 0)

Arc center (0, 2)

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

A mathematically exact circle has of course zero deviation. The interpretation of the arc

command is then obvious. However, which curve is represented by a “circular arc” with a non-

zero deviation? It cannot be a circular arc with the given center. Either it is not circular, it has

another center, or it does not go from start to end. The curve is defined as follow.

Any continuous and monotonic curve starting at the start point and ending at the end point,

approximating the ring with the given center point and with inner and outer radii equal to the

start radius and end radius is a valid rendering of the arc command. See figure below.

22. Arc with a non-zero deviation

The arc therefore has a fuzziness of the order of magnitude of the arc deviation. The writer of

the Gerber file accepts any interpretation within the fuzziness above as valid. If the writer

requires a more precise interpretation of the arc he needs to write more precise arcs, with lower

deviation.

It is however not allowed to place the center point close to the straight line through begin and

end point except when it is strictly in between these points. When the center is on or outside the

segment between start and end point the construct is nonsensical. See figure below.

23. Nonsensical center point

Note that self-intersecting contours are not allowed, see 4.10.3. If any of the valid arc

interpretations turns the contour in a self-intersecting one, the file is invalid, with unpredictable

results.

The root cause of most problems with arcs is the use a low resolution. One sometimes attempts

to force arcs of size of the order of e.g. 1/10 of a mil in a file with resolution of 1/10. This is

asking for problems. Use higher resolution. See 4.14.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.8 Operations (D01/D02/D03)

Overview

Commands consisting of coordinate data followed by a D01, D02 or D03 function code are

called operations.

 Operation with D01 code is called interpolate operation. It creates a straight-line segment or

a circular segment by interpolating from the current point to the operation coordinates. The

segment is then stroked with the current aperture to generate a draw or arc graphical

object, except in a region statement where the segment is added to the contour being

constructed. The current point is moved to operations coordinate before processing the

next command.

 Operation with D02 code is called move operation. It moves the current point to the

operation coordinates. No graphical object is generated.

 Operation with D03 code is called flash operation. It creates a flash object by replicating

(flashing) the current aperture at the operation coordinates. When the aperture is flashed

its origin is positioned at the coordinates of the operation. The origin of a standard aperture

is its geometric center. The origin of a macro aperture is the origin used in the defining AM

command. The current point is moved to operations coordinate before processing the next

command.

The operations are controlled by the graphics state (see 2.5), as summarized in the table below.

G01 sets linear, G02 clockwise and G03 counterclockwise circular interpolation.

Operation

code

Inside a region statement (G36/G37) Outside a region statement

Linear mode

(G01)

Circular mode

(G02, G03)

Linear mode

(G01)

Circular mode

(G02, G03)

D01

Adds linear segment

to the contour under

construction

Moves current point

Adds circular

segment to the

contour under

construction

Moves current point

Creates a draw

Moves current point

Creates an arc

Moves current point

D02

Starts a new contour

Moves current point

D03 Not allowed

Creates a flash

Moves current point

Effect of operation codes depending on graphics state

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

The parameters of the operations are coordinate data, see Error! Reference source not

found.. The FS and MO commands specify how to interpret the coordinate data.

Examples:

X200Y200D02* move to (+200, +200)

Y-300D03*

flash at (+200, -300)

I300J100D01*

interpolate to (+200, -300) with center offset (+300, +100)

Y200I50J50D01*

interpolate to (+200, +200) with center offset (+50, +50)

X200Y200I50J50D01*

interpolate to (+200, +200) with center offset (+50, +50)

X+100I-50D01*

interpolate to (+100, +200) with center offset (-50, 0)

D03* flash at (+100,+200)

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Interpolate (D01)

Performs an interpolation operation, creating a draw or an arc segment. The interpolation state

defines which type of segment is created, see 4.7. The syntax depends on the required

parameters, and, hence, on the interpolation state.

Interpolation

state

Syntax

Linear (G01)

D01 = (['X' x_coordinate] ['Y' y_coordinate] 'D01') '*';

Circular (G02|G03)

D01 = (['X' x_coordinate] ['Y' y_coordinate] 'D01' 'I' x_offset 'J'

y-offset ) '*';

Syntax

Comments

x_coordinate <Coordinate> is coordinate data – see section 0. It defines the X coordinate of the

new current point. The default is the X coordinate of the old current point.

x_coordinate

As above, but for the Y coordinate

i_offset <Offset> is the offset in X – see section 0. It defines the X coordinate the center of the

circle. It is of the coordinate type. There is no default offset.

j_offset

As above, but for the Y axis.

D01

Move operation code

After the interpolation operation the current point is set to X,Y.

Move (D02)

Moves the current point to the (X,Y) in the comment. The syntax is:

D02 = (['X' x_coordinate] ['Y' y_coordinate] 'D02') '*';

Syntax

Comments

x_coordinate <Coordinate> is coordinate data – see section 0. It defines the X

coordinate of the new current point. The default is the X coordinate of

the old current point.

x_coordinate

As above, but for the Y coordinate.

D02

Move operation code

The D02 command sets the new value for the current point. Inside a region statement it also

closes the current contour and starts a new one. (see 4.10).

Example:

X2152000Y1215000D02*

Flash (D03)

Performs a flash operation, creating a flash object at (X,Y). The syntax is:

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

D02 = (['X' x_coordinate] ['Y' y_coordinate] 'D02') '*';

Syntax

Comments

x_coordinate <Coordinate> is an integer specifying the X coordinate of the

aperture origin. The default is the X coordinate of the old current point.

x_coordinate

As above, but for the Y coordinate.

D03

Flash operation code

Example:

X1215000Y2152000D03*

After the flash operation the current point is set to (X,Y).

Example

The example shows a stream of commands in a Gerber file. Some of the commands are

operation codes, others are G code commands (G01, G03, G36, G37, G74, and G75). The G

code commands set the graphics state parameters that are relevant for the operations:

interpolation mode (G01, G02, G03, G75) – see 4.7.

Example:

X275000Y115000D02*

G01*

X2512000Y115000D01*

G75*

G03*

X5005000Y3506000I3000J0D01*

G01*

X15752000D01*

Y12221000D01*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.9 Aperture Transformations ( L P, LM, LR, LS)

Overview

The commands LP, LM, LR and LS load the following object transformation graphics state

parameters:

Object transformation commands

Command

Long name

Parameter

Load polarity

Polarity (Positive, Negative)

Load mirroring

Mirror axis (N|X|Y|XY)

Load rotation

Rotation angle

Load scaling

Scaling factor

An object transformation parameter transforms the current aperture when it is used to create

object. The transformation is temporary, after the object is created the current aperture returns

to its original value. Consequently, the parameter is always applied on the original shape of the

current aperture.

The polarity option directly sets the polarity of the objects. The mirror/rotate/scale parameters

affect the shape of the objects by temporarily transforming the current aperture before the object

is created. Flashes are mirrored/rotated/scaled around the flash point according to the

transformation parameters. Draws and arcs (D01) are also affected; however, the only useful

application seems to rotate a square aperture to align it with a draw. As the current aperture

does not affect regions shape, the mirror/rotate/scale parameters do not affect the region shape

either.

Object transformation parameters become effective immediately after loading and remain in

effect until a new value is loaded. No other command alters the object transformation

parameters. The object transformation parameters affect nor the aperture dictionary nor the

current aperture.

Example on how the parameter changes affect the image

D123* Select D123

X5000Y7000D03* Flash D123

%LR90.0*% Set object rotation to 90 degrees

X6000Y8000D03* Flash D123 rotated 90 degrees

D124* Select D124

X6000Y8000D03* Flash D124 rotated 90 degrees

%LR0.0*% Set object rotation to 0 degrees

X7000Y9000D03* Flash D124, not rotated

D123* Select D123

X1000Y2000D03* Flash D123, this is the original, not rotated

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Example of the effect on interpolations (draws and arcs)

%MOMM*%

%FSLAX26Y26*%

%ADD10C,1*% Define aperture 10 as a 1mm circle

D10*

Select aperture 10

G01*

Set linear interpolation

X00000000Y00000000D02*

Move to origin

X01000000D01*

Draw a 1mm thick line

%LS1.5*%

Set scale factor to 1.5

Y02000000D01*

Draw a 1.5mm thick line

M02*

This results in the following image:

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Load Polarity (LP)

The LP command sets the polarity graphics state parameter, see 2.5. It defines the polarity

applied to objects when they are created. Polarity can be either dark or clear. Its effect is explained

in 2.7. There is an example in 4.10.4.6. The syntax for the LP command is:

LP = '%' ('LP' ('C'|'D')) '*%';

Syntax

Comments

LP for Load Polarity

C|D

C – clear polarity

D – dark polarity

The LP command can be used multiple times in a file. The polarity remains as set until overruled

by another LP command.

Load Mirroring (LM)

The LM command sets the mirroring graphics state parameter, see 2.5. The mirroring option

defines the mirroring axis used when creating objects. The aperture is mirrored around its origin

(which may not be its geometric center) before being used. The syntax for the LM command is:

LM = '%' ('LM' ('N'|'XY'|'Y'|'X')) '*%';

Syntax

Comments

LM for Load Mirroring

N|X|Y|XY

N – No mirroring

X – Mirroring along the X axis; mirror left to right; the signs of the x

coordinates are inverted

Y – Mirroring along the Y axis; mirror top to bottom; the signs of the

y coordinates are inverted

XY – Mirroring along both axes; mirror left to right and top to bottom;

the signs of both the x and y coordinates are inverted

Mirroring is performed before the rotation.

The LM command can be used multiple times in a file. The mirroring remains as set until overruled

by another LM command. Mirroring is set at the value in the command, it is not cumulated with

the previous value.

The LM command was introduced in revision 2016.12.

Load Rotation (LR)

The LR command sets the rotation graphics state parameter, see 2.5. It defines the rotation angle

used when creating objects. The aperture is rotated around its origin (which may or may not be

its geometric center). The syntax for the LR command is:

LR = '%' ('LR' decimal) '*%';

Syntax

Comments

LR for Load Rotation

The rotation angle, in degrees, counterclockwise. A decimal.

Mirroring is performed before the rotation.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

The LR command can be used multiple times in a file. The object rotation remains as set until

overruled by a subsequent LR command. Rotation is set at the value in the command, it is not

cumulated with the previous value.

The LR command was introduced in revision 2016.12.

Load Scaling (LS)

The LS command sets the scaling graphics state parameter, see 2.5. It defines the scale factor

used when creating objects. The aperture is scaled centered on its origin (which may or may not

be its geometric center). The syntax for the LS command is:

LS = '%' ('LS' decimal) '*%';

Syntax

Comments

LS for Load Scaling

<Scale>

A decimal > 0.

The LS command can be used multiple times in a file. The object scaling remains as set until

overruled by a subsequent LS command. Scaling is set at the value in the command, it is not

cumulated with the previous scale factor.

The LS command was introduced in revision 2016.12.

Examples

Syntax

Comments

%LPD*%

Sets the object polarity to dark

%LPC*%

Sets the object polarity to clear

%LMX*%

Sets object mirroring to mirroring along the X axis

%LMN*%

Sets object mirroring to no mirroring

%LR45.0*%

Sets object rotation to 45 degrees counterclockwise

%LR-90*%

Sets object rotation to 90 degrees clockwise

%LS0.8*%

Sets object scaling to 80%

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Example of a block flashed in different mirroring, orientation, scaling

G04 Ucamco copyright*

%TF.GenerationSoftware,Ucamco,UcamX,2016.04-160425*%

%TF.CreationDate,2016-04-25T00:00:00+01:00*%

%FSLAX26Y26*%

%MOMM*%

%ADD10C,1*%

%LPD*%

G04 Define block aperture D12*

%ABD12*%

%ADD11C,0.5*%

D10*

G01*

X-2500000Y-1000000D03*

Y1000000D03*

%LPC*%

D11*

X-2500000Y-1000000D03*

%LPD*%

X-500000Y-1000000D02*

X2500000D01*

G75*

G03*

X500000Y1000000I-2000000J0D01*

G01*

%AB*%

G04 Flash block aperture D12 in four different orientation*

D12*

X0Y0D03*

%LMX*%

X10000000D03*

%LMY*%

%LR30.0*%

X0Y8000000D03*

%LMXY*%

%LR45.0*%

%LS0.8*%

X10000000D03*

%LPD*%

%LMN*%

%LR0.0*%

%LS1.0*%

M02*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

24. Block flashed in different orientations

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.10 Region Statement (G36/G37)

Region Overview

A region is a graphical object defined by its contour(s) - see 4.10.3.

The G36 command begins a region statement and G37 ends it. A region statement creates

contour objects by defining its contour. In a region statement the D01 and D02 commands

create the contour segments. The first D01 encountered in a region statement starts the first

contour by creating the first segment. Subsequent D01’s add segments to it. When a D02

command is encountered the contour is considered finished. (Note that a D02 without effect on

the current point, e.g. a D02*, also finishes the current contour. ) A D02 is only allowed if the

preceding contour is closed. The next D01 command starts a new contour. Thus an unlimited

number of contours can be created between a single G36/G37 commands pair.

When a G37 command is encountered, the region statement is closed and region graphical

objects are added to the object stream by filling the newly created contours. All object and

aperture objects are attached to the region. A G37 is only allowed when all contours are

properly closed. A G37 finishes the last contour in the absence of a finishing D02. Each contour

is filled individually. The overall filled area is the union of the filled areas of each individual

contour. The number of region objects created by a single G36/G37 pair is intentionally not

specified to leave more freedom to implementations; - for example, two overlapping contours

may be merged in a single region object.

Holes in a region are defined with cut-ins (see 4.10.3 and 4.10.4.7).

D01 and D02 are the only D code commands allowed in a region statement; D03 and Dnn

(nn≥10) are not allowed. Extended commands are not allowed. The M02 (end-of-file) command

is not allowed. However, G code commands are allowed – they are needed to control the

interpolation state.

Contour segments are not in themselves graphical objects –they define the regions which are

graphical objects.

Aperture attributes can be attached to a region, see 5.3.1.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Region Statement Syntax

The G36 and G37 commands begin and end a region statement respectively. The syntax is:

G36 = ('G36') '*';

G37 = ('G37') '*';

Syntax

Comments

G36

Begins a region statement.

G37 Ends a region statement.

This creates the set of region graphical object.

interpolation_state_command =

|G01

|G02

|G03

|G75

;

region_statement = G36 {contour}+ G37;

contour = D02 {D01|interpolation_state_command}*;

A valid contour must not only comply with this syntax, but the sequence of draws/arcs must

represent a connected closed contour that does not self-intersect. See 4.10.3.

Valid Contours

A contour is a sequence of connected linear or circular segments. A pair of segments is said to

connect only if they are defined consecutively, with the second segment starting where the first

one ends. Thus, the order in which the segments are defined is significant. Non-consecutive

segments that meet or intersect fortuitously are not considered to connect. A contour is closed:

the end point of the last segment must coincide with the start point of the first segment. A

contour thus defines a closed curve.

There are two classes of valid contours.

Simple contours. A contour is said to be simple if all its segments are disjoint, except for

consecutive segments having only their connection point in common. However, zero-length

segments have no effect: readers can remove them before processing the contour. (Avoid zero-

length segments as they are useless and can only cause confusion.) A simple contour does not

self-intersect or self-touch. The inside of the contour constitutes the region object. A simple

contour defines a simple region, without holes.

Simple cut-in contours. These contours allow to create a region with holes. A cut-in connects

the contour defining the hole to its enclosing contour, thus joining them into a single contour. If

one travels along the contour in the direction of the segments and the inside must always be to

the same side, just as for simple contours. See the illustration below; see 4.10.4.7

for a fully

worked out example.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

25. A contour with a cut-in

A cut-in is subject to strict requirements: it must consist of two fully coincident linear segments;

a pair of linear segments are said to be fully coincident if the segments coincide completely, with

the second segment starting where the first one ends; cut-ins must be either horizontal or

vertical; all cut-ins in a contour must have the same direction; cut-ins cannot intersect the

contour in any other location than their start and end points.

All contours except simple contours and simple cut-in contours are called self-intersecting and

are not allowed. Segments cannot cross, overlap or touch except

 connected segments

 cut-ins.

Any other form of self-touching or self-intersection is not allowed. For the avoidance of doubt,

not allowed are, amongst others: segments that partially overlap, fully coincident linear

segments that are diagonal, fully coincident circular segments, circular segments that are

tangent to another segment, vertices on a segment at another location than its endpoints, points

where more than two segments end, full arcs except when the contour consist solely of that full

arc or the full arc is at the end of a cut-in.

An invalid contour has no specified interpretation.

For the mathematically inclined: A contour is said to be weakly simple if there exists an

arbitrarily small perturbation of the vertices changing it in a simple contour. Simple contours with

cut-ins are weakly simple. The winding number for valid Gerber contours is for the outside 0 and

for the inside everywhere either +1 or -1, depending on the orientation. However, not all weakly

simple contours or contours with these winding numbers are valid.

Contours are also used to define outline primitives in macro apertures (see 4.5.1.6).

Processing Gerber files is inevitably subject to rounding errors. Contours must be constructed

robustly so that perturbations due to this rounding do not turn an otherwise valid contour in a

self-intersecting one. See 4.14.2.

In Gerber, the orientation of the contour is not significant.

Warning: Use maximum resolution. Low file coordinate resolution brings uncontrolled

rounding and often results in self-intersecting contours, see 4.1.

Warning: Sloppy construction of cut-ins can lead to self-intersecting contours – in fact this

is the most prevalent cause of missed clearances in planes. Construct cut-ins carefully or avoid

them altogether by making holes in regions with negative objects.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Examples

4.10.4.1 A Simple Contour

Syntax

Comments

G36*

X200Y300000D02*

G01*

X700000D01*

Y100000D01*

X1100000Y500000D01*

X700000Y900000D01*

Y700000D01*

X200000D01*

Y300000D01*

G37*

Begins a region statement

Set the current point to (2, 3). Begin of a contour.

Set linear interpolation mode

Create linear segment to (7, 3)

Create linear segment to (7, 1)

Create linear segment to (11, 5)

Create linear segment to (7, 9)

Create linear segment to (7, 7)

Create linear segment to (2, 7)

Create linear segment to (2, 3), closing the contour.

Create the region by filling the contour

26. Simple contour example: the segments

6 8 10

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

27. Simple contour example: resulting image

4.10.4.2 Use D02 to Start a Second Contour

D02 command can be used to start the new contour. All the created contours are converted to

regions when the command G37 is encountered. The example below creates two non-

overlapping contours which are then converted into two regions.

Example:

G04 Non-overlapping contours*

%FSLAX24Y24*%

%MOMM*%

%ADD10C,1.00000*%

G01*

%LPD*%

G36*

X0Y50000D02*

Y100000D01*

X100000D01*

Y0D01*

X0D01*

Y50000D01*

X-10000D02*

X-50000Y10000D01*

X-90000Y50000D01*

X-50000Y90000D01*

X-10000Y50000D01*

G37*

M02*

6 8 10

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

This creates the following image:

28. Use of D02 to start a new non-overlapping contour

Two different contours were created. Each contour is filled individually. The filled area is the

union of the filled areas.

4.10.4.3 Overlapping Contours

The example below creates two overlapping contours which are then converted into one region.

Example:

G04 Overlapping contours*

%FSLAX24Y24*%

%MOMM*%

%ADD10C,1.00000*%

G01*

%LPD*%

G36*

X0Y50000D02*

Y100000D01*

X100000D01*

Y0D01*

X0D01*

Y50000D01*

X10000D02*

X50000Y10000D01*

X90000Y50000D01*

X50000Y90000D01*

X10000Y50000D01*

G37*

M02*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

This creates the following image:

29. Use of D02 to start a new overlapping contour

Two different contours were created. Each contour is filled individually. The filled area is the

union of the filled areas. As the second contour is completely embedded in the first, the effective

filled area is the one of the first contour. The created region object is the same as would be

defined by the first contour only.

4.10.4.4 Non-overlapping and Touching

The example below creates two non-overlapping touching contours which are then converted

into one region.

Example:

G04 Non-overlapping and touching*

%FSLAX24Y24*%

%MOMM*%

%ADD10C,1.00000*%

G01*

%LPD*%

G36*

X0Y50000D02*

Y100000D01*

X100000D01*

Y0D01*

X0D01*

Y50000D01*

D02*

X-50000Y10000D01*

X-90000Y50000D01*

X-50000Y90000D01*

X0Y50000D01*

G37*

M02*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

This creates the following image:

30. Use of D02 to start a new non-overlapping contour

As these are two different contours in the same region touching is allowed.

4.10.4.5 Overlapping and Touching

The example below creates two overlapping touching contours which are then converted into

one region.

Example:

G04 Overlapping and touching*

%FSLAX24Y24*%

%MOMM*%

%ADD10C,1.00000*%

G01*

%LPD*%

G36*

X0Y50000D02*

Y100000D01*

X100000D01*

Y0D01*

X0D01*

Y50000D01*

D02*

X50000Y10000D01*

X90000Y50000D01*

X50000Y90000D01*

X0Y50000D01*

G37*

M02*

This creates the following image:

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

31. Use of D02 to start an new overlapping and touching contour

As these are two different contours in the same region touching is allowed.

4.10.4.6 Using Polarity to Create Holes

The recommended way to create holes in regions is by alternating dark and clear polarity, as

illustrated in the following example. Initially the polarity mode is dark. A big square region is

generated. The polarity mode is set to clear and a circular disk is added to the object stream;

the disk is cleared from the image and creates a round hole in the big square. Then the polarity

is set to dark again and a small square is added to the stream, darkening the image inside the

hole. The polarity is set to clear again and a small disk added, clearing parts of the big and the

small squares.

Example:

G04 This file illustrates how to use polarity to create holes*

%FSLAX25Y25*%

%MOMM*%

G01*

G04 First object: big square - dark polarity*

%LPD*%

G36*

X2500000Y2500000D02*

X17500000D01*

Y17500000D01*

X2500000D01*

Y2500000D01*

G37*

G04 Second object: big circle - clear polarity*

%LPC*%

G36*

G75*

X5000000Y10000000D02*

G03*

X5000000Y10000000I5000000J0D01*

G37*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

G04 Third object: small square - dark polarity*

%LPD*%

G01*

G36*

X7500000Y7500000D02*

X12500000D01*

Y12500000D01*

X7500000D01*

Y7500000D01*

G37*

G04 Fourth object: small circle - clear polarity*

%LPC*%

G36*

G75*

X11500000Y10000000D02*

G03*

X11500000Y10000000I2500000J0D01*

G37*

M02*

Below there are pictures which show the resulting image after adding each object.

32. Resulting image: first object only

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

33. Resulting image: first and second objects

34. Resulting image: first, second and third objects

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

35. Resulting image: all four objects

4.10.4.7 A Simple Cut-in

The example below illustrates how a simple cut-in can be used to create a hole in a region. The

coinciding contour segments must follow the requirements defined in 4.10.3.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Syntax

Comments

%FSLAX26Y26*%

G75*

G36*

X20000Y10000000D02*

G01*

X12000000D01*

Y20000000D01*

X2000000D01*

Y6000000D01*

X5000000D01*

G03*

X50000Y60000I30000J0D01*

G01*

X20000D01*

Y100000D01*

G37*

Format specification

Must be called before an arc is created

Begins a region statement

Set the current point to (2,10)

Set linear interpolation mode

Create linear contour segment to (12,10)

Create linear contour segment to (12, 2)

Create linear contour segment to (2, 2)

Create linear contour segment to (2, 6)

Create linear contour segment to (5, 6),1

fully coincident segment

Set counterclockwise circular interpolation mode

Create counterclockwise circle with radius 3

Set linear interpolation mode

Create linear contour segment to (2, 6), 2

fully coincident segment

Create linear contour segment to (2, 10)

Create the region by filling the contour

36. Simple cut-in: the segments

6 8 10

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

37. Simple cut-in: the image

Note the orientation of the inner circle. If the orientation would be different the contour would be

self-intersecting. This becomes immediately apparent if you try to perturb the contour to convert

it to a simple contour.

4.10.4.8 Fully Coincident Segments

The first example below illustrates how one contour may result in two regions. This happens

because there are two fully coincident linear segments which give the gap between filled areas.

Example:

G04 ex1: non overlapping*

%FSLAX24Y24*%

%MOMM*%

%ADD10C,1.00000*%

G01*

%LPD*%

G36*

X0Y50000D02*

Y100000D01*

X100000D01*

Y0D01*

X0D01*

Y50000D01*

G04 first fully coincident linear segment*

X-10000D01*

X-50000Y10000D01*

X-90000Y50000D01*

X-50000Y90000D01*

6 8 10

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

X-10000Y50000D01*

G04 second fully coincident linear segment*

X0D01*

G37*

M02*

This creates the following image:

38. Fully coincident segments in contours: two regions

The second example illustrates how one contour allows creating region with hole.

Example:

G04 ex2: overlapping*

%FSLAX24Y24*%

%MOMM*%

%ADD10C,1.00000*%

G01*

%LPD*%

G36*

X0Y50000D02*

Y100000D01*

X100000D01*

Y0D01*

X0D01*

Y50000D01*

G04 first fully coincident linear segment*

X10000D01*

X50000Y10000D01*

X90000Y50000D01*

X50000Y90000D01*

X10000Y50000D01*

G04 second fully coincident linear segment*

X0D01*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

G37*

M02*

This creates the following image:

39. Fully coincident segments in contours: region with hole

4.10.4.9 Valid and Invalid Cut-ins

Contours with cut-ins are susceptible to rounding problems: when the vertices move due to the

rounding the contour may become self-intersecting. This may lead to unpredictable results. The

first example below is a cut-in with valid fully coincident segments, where linear segments which

are on top of one another have the same end vertices. When the vertices move due to rounding,

the segments will remain exactly on top of one another, and no self-intersections are created.

This is a valid and robust construction.

Example:

G36*

X1220000Y2570000D02*

G01*

Y2720000D01*

X1310000D01*

Y2570000D01*

X1250000D01*

Y2600000D01*

X1290000D01*

Y2640000D01*

X1250000D01*

Y2670000D01*

X1290000D01*

Y2700000D01*

X1250000D01*

Y2670000D01*

Y2640000D01*

Y2600000D01*

Y2570000D01*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

X1220000D01*

G37*

This results in the following contour:

40. Valid cut-in: fully coincident segments

This creates the following image:

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

41. Valid cut-in: resulting image

The next example attempts to create the same image as the first example from above, but it is

invalid due to the use of invalid partially coinciding segments (see the description of a valid

contour in 4.10.3). The number of linear segments has been reduced by eliminating vertices

between collinear segments, creating invalid overlapping segments. This construction is invalid.

It is prohibited because it is not robust and hard to handle: when the vertices move slightly due

to rounding, the segments that were on top of one another may become intersecting, with

unpredictable results.

Example:

G36*

X1110000Y2570000D02*

G01*

Y2600000D01*

X1140000D01*

Y2640000D01*

X1110000D01*

Y2670000D01*

X1140000D01*

Y2700000D01*

X1110000D01*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Y2570000D01*

X1090000D01*

Y2720000D01*

X1170000D01*

Y2570000D01*

X1110000D01*

G37*

This results in the following contour:

42. Invalid cut-in: overlapping segments

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Power and Ground Planes

The simplest way to construct power and ground planes is first to create the copper pour with a

region in dark polarity (LPD), and then erase the clearances by switching to clear polarity (LPC)

and flash the anti-pads.

Example:

G04 We define the antipad used to create the clearances*

%TA.AperFunction,AntiPad*%

%ADD11C….*%

….

G04 We now define the copper pour as a region*

LPD*

G36*

X…Y…D02*

X…Y…D01*

…

G37*

G04 We now flash clearances*

%LPC*%

D11*

X…Y…D03*

This is simple and clear. In the CAD layout, the location of the anti-pads is known. With negative

anti-pads this information is transferred directly to CAM in a simple way.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Clearances in power and ground planes can also be constructed with cut-ins, as below.

43. Power and ground planes with cut-ins.

The cut-ins are rather complex to create on output; on input in CAM the cut-ins must be

removed and the original clearances restored, again rather complex. Use this more complex

construction only if there is a good reason not to use the anti-pad method.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Care must be taken to only create valid cut-ins. Sloppy cut-ins are the most frequent cause of

scrap due to faulty Gerber files, causing a self-intersecting contour and a missing clearance.

Below is an example of such sloppy cut-in; it is a real-life example that lead to expensive scrap.

Watch out for rounding errors. Make sure that coincident points indeed are coincident in the file.

With the highest resolution on outputs reduces rounding errors.

44. Power plane with invalid cut-in.

It is sometimes recommended to avoid the cut-ins altogether by splitting the plane in separate

pieces, where no piece has holes. Do not follow this terrible recommendation. The remedy is

worse than the disease. Splitting the single contour in separate contours without holes is as

complex as adding cut-ins. All clearance boundaries must be cut in pieces and split over

different contours; not much of an improvement over finding cut-in points. Rounding errors still

lurk, and can lead to pieces that are no longer connected; not much of an improvement over

invalid cut-ins. The situation is far worse on input. If the plane consists of a single contour it is

clear it is a single plane. When planes are split in pieces the coherence is lost. The file reader

must figure out from a bewildering set of contours that a single plane is intended. It must

recover clearances which boundaries are scattered over different contours. Cutting a plane in

pieces to avoid clearances is bad practice. It is asking for problems. See also 4.14.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.11 Block Aperture (AB)

Overview of block apertures

The AB command creates a block aperture. The command stream between the opening and

closing AB command defines a block aperture which is stored in the aperture dictionary. Thus

the AB commands add an aperture to the dictionary directly, without needing an AD command.

The LM, LR, LS and LP commands affect the flashes of block apertures in as any other

aperture: when a block aperture is flashed, it is first transformed according to the transformation

parameters in the graphics state and then added to the object stream.

The origin of the block aperture is the (0,0) point of the file.

A block aperture is not a single graphical object but a set of objects. While a standard or macro

aperture always adds a single graphical object to the stream, a block aperture can add any

number of objects, each with their own polarity. Standard and macro apertures always have a

single polarity while block apertures can contain both dark and clear objects.

If the polarity is dark (LPD) when the block is flashed then the block aperture is inserted as is. If

the polarity is clear (LPC) then the polarity of all objects in the block is toggled (clear becomes

dark, and dark becomes clear). This toggle propagates through all nesting levels. In the

following example the polarity of objects in the flash of block D12 will be toggled.

%ABD12*%

…

%AB*%

….

D12*

%LPC*%

X-2500000Y-1000000D03*

A D03 of a block aperture updates the current point but otherwise leaves the graphics state

unmodified, as with any other aperture.

The AB command was introduced in revision 2016.12

AB Statement Syntax

The syntax for the AB command is:

<AB command> = AB[<block aperture number>]*

Syntax

Comments

AB for Aperture Block. Opens/closes an AB statement.

<block aperture

number>

The aperture number under which the block is stored in the

aperture dictionary.

Examples:

Syntax

Comments

%ABD12*%

Opens the definition of aperture D12

%AB*%

Closes the current AB statement.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

The section between the opening and closing AB commands can contain nested AB

commands. The resulting apertures are stored in the library and are available subsequently until

the end of the file, also outside the enclosing AB section. The syntax is:

AB_statement = AB_open {in_block_statement}* AB_close;

AB_open = '%' ('AB' aperture_ident) '*%';

AB_close = '%' ('AB') '*%';

in_block_statement =

|single_statement

|region_statement

|AB_statement

;

single_statement =

| operation

| interpolation_state_command

| Dnn

| G04

| attribute_command

| AD

| AM

| coordinate_command

| transformation_state_command

;

Consequently, an AB statement can contain embedded AB statements. The scope of names

defined by an AB statement is the whole file.

The current point is undefined after an AB statement.

Usage of Block Apertures

The main purpose of block apertures is to repeat a sub-image without the need to repeat all the

generating commands. Block apertures can be repeated at any location and individually mirrored,

rotated and scaled. Block apertures are more powerful than the SR command: the SR only allows

repeats on a regular grid, without mirror, rotate or scale, and, crucially, without nesting. Blocks

are typically used to create panels without duplicating the data.

The second purpose of block apertures is to complement macro apertures. A block aperture

consisting of a single region creates a single object with one polarity– as with standard or macro

apertures. Thus, single object apertures of any shape can easily be created. Such a block

aperture can be used to define pads. Blocks are simpler to create than macros. However, macros

can have parameters and blocks cannot. On the other hand, a macro outline primitive support

only linear segments while the contours in blocks support both linear and circular segments.

Do not use blocks – or macros - when a standard aperture is available. Standard apertures are

built-in and therefore are processed faster.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Example

A complete Gerber file with nested blocks

G04 Ucamco copyright*

%TF.GenerationSoftware,Ucamco,UcamX,2016.04-160425*%

%TF.CreationDate,2016-04-25T00:00;00+01:00*%

%TF.Part,Other,Testfile*%

%FSLAX46Y46*%

%MOMM*%

G04 Define standard apertures*

%ADD10C,7.500000*%

%ADD11C,15*%

%ADD12R,20X10*%

%ADD13R,10X20*%

G04 Define block aperture 100, consisting of two draws and a round dot*

%ABD100*%

D10*

X65532000Y17605375D02*

Y65865375D01*

X-3556000D01*

D11*

X-3556000Y17605375D03*

%AB*%

G04 Define block aperture 102, consisting of 2x3 flashes of aperture 101

and 1 flash of D12*

%ABD102*%

G04 Define nested block aperture 101, consisting of 2x2 flashes of

aperture 100*

%ABD101*%

D100*

X0Y0D03*

X0Y70000000D03*

X100000000Y0D03*

X100000000Y70000000D03*

%AB*%

D101*

X0Y0D03*

X0Y160000000D03*

X0Y320000000D03*

X230000000Y0D03*

X230000000Y160000000D03*

X230000000Y320000000D03*

D12*

X19500000Y-10000000D03*

%AB*%

G04 Flash D13 twice outside of blocks*

D13*

X-30000000Y10000000D03*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

X143000000Y-30000000D03*

G04 Flash block 102 3x2 times*

D102*

X0Y0D03*

X0Y520000000D03*

X500000000Y0D03*

X500000000Y520000000D03*

X1000000000Y0D03*

X1000000000Y520000000D03*

M02*

45. Block aperture example 1

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.12 Step and Repeat (SR)

The purpose of the SR command is to replicate a set of graphical objects without replicating

the commands that creates the set.

The SR command %

SRX…Y…I…J…*% opens an SR statement. All subsequent commands are

part of the SR statement until it is closed by an

%SR*%. The parameters X, Y specify the number

of repeats in X and Y and I, J their respective step distances. The graphical objects generated

by the command stream in a SR statement are collected in a block - see 2.8 - instead of being

added directly to the object stream. When the SR command is closed by an

%SR*%, the block is

step-repeated (replicated) in the image plane according to the parameters X, Y, I and J in the

opening SR command. Blocks are copied first in the positive Y direction and then in the positive

X direction. The syntax for the SR command is:

<SR command> = SR[X<Repeats>Y<Repeats>I<Distance>J<Distance>]*

Syntax

Comments

SR for Step and Repeat

X<Repeats> Defines the number of times the block is repeated along the X axis.

<Repeats> is an integer ≥ 1

Y<Repeats> Defines the number of times the block is repeated along the Y axis.

<Repeats> is an integer ≥ 1

I<Distance> Defines the step distance along the X axis.

<Distance> is a decimal number ≥ 0, expressed in the unit of the MO

command

J<Distance> Defines the step distance along the Y axis.

<Distance> is a decimal number ≥ 0, expressed in the unit of the MO

command

Examples:

Syntax

Comments

%SRX2Y3I2.0J3.0*%

Opens an SR statement and starts block accumulation.

When block accumulation is finished the block will be repeated 2 times

along the X axis and 3 times along the Y axis. The step distance

between X-axis repeats is 2.0 units. The step distance between Y-

axis repeats is 3.0 units.

%SRX4Y1I5.0J0*%

Opens an SR statement and starts block accumulation.

When block accumulation is finished the block will be repeated 4 times

along the X axis with the step distance of 5.0 units. The step distance

in the J parameter is ignored because no repeats along the Y axis are

specified.

%SR*%

Closes the SR statement and repeats the previously accumulated

block

The syntax is:

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

SR_statement = SR_open {in_block_statement}* SR_close;

SR_open = '%' ('SR' 'X' positive_integer 'Y' positive_integer 'I' decimal 'J'

decimal) '*%';

SR_close = '%' ('SR') '*%';

in_block_statement =

|single_statement

|region_statement

|AB_statement

;

single_statement =

| operation

| interpolation_state_command

| Dnn

| G04

| attribute_command

| AD

| AM

| coordinate_command

| transformation_state_command

;

Example:

G04 A block of two flashes is repeated 3x2 times*

%SRX3Y2I5.0J4.0*%

D13*

X123456Y789012D03*

D14*

X456789Y012345D03*

%SR*%

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

46. Blocks replication with SR command

Note that a block contains the graphical objects, not the Gerber source code. The graphical

objects in each copy are always identical, even if the graphics state is modified during the SR

statement.

The current point is undefined after an SR statement.

A file can contain multiple SR statements. The number of steps and the step distances can be

different in X and Y. The number of repeats along an axis can be one; it is then recommended

to use the step distance 0.

A step & repeat block can contain different polarities (LPD and LPC – see 4.9.2

). A clear object

in a block clears all objects beneath it, including objects outside the block. When repeats of

blocks with both dark and clear polarity objects overlap, the step order affects the image; the

correct step order must therefore be respected: step the complete block first in Y and then in X.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.13 End-of-file (M02)

The M02 command indicates the end of the file. The syntax is as follows:

M02 = ('M02') '*';

Example:

M02*

The last command in a Gerber file must be the M02 command. No data is allowed after an M02.

Gerber readers are encouraged to give an error on a missing M02 as this is an indication that

the file has been truncated.

Note that a block or region statement must be explicitly closed. Consequently, an M02

command cannot be issued within a block or region statement.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

4.14 Numerical Accuracy

The coordinates of all points and all geometric parameters (e.g. a diameter) have an exact

numerical value. Graphical objects are therefore in principle defined with infinite precision with

the exception of arcs, which are intrinsically slightly fuzzy (see 4.7.2.). A Gerber file specifies an

image with infinite precision.

However, Gerber file writers cannot assume that file readers will process their files with infinite

precision as this is simply impossible. Nemo potest ad impossibile obligari. This raises the

question to what a Gerber file reader is held, and what a Gerber writer can assume.

Visualization

Gerber files are often used to visualize an image on a screen, a photoplotter, a direct imager.

Visualization is unavoidably constrained by the limitations of the output device. Nonetheless,

visualization must comply with the following rules:

 Each individual graphical object must be rendered within the stated accuracy of the output

device.

 No spurious holes may appear - solid objects must be visualized solid.

 No spurious objects may appear.

 Zero-size objects are not visualized.

 Graphical object can be rendered individually, without considering neighboring objects. In

other words, each graphical object is handled individually, regardless of context.

It is intentionally not specified if rendering must be “fat” or “thin” - fat meaning that features

below the device accuracy are blown up to be visible, thin meaning that they disappear.

These rules have several noteworthy consequences:

 Gerber objects separated by a very small gap may touch in the visualized image.

 Gerber objects that touch or marginally overlap may be separated by a gap in the

visualized image.

 Gerber objects smaller or thinner than the device resolution may totally disappear in the

visualized image.

 When what is intended to be a single object is broken down in simpler graphical objects,

and these elementary objects do not sufficiently overlap, the resulting image may not be

solid - it may have internal holes or even break up in pieces. To avoid these effects the best

and most robust approach is not to break up the single object at all: the Gerber format has

powerful primitives to create almost any shape with a single graphical object or possible a

succession of dark and clear objects.

Construct files robustly.

Image Processing

Gerber files are processed for visualization but often also to complex image processing

algorithms: e.g. etch compensation, design rule checks in CAM and so on. These algorithms

perform long sequences of numerical calculations. Rounding errors unavoidably accumulate.

Coordinates can move and object sizes can vary. The specification limits the allowed

perturbation to [-0.5µm, +0.5 µm]; furthermore coincident coordinates must remain coincident.

The writer can assume that the perturbation is within this limit. Higher accuracy cannot be

blindly assumed; if it is needed it must be checked that the applications downstream can handle

this. A file is therefore only robust if, under any allowed perturbation, it remains valid and

represents the same image.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

The perturbation has some noteworthy consequences:

 Contours that are not self-intersecting by a margin of ≤1µm can become self-intersecting

under a valid perturbation. Such contours are therefore invalid; see section 4.10.3.

Contours must be constructed robustly so that allowed processing perturbations do not turn

an otherwise valid contour in a self-intersecting one. See 4.14.2. Consequently, points and

segments that are not coincident must be separated by at least 1µm. Furthermore, circular

segments add their own intrinsic fuzziness, see 4.7.2. If any valid interpretation of the arc

violates the requirement of 1µm separation the contour is invalid. Construct contours

defensively. Observe sufficient clearances. Marginal contours can and do lead to problems

 Objects that touch or overlap marginally can become separated under perturbation. This is

important for electrical connection. An electrical connection that is realized by touching

objects can get separated by a valid perturbation. Such marginal construction can be validly

interpreted as either isolating or connecting. Make proper and robust electrical connections,

with an overlap of the order of magnitude of at least the minimum conductor width.

 Arcs with end points separated by less than 1 µm can toggle between very small or nearly

360 degrees under valid perturbations. Do not write such arcs.

 Avoid objects smaller than 1 µm.

Construct files robustly.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

5 Attributes

5.1 Attributes Overview

Attributes add meta-information to a Gerber file. Attributes are akin to labels providing

information about the file or features within them. Examples of meta-information conveyed by

attributes are:

 The function of the file in the layer structure. Is the file the top solder mask, the bottom

copper layer, …?

 The function of a pad. Is the pad an SMD pad, or a via pad, or a fiducial, ...?

The attribute syntax provides a flexible and standardized way to add meta-information to a

Gerber file, independent of the specific semantics or application.

Attributes do not affect the image. A Gerber reader will generate the correct image if it simply

ignores the attributes.

Each attribute consists of an attribute name and an optional attribute value:

<Attribute> = <AttributeName>[,<AttributeValue>]*

Attribute names follow the name syntax in section 3.4.3.

The attribute value consists of one or more comma-separated fields, see section 3.4.4.

<AttributeValue> = <Field>{,<Field>}

There are three types of attributes by the item they attach to:

Attachment type

The item to which they attach meta-information

File attributes

Attach meta-information to the file as a whole.

Aperture attributes Attach meta-information to an aperture or a region. Objects created by

the aperture inherit the aperture meta-information

Object attributes

Attach meta-information to on object directly

There are two types of attributes by the scope of their use:

 Standard attributes. Standard attribute names, values and semantics are defined in this

specification and are part of it. As they are standardized, they can exchange meta-

information between all applications.

 User attributes. User attributes can be chosen freely by users to extend the format with

custom meta-information. Use custom attributes only for unequivocally defined

machine-readable information, use G04 for mere human-readable comments.

In accordance with the general rule in 3.4.3 standard attribute names must begin with a dot ‘.’

while user attribute names cannot begin with a dot. The dot, if present, is part of the attribute

name and indicates that it is a standard attribute whose syntax and semantics are defined in

section 5.6.

Example of a user attributes:

%TFMyAttribute,Yes*%

%TFZap*%

%TFZonk*%

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

The following commands govern attributes. (They start with a T as the more obvious A is

already taken by the aperture commands.)

Command

Description

Section

Attribute file. Set a file attribute.

5.2

TA Attribute aperture. Add an aperture attribute to the dictionary or

modify it.

5.3

TO Attribute object. Add an object attribute to the dictionary or modify

it.

5.4

Attribute delete. Delete one or all attributes in the dictionary.

5.5

The syntax is as follows:

TF = '%' ('TF' attribute_name {',' attribute_value}*) '*%';

TA = '%' ('TA' attribute_name {',' attribute_value}*) '*%';

TO = '%' ('TO' attribute_name {',' attribute_value}*) '*%';

TD = '%' ('TD' [attribute_name]) '*%';

attribute_name = field;

attribute_value = field;

During the processing of a Gerber file an attribute dictionary is maintained. Dictionary entries

consist of the attribute name, its domain and its value. The attribute name is the key of the

entry; it must consequently be unique, even for attributes with a different domain.

The current aperture dictionary is defined after each command by the following rules:

 Initially the attribute dictionary is empty

 File attributes are added with the TF command

 Aperture attributes are added or updated with the TA command

 Object attributes are added or updated with the TO command

 Attributes are deleted with the TD command

When an aperture or a graphical object is created all attributes with the proper domain present

in the dictionary at the time of creation are attached to it. They remain fixed and cannot be

changed.

In the following example the command TF defines an attribute with name “.FileFunction” and

value composed of the two fields: “Soldermask,Top”.

Example:

%TF.FileFunction,Soldermask,Top*%

Note that attribute commands are not allowed within a region statement, see 4.10.2.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

5.2 File Attributes (TF)

File attributes provide meta-information about entire files.

The semantics of a file attribute specifies where it must be defined, typically in the header of the

file. A file attribute can only be defined once. It cannot be redefined.

File attributes are set with the uppercase TF command with the following syntax

<TF command> = %TF<AttributeName>[,<AttributeValue>]*%

<AttributeValue> = <Field>{,<Field>}

The attribute name must follow the syntax in section 3.4.3, fields this in 3.4.4. The name is

unique and cannot be used for any other attribute, even of another type.

Example:

%TF.FilePolarity,Negative*%

5.3 Aperture Attributes (TA)

An aperture attribute is attached to an aperture or a region. They are a method to assign

attributes to graphical objects in bulk: all objects that are created with an aperture inherit its

attributes; for example, a via attribute on an aperture means that all pads flashed with this

aperture are via pads. Providing information about graphical objects via their apertures is

elegant, compact and efficient. As region objects are created without intermediary aperture,

aperture objects can be assigned to regions directly.

The TA command adds an aperture attribute into the attributes dictionary. It has the following

syntax:

<TA command> = %TA<AttributeName>[,<AttributeValue>]*%

<AttributeValue> = <Field>{,<Field>}

The attribute name must follow the syntax in section 3.4.3, fields the one in 3.4.4. The name

must be unique. The value of an aperture attribute can be modified by a new TA with the same

attribute name.

The example below defines several attributes.

Example:

%TA.AperFunction,ComponentPad*%

%TAMyApertureAttributeWithValue,value*%

%TAMyApertureAttributeWithoutValue*%

In the next example the aperture value is initially set to ComponentPad and later overruled to

ViaPad.

Example:

%TA.AperFunction,ComponentPad*%

…

%TA.AperFunction,ViaPad*%

When an AD or an AB command creates an aperture all aperture attributes then in the attribute

dictionary are attached to it. Once an aperture is defined its attributes cannot be changed.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Aperture Attributes on Regions

Counter-intuitively, aperture attributes can be attached to regions. When a G36/G37 creates a

region all aperture attributes in the dictionary are attached to it, in the same way as they are

attached to an aperture created with an AD command. A way to view this is that the G36

command creates a virtual region aperture and attaches attributes to it in the same way as an

AD. Regions effectively function as single-use apertures that are flashed and immediately

forgotten when the region definition is completed.

Aperture attributes on regions are necessary. Aperture attributes are a way to attach properties

to objects such as draws or flashes. It is sometimes necessary to attach the same property to

region objects. For example, the function ‘conductor’ must be assigned both to tracks – draws –

and copper pours – regions. For the tracks this is done with an aperture attribute, a convenient

way to attach an attribute to a larger number of objects. For the regions this is done with the

mechanism in the first paragraph.

Note that aperture attributes are not attached directly to draws, arcs and flashes, because there

it is done indirectly via their aperture.

Example: Define a copper pour as a region

%TA.AperFunction,Conductor*%

G36*

X118151529Y-78573554D02*

G01*

X118230607Y-78626393D01*

X118283446Y-78705471D01*

X118302000Y-78798750D01*

X118302000Y-79286250D01*

…

X118151529Y-78573554D01*

G37*

For the avoidance of doubt: regions take the aperture attributes from the dictionary, not from the

current aperture.

5.4 Object Attributes (TO)

An object attribute is attached to graphical objects. When a D01, D03 or region statement

(G36/G37) creates an object all object attributes in the attribute dictionary are attached to it. As

attribute commands are not allowed inside a region statement, all regions created by that

statement have the same object attributes. Once attached to an object they cannot be changed.

The TO command adds an object attribute into the attributes dictionary. It has the same syntax

as the TF command:

<TO command> = %TO<AttributeName>[,<AttributeValue>]*%

<AttributeValue> = <Field>{,<Field>}

The attribute name must follow the syntax in section 3.4.3, fields the one in 3.4.4. The name is

unique and cannot be used for any other attribute, even of another type. The value of an object

attribute can be modified by a new TO command with the same attribute name.

Example:

%TO.C,R6*%

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

5.5 Delete Attribute (TD)

The TD command deletes an attribute from the attributes dictionary. Note that the attribute

remains attached to apertures and objects to which it was attached before it was deleted.

<TD command> = %TD[<AttributeName>]*%

The <AttributeName> is the name of the attribute to delete. If omitted, the whole dictionary is

cleared.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

5.6 Standard Attributes

Overview

Name Usage Section Attached

.Part

Identifies the part the file represents, e.g. a

single PCB

5.6.2 File

.FileFunction

Identifies the file’s function in the PCB, e.g. top

copper layer

5.6.3 File

.FilePolarity

Positive or Negative. This defines whether

the image represents the presence or

absence of material.

5.6.4 File

.SameCoordinates

All files in a fabrication data set with this

attribute use the same coordinates. In other

words, they align.

5.6.5 File

.CreationDate

Defines the creation date and time of the

file.

5.6.6 File

.GenerationSoftware

Identifies the software creating the file.

5.6.7

File

.ProjectId

Defines project and revisions.

5.6.8

File

.MD5

Sets the MD5 file signature or checksum.

5.6.9

File

.AperFunction

Function objects created with the apertures,

e.g. SMD pad

5.6.10 Aperture

.DrillTolerance

Tolerance of drill holes

5.6.11

Aperture

.FlashText

If a flash represents text allows to define

string, font, …

5.6.12 Aperture

The CAD net name of a conducting object,

e.g. Clk13.

5.6.13 Graphical

object

The pin number (or name) and reference

descriptor of a component pad on an outer

layer, e.g. IC3,7.

5.6.14 Graphical

object

The component reference designator linked

to an object, e.g C2.

5.6.15 Graphical

object

Table with the standard attributes

Attributes are not needed when the image only needs to be rendered. However, attributes are

needed in PCB fabrication data, when transferring PCB data from design to fabrication. For

example, the fabricator needs to know what are the via pads to handle the solder mask

properly. The standard attributes transfer the design intent from CAD to CAM in an unequivocal

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

and standardized manner. This is sometimes rather grandly called “adding intelligence to the

image”. Without standard attributes the design intent must be gathered from various documents,

unwritten rules, conversations or reverse engineering, with all the risks of error and delay that

this entails.

It is strongly recommended to use standard attributes as comprehensively as possible. If you

cannot provide all the attributes or are unsure of their use then provide all the attributes you are

comfortable with. Partial information is better than no information. For professional PCB

production the bare minimum is to set .FileFunction and .FilePolarity.

Note that standard attribute values typically contain a value “Other” to cater to requirements not

yet foreseen in the specification. The intention is to add new values as the need arises to

reduce the use of “Other” over time.

We are open to your suggestions for new generally useful attributes. Please contact Ucamco at

[email protected]

to request it. Authors will be properly acknowledged when their

suggestions are included in the standard.

Warning: Do not invent your own standard attribute names (names starting with a dot).

This would defeat the purpose of standardization. User attributes cater to specific needs that are

not covered by the standard attributes. Feel free to invent any user attribute you wish.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

.Part

The value of the .Part file attribute identifies which part is described. The attribute – if present -

must be defined in the header.

.Part value

Usage

Single

Single PCB

Array

A.k.a. customer panel, assembly panel, shipping panel,

biscuit

FabricationPanel

A.k.a. working panel, production panel

Coupon

A test coupon

Other,<mandatory

field>

None of the above. The mandatory field informally

indicates the part

.Part file attribute values

Example:

%TF.Part,Array*%

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

.FileFunction

The .FileFunction file attribute identifies the function of the file in the PCB layer structure. Of all

the attributes it is the most important.

Example:

%TF.FileFunction,Copper,L1,Top*%

The attribute must be defined in the header.

The existence of a file function does not mean that it must be included in each PCB fabrication

data sets. Include the files that are needed: no more, no less.

The file functions are designed to support all file types in current use. If a type you need is

missing please contact us at [email protected].

.FileFunction value

Usage

Data files

Copper,L,(Top|Inr|Bot)[,<type>]

A conductor or copper layer.

L (p is an integer>0) specifies the physical

copper layer number. Numbers are

consecutive. The top layer is always L1. (L0

does not exist.) The mandatory field

(Top|Inr|Bot) specifies it as the top, an inner or

the bottom layer; this redundant information

helps in handling partial data. The specification

of the top layer is “

Copper,L1,Top[,type]”,

of the bottom layer of an 8 layer job it is

Copper,L8,Bot[,type]

The top side is the one with the through-hole

components, if any.

The optional <type> field indicates the layer

type. If present it must take one of the following

values: Plane, Signal, Mixed or Hatched.

Plated,i,j,(PTH|Blind|Buried)

[,<label>]

Plated drill/rout data, span from copper layer i

to layer j. The from/to order is not significant.

The (PTH|Blind|Buried) field is mandatory.

The label is optional. If present it must take one

of the following values: Drill, Rout or Mixed.

NonPlated,i,j,(NPTH|Blind|Buried)

[,<label>]

Non-plated drill/rout data, span from copper

layer i to layer j. The from/to order is not

significant. The (NPTH|Blind|Buried) field is

mandatory.

The label is optional. If present it must take one

of the following values: Drill, Rout or Mixed.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

.FileFunction value

Usage

Profile,(P|NP)

A file containing the board profile (or outline)

and only the board profile. Such a file is

mandatory in a PCB fabrication data set. See

6.5.

The mandatory (P|NP) label indicates whether

board is edge-plated or not.

Soldermask,(Top|Bot)[,<index>]

Solder mask or solder resist.

Usually the image represents the solder mask

openings; it then has negative polarity, see

5.6.4.

The optional field is only needed when there is

more than one solder mask on one side – top

or bottom. The integer <index> then numbers

the solder masks from the PCB side outwards,

starting with 1 for the mask directly on the

copper. Usually there is only one solder mask

on a side, and then <index> is omitted. An

example with two top solder masks:

Soldermask,Top,1 Mask on the copper

Soldermask,Top,2  Mask on the first

mask

Legend,(Top|Bot)[,<index>]

A legend is printed on top of the solder mask to

show which component goes where. A.k.a.

‘silk’ or ‘silkscreen’.

See the Soldermask entry for an explanation of

the index.

Component,L,(Top|Bot)

A layer with component information.

L The integer p is the copper layer number

to which the components described in this file

are attached. (Top|Bot) indicates if the

components are on top, upwards, or on the

bottom, downward, of the layer to which they

are attached. This syntax caters for embedded

components.

For jobs without embedded components there

is an intentional redundancy.

Paste,(Top|Bot)

Locations where solder paste must be applied.

Glue,(Top|Bot)

Glue spots used to fix components to the board

prior to soldering.

Carbonmask,(Top|Bot)[,<index>]

See Soldermask for the usage of <index>.

Goldmask,(Top|Bot)[,<index>]

See Soldermask for the usage of <index>.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

.FileFunction value

Usage

Heatsinkmask,(Top|Bot)[,<index>]

See Soldermask for the usage of <index>.

Peelablemask,(Top|Bot)[,<index>]

See Soldermask for the usage of <index>.

Silvermask,(Top|Bot)[,<index>]

See Soldermask for the usage of <index>.

Tinmask,(Top|Bot)[,<index>]

See Soldermask for the usage of <index>.

Depthrout,(Top|Bot)

Area that must be routed to a given depth

rather than going through the whole board.

Vcut[,(Top|Bot)]

Contains the lines that must be v-cut. (V-

cutting is also called scoring.)

If the optional attachment (Top|Bot) is not

present the scoring lines are identical on top

and bottom – this is the normal case. In the

exceptional case scoring is different on top and

bottom two files must be supplied, one with

Top and the other with Bot.

Viafill

Contains the via’s that must be filled. It is

however recommended to specify the filled

via’s with the optional field in the .AperFunction

ViaDrill.

Drawing files

Drillmap

A drawing with the locations of the drilled

holes. It often also contains the hole sizes,

tolerances and plated/non-plated info.

FabricationDrawing

A auxiliary drawing with additional information

for the fabrication of the bare PCB: the location

of holes and slots, the board outline, sizes and

tolerances, layer stack, material, finish choice,

etc.

Vcutmap

A drawing with v-cut or scoring information.

AssemblyDrawing,(Top|Bot)

An auxiliary drawing with the locations and

reference designators of the components. It is

mainly used in PCB assembly.

ArrayDrawing

A drawing of the array (biscuit, assembly

panel, shipment panel, customer panel).

OtherDrawing,<mandatory field>

Any other drawing than the five ones above.

The mandatory field informally describes its

topic.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Other files

Pads,(Top|Bot)

A file containing only the pads (SMD, BGA,

component, …). Not needed in a fabrication

data set.

Other,<mandatory field>

The value ‘Other’ is to be used if none of the

values above fits. By putting ‘Other’ rather than

simply omitting the file function attribute it is

clear the file has none of the standard

functions, already useful information. Do not

abuse standard values for a file with a vaguely

similar function – use ‘Other’ to keep the

function value clean and reliable.

The mandatory field informally describes the

file function.

.FileFunction attribute values

Examples. File functions of a four layer board (One for each Gerber file):

%TF.FileFunction,Legend,Top*%

%TF.FileFunction,Soldermask,Top*%

%TF.FileFunction,Copper,L1,Top*%

%TF.FileFunction,Copper,L2,Inr,Plane*%

%TF.FileFunction,Copper,L3,Inr,Plane*%

%TF.FileFunction,Copper,L4,Bot*%

%TF.FileFunction,Soldermask,Bot*%

%TF.FileFunction,NonPlated,1,4,NPTH,Drill*%

%TF.FileFunction,NonPlated,1,4,NPTH,Rout*%

%TF.FileFunction,Plated,1,4,PTH*%

%TF.FileFunction,Profile,NP*%

%TF.FileFunction,Drillmap*%

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

.FilePolarity

The .FilePolarity specifies whether the image represents the presence or absence of material.

The .FilePolarity attribute does not change the image - no attribute does. It changes the

interpretation of the image. For example, in a copper layer in positive polarity a round flash

generates a copper pad. In a copper layer in negative polarity it generates a clearance.

The attribute must be defined in the header.

Warning: Solder mask images nearly always represent the solder mask openings and are

therefore negative. This may be counter-intuitive.

Drill and rout files represent the removed material. Drill files are therefore positive, as is intuitive.

.FilePolarity value

Usage

Positive

The image represents the presence of material

(recommended)

Negative

The image represents the absence of material

.FilePolarity attribute values

Example:

%TF.FileFunction,Copper,L2,Inr,Plane*%

%TF.FilePolarity,Positive*%

Note: It is recommended output copper layers in positive. Power/ground planes in negative

was introduced in the 1970s and 1980s to get around the limitations in the vector photoplotters

then used. There is no longer any reason to use them, and they have a problem: they cannot

not define how close the copper gets to the outline of the PCB. See 4.10.5 in how to create

power/ground planes in positive. But if you need to output negative copper layers, make it clear

they are negative by setting the .FilePolarity attribute.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

.SameCoordinates

All layers in a PCB fabrication data set- a folder or archive - must use the same coordinate

system. In other words, they must align or register as the layers in the physical PCB do. For

example, the pads, drill holes, pads and solder mask openings of a pad stack must all have the

same coordinates.

Layers must not be offset, mirrored of flipped versus one another. This may seem obvious but

unfortunately layers do not align in 1/3 of the data sets. The fabricator consequently cannot trust

the alignment of the incoming data. This uncertainty interferes with fast and automatic

processing; worse, it can lead to scrap with boards where wrong alignment is not obvious, such

as very symmetric HF boards.

The .SameCoordinates attribute tells the fabricator that the alignment is correct.

The attribute must be defined in the header. The syntax is as follows:

%TF.SameCoordinates[,<ident>]*%

Example – without ident:

%TF.SameCoordinates*%

If this attribute is present in a number of Gerber files in a PCB fabrication data set then

these files are in alignment with each other.

Example – with a GUID as ident:

%TF.SameCoordinates,f81d4fae-7dec-11d0-a765-00a0c91e6bf6*%

The ident is optional. Its purpose is the following. There may be situations where files in the

fabrication data are output at different times, with different coordinate systems. In that

situation simply outputting the attribute would wrongly signal the layers do align. Adding the

ident avoids this error by distinguish between these different coordinate systems at output

time. If the attribute with the same ident is present in a number of Gerber files then they

align. If the ident is different they may not align – which would be an error because all files

must align. For the fabricator the only important fact is whether the ident, if present, are

identical or not; otherwise the ident has no meaning. A very safe ident is a GUID. When all

files are output at the same time, with the same coordinates, the ident is not needed.

Note that all data files must align anyhow, attribute or no attribute.

.CreationDate

The .CreationDate file attribute identifies the moment of creation of the Gerber file.

The attribute – if present - must be defined in the header. The attribute value must conform to

the full version of the ISO 8601 date and time format, including the time zone. A formally defined

creation date can be helpful in tracking revisions – see also 5.6.8

Example:

%TF.CreationDate,2015-02-23T15:59:51+01:00*%

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

.GenerationSoftware

The .GenerationSoftware file attribute identifies the software that generated the Gerber file. The

field <vendor> identifies the organization that supplies the generating software to its users; this

can be a commercial company, an open source organization, etc.

The attribute – if present - must be defined in the header. The syntax is as follows:

%TF.GenerationSoftware,<vendor>,<application>[,<version>]*%

Example:

%TF.GenerationSoftware,Ucamco,UcamX,2017.04*%

.ProjectId

Usually a Gerber file is part of a PCB project with a sequence of revisions. The purpose of the

.ProjectId file attribute is to uniquely identify project and revision. This is especially important to

check whether all files belong to the same revision. By its nature, these values can only be

defined by the creator of the project and revision.

The attribute – if present - must be defined in the header. The syntax is as follows:

%TF.ProjectId,<Name>,<GUID>,<Revision>*%

The field <Name> is the id or reference used by the design owner, <GUID> defines the project

using a global unique ID and <Revision> specifies its revision. All parameters must conform to

the field syntax, see 3.4.4. The <GUID> is a field conforming to RFC4122 version 1 or version 4.

Examples:

%TF.ProjectId,My PCB,f81d4fae-7dec-11d0-a765-00a0c91e6bf6,2*%

%TF.ProjectId,project#8,68753a44-4D6F-1226-9C60-0050E4C00067,/main/18*%

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

.MD5

The .MD5 file attribute sets a file signature (checksum, hash, digest) that uniquely identifies the

file and provides a high degree of security against accidental modifications.

The .MD5 checksum is not intended for CAD to CAM data transfer which is probably sufficiently

protected by the checksum of the zip, but rather for individual files used within fabrication, with a

bewildering collection of legacy systems and protocols, and where file transmission errors

sometimes occur.

The 128 bit signature is calculated with the MD5 algorithm and expressed as a 32 digit

hexadecimal number (see Error! Reference source not found.). The signature is calculated

over the bits from the beginning of the file up to but excluding the .MD5 file attribute command.

Note that this excludes the closing M02*. The complete .MD5 file attribute command, with both

‘%’and ‘*’, is excluded. Any CR and LF are excluded from signature calculation. As CR and LF

do not affect the interpretation of the file but may be altered when moving platforms excluding

them makes the signature portable without sacrificing security.

The signature, if present, must be put at the end of the file, just before the closing M02*. Thus

the file can be processed in a single pass.

Example:

Consider the following Gerber file segment, without checksum:

…

D11*

X1500000Y2875000D03*

X2000000D03*

D19*

X2875000Y2875000D03*

M02*

As the CR and LF characters are skipped the checksum is taken over the following data:

…D11*X1500000Y2875000D03*X2000000D03*D19*X2875000Y2875000D03*

With the checksum the file then becomes:

…

D11*

X1500000Y2875000D03*

X2000000D03*

D19*

X2875000Y2875000D03*

%TF.MD5,6ab9e892830469cdff7e3e346331d404*% <- Excluded from the MD5

M02* <- Excluded from the MD5

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

The following Perl script specifies precisely how the .MD5 is calculated:

#script expects one parameter (original Gerber X2 file)

use Digest::MD5;

local $_ = shift;

local *IN;

my $content;

local $/;

open(IN, "<$_") or die "Cannot open $_ due to $!";

$content = <IN>; #read file to the variable

close IN;

$content =~ s/\r|\n//g; #remove all CRLF (end of line) characters

$content =~ s/M02\*//; #remove M02 from the end of file

#calculate MD5

$md5 = Digest::MD5->new; #init MD5

$md5->add($content); #send content of the file to MD5 engine

print "Add 2 following lines to the Gerber file, please.\n";

print "%TF.MD5,";

print $md5->hexdigest; #print correct MD5 hash

print "*%\nM02*\n\n";

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

.AperFunction

The .AperFunction aperture attribute defines the function or purpose of an aperture, or rather

the graphical objects created with it. PCB CAM needs to know the function of graphical objects,

especially pads. If this is not possible define the function of all attributes then at least define if

for those where you can - partial information is better than no information. The bare minimum is

to identify via pads: the PCB fabricator must know where the via pads are.

One function, one aperture. Objects with different functions must have different apertures,

even if they are of the same shape and size. Apertures with multiple functions are devilishly

hard to handle in CAM to start with: the CAM operator can no longer perform functions per

aperture, but must check each individual hole. Furthermore, their functions cannot be identified

by an aperture attribute: all objects created with it have the same function. This also applies to

drill tools: e.g. if the same diameter is used for component holes and via holes, these still must

be separate apertures. It is recommended to also use different apertures for drill holes and rout

slots.

Regions. Counterintuitively, regions can carry aperture attributes, see 5.3.1. Use .AperFunction

to define the function of the regions.

Painting (aka vector-fill).

It is strongly recommended not to use painting, see 7.2. If you still construct objects by painting,

the function of the painted object is set by the function of apertures used for painting. For

example, if aperture 21 is used to paint SMD pads then the function of aperture 21 is SMDPad.

If aperture 50 is used to paint a conductive region then the function of aperture 50 is conductor.

The .AperFunction values are defined in the tables below. Note that the attribute values typically

can only be applied to specific layers - for example, an SMD pad can only be defined on an

outer copper layer.

Drill and rout files

Note that these values can apply to drill holes and rout slots.

.AperFunction value

Usage

ViaDrill[,

<IPC-4761>

]

<IPC-4761>=(Ia|Ib|IIa|IIb|

IIIa|IIIb|IVa|IVb|V|VI|

VII|None)

A via hole. This is reserved for holes whose sole

function is to connect different layers. It is not to be

used for holes for component leads. No pins will be

pushed in via holes.

An optional field specifies the via protection according

to IPC-4761

BackDrill

A hole to remove plating over a sub-span by drilling that

sub-span with a larger diameter.

ComponentDrill

[,PressFit]

A hole that is used for the attachment and/or electrical

connection of component terminations, including pins

and wires, to a printed board. (Per IPC-T-50).

The optional label PressFit indicates drill holes for press

fit leads. Press fit leads are pressed in properly sized

plated-through holes to realize the electrical contact.

The label can only be applied on PTH holes.

See also ComponentDrill.

SMDPad,(CuDef|SMDef)

A pad belonging to the footprint of an SMD component.

They are pasted or otherwise electrically connected to

the PCB. The purpose of these pads is normally to

connect the component circuitry to the PCB but for

specific components some pads may not connected to

the component inside the package. Excludes BGA pads

which have their own type. This function is valid only for

the normal electrical pads, thermal pads have their own

function; see HeatsinkPad.

The specifier (CuDef|SMDef) is mandatory. CuDef

stands for copper defined; it is by far the most common

SMD pad; the copper pad is completely free of solder

mask; the area to be covered by solder paste is defined

by the copper pad. SMDef stand for solder mask

defined; the solder mask overlaps the copper pad; the

area to be covered by solder paste is defined by the

solder mask opening and not by the copper pad.

(CuDef is sometimes rather awkwardly called non

solder mask defined.)

Only applicable for outer layers.

When an SMD pad contains a via hole the pad where

the SMD is soldered, on the outer layer with the SMD,

is SMDPad, all other pads in the stack are ViaPad. If

the SMD pad contains an embedded via pad, as it

should, then that embedded pad is of course ViaPad.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

BGAPad,(CuDef|SMDef)

A pad belonging to the footprint of an BGA component.

They are soldered or otherwise electrically connected to

the PCB. The purpose of these pads is normally to

connect the component circuitry to the PCB but for

specific components some pads may not connected to

the component inside the package.

The specifier (CuDef|SMDef) is mandatory. CuDef

stands for copper defined, SMDef for solder mask

defined; see SMDPad.

Only applicable for outer layers.

When a BGA pad contains a via hole the pad where the

BGA is soldered is BGAPad, all other pads in the stack

are ViaPad. If the BGA pad contains an embedded via

pad, as it should, then that embedded pad is of course

ViaPad.

ConnectorPad

An edge connector pad.

Only applicable for outer layers.

HeatsinkPad

Heat sink or thermal pad, typically for SMDs

ViaPad

A via pad. It provides a ring to attach the plating in the

barrel. This is reserved for pads that have no other

function than making the connection between layers:

Component pads often also have a via function;

however their main function is component pad and they

must have this function; similar for test pads, via in BGA

etc.

TestPad

A test pad. Only applicable for outer layers.

Sometimes a test pad is drilled and also has a via

function, to save space. Such a pad must be specified

as test pad. (It is clear from the construction that it has

a via function, but the fabricator must know it is a test

pad, and this is not obvious. Similarly, a component pad

can also function as a via, but it remains a component

pad.)

CastellatedPad

Pads on plated holes cut- through by the board edge;

used to join PCBs.

Image courtesy Eurocircuits.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

FiducialPad

,(Local|Global|Panel)

A fiducial pad.

The specifier (Local|GlobalPanel) is mandatory. Local

fiducials pads are used to locate the position of an

individual component, global to locate a single PCB,

and Panel to locate a panel.

ThermalReliefPad

A thermal relief pad connected to the surrounding

copper while restricting heat flow.

WasherPad

A pad around a non-plated hole without electrical

function. Several applications, e.g. a pad that

strengthens the PCB where fixed with a bolt – hence

the name washer.

AntiPad

A pad with clearing polarity (LPC) creating a clearance

in a plane. It makes room for a drill pass without

connecting to the plane. Note that setting the AntiPad

attribute itself has no effect on the image, and therefore

does not turn the pad into LPC as a side effect– this

must be done explicitly by an %LPC*% command.

OtherPad,<mandatory field>

A pad not specified above. The mandatory field

informally describes the type.

Conductor

Copper whose function is to connect pads or to provide

shielding, typically tracks and copper pours such as

power and ground planes. Note that conductive copper

pours should carry this attribute, whether made properly

by a region statement or by painting – see Regions.

(Note that painting is poor practice, but if you have to

paint, at least add the attribute so that it is clear what

the tangle of draws mean.)

EtchedComponent

Etched components are embedded inductors,

transformers and capacitors which are etched into the

PCB copper. The following illustration shows two

etched inductors:

For the CAD netlist these are components like others:

the net names are different on both sides. (However, for

bare-board electrical test they may be conducting

copper and connect the net on both sides.)

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

NonConductor

Copper that does not serve as a conductor, that has no

electrical function; typically text in the PCB such as a

part number and version. Not that this attribute can

only be applied to copper, not to drawing elements in a

copper layer; see also NonMaterial and Profile.

CopperBalancing

Copper pattern added to balance copper coverage for

the plating process.

Border

The copper border of a production panel.

OtherCopper,<mandatory

field>

Indicates another function. The mandatory field

informally describes the type.

The values in All layers

can also be used

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Component Layers

.AperFunction value

Usage

ComponentMain

This aperture is flashed at the centroid of a component.

The flash carries the object attributes with the main

characteristics of the component.

The following aperture must be used:

%ADDnnC,0.300*% (mm)

%ADDnnC,0.012*% (in)

nn is an aperture number, an integer ≥ 10.

ComponentOutline,<type>

<type>=(Body|Lead2Lead|

Footprint|Courtyard)

This attribute is used to draw the outline of the component.

An outline is a sequence of connected draws and arcs.

They are said to connect only if they are defined

consecutively, with the second starting where the first one

ends. Thus, the order in which they are defined is

significant. A contour is closed: the end point of the last

draw/arc must coincide with the start point of the first.

Outlines cannot self-intersect.

Four different types of outlines are defined. See drawing,

courtesy Thiadmer Riemersma:

Outlines of different types on the same component are

allowed. The following aperture must be used:

%ADDnnC,0.100*% (mm)

%ADDnnC,0.004*% (in)

ComponentPin

The coordinates in the flash command (D03) indicate the

location of the component pins (leads). The .P object

attribute must be attached to each flash to identify the

reference descriptor and pin.

For the key pin, typically pin "1" or "A1", the following

diamond shape aperture must be used:

%ADDnnP,0.360X4X0.0*% (mm)

%ADDnnP,0.017X4X0.0*% (in)

The key pin is then visible in the image.

For all other pins the following zero size aperture must be

used:

%ADDnnC,0*%...(both mm and in)

These pins are not visible which avoids cluttering the

image.

The values in All layers

can also be used

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

All layers

The values in this table can be used on all layers, including plated, non-plated and copper.

.AperFunction value

Usage

Profile

Identifies the draws and arcs that exactly define the

profile or outline of the PCB. This is the content of the

Profile file but can also be present in other layers. See

6.5

NonMaterial

The attribute value NonMaterial identifies objects that do

not represent physical material but drawing elements.

NonMaterial is only meaningful on files that define the

pattern of physical layers of a PCB such as copper layers

or solder mask. Such files unfortunately sometimes not

only contain data representing material but also drawing

elements such as a frame and a title block. (Note:

drawing elements should not be mixed with pattern data,

all, see 6.6.1.2. Use drawing files for drawings.).

Material

Identifies the proper part of the data file.

Solder masks are traditionally negative. The image

represents the solder mask openings. The apertures take

the value ‘Material’ – they define solder mask material,

but in a negative way.

For copper and drill layers Material is split into more

specific functions such as SMD pad. Use the specific

functions when available rather than ‘Material’.

Other,<mandatory field>

The value ‘Other’ is to be used if none of the values

above fits. By putting the value ‘Other’ rather than crudely

omitting the attribute it is made explicit that the value is

none of the above – an omitted attribute can be one of

the above. Certainly do not abuse existing values by

horseshoeing an attribute with a vaguely similar function

into that value that does not fit perfectly – keep the

identification clean by using ‘Other’.

The mandatory field informally describes the aperture

function.

.AperFunction aperture attribute values

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Functions on extra layers. The solder mask, paste and other extra layers openings cannot

take the pad values. Pad values are reserved for outer copper layers. The solder mask

openings and paste pads take their function from the underlying copper pads. The reason for

this is that a single solder mask opening may have multiple underlying copper pads – e.g. an

SMP pad with an embedded via pad - and hence multiple functions.

Consequently, solder mask openings have the aperture function ‘Material’. Admittedly this is

somewhat a misnomer in this context as solder masks are usually negative, and the presence

of image indicates therefore the absence of material; this has nothing to do with the pad

functions but with the layer being negative.

The following file creates a circular hole in the solder mask. In negative file polarity the image

represents the absence of material.

%FSLAX36Y36*%

%MOMM*%

%TF.FileFunction,Soldermask,Top*%

%TF.Part,Single*%

%TF.FilePolarity,Negative*%

%TA.AperFunction,Material*%

%ADD10C,2.54*%

%LPD*%

D10*

X123500000Y12500D0003*

...

M02*

If the file polarity is positive an otherwise identical file creates a circle consisting of solder mask.

%FSLAX36Y36*%

%MOMM*%

%TF.FileFunction,Soldermask,Top*%

%TF.Part,Single*%

%TF.FilePolarity,Positive*%

%TA.AperFunction,Material*%

%ADD10C,2.54*%

%LPD*%

D10*

X123500000Y125000000D03*

...

M02*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

.DrillTolerance

.DrillTolerance defines the plus and minus tolerance of a drill hole end diameter. Both values

are positive decimals expressed in the MO units. The attribute value has the following syntax:

Examples:

%TA.DrillTolerance,0.01,0.005*%

.FlashText

Gerber intentionally does not contain fonts or typographic text – this would introduce a

complexity out of proportion to its benefits. Any text can be represented with the available

graphic constructs, especially with contours. However, such generic graphic constructs do not

maintain the information which text string is represented; this is sometimes a disadvantage.

The .FlashText aperture attribute transfers this otherwise lost information. .FlashText is

designed for text image created with a flash. If the text is created with draws and arcs rather

than a flash, it can always be flashed by collecting them in a block aperture.

Bar codes are handled as text – one can view a barcode as a special font.

The syntax and semantic of the attribute value is as follows:

<Text>,(B|C),[(R|M)],[],[Size],[<Comment>]

.FlashText fields

Usage

<text>

The text string represented by the aperture image.

(B|C)

Indicates if the text is represented by a barcode – B -or

by characters - C.

(R|M)

Indicates if the text is readable or mirrored left-right .

Optional.

Font name. Content not standardized. Optional.

<Size>

Font size. Content not standardized. Optional.

Any extra information one wants to add. Optional.

An empty field means that the corresponding meta-data is not specified.

Examples:

%TA.FlashText,L1,C,R,Courier,10,Layer number (L1 is top)*%

Text: L1

B|C: Characters,

(R|M): Readable

Font: Courier

Size: 10

Comment: Layer number (L1 is top)

%TA.FlashText,XZ12ADF,B,,Code128,,Project identifier *%

Text: XZ12ADF

B|C: Barcode

(R|M) Not specified

Font: Code128

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Size: Not specified

Comment: Project identifier

.N (Net)

The .N object attribute attaches a CAD netlist name to any conducting object. The attribute can

be attached to objects on any copper layer or plated drill/rout file. It indicates the object is part of

the given net. The .N attribute is intended to allow quick visualization of nets and, more

importantly, to define the CAD netlist.

The syntax is:

<.N Attribute> = .N,<netname>{,<netname>}

.N field

Usage

The CAD net name. It can take any value conforming to

the field syntax.

Example:

%TA.aperFunction,Conductor*%

%ADD21C,1*% Create aperture 21, for conductive tracks

…

D21* Select aperture 21

%TO.N,Clk3*% Select net Clk3

X5600000Y1200000D02* Move to the start of a track

X5600000Y1202500D01* Draw the tracks with Clk3 is attached

X5605000Y1205000D01*

X5605000Y1220000D01*

…

There are two reserved net names:

1) The empty string, defined by

%TO.N,*% identifies objects not connected to a net, such as

tooling holes, text, logos, pads for component leads not connected to the component

circuitry.

2) The name N/C, defined by

%TO.N,N/C*%, identifies a single pad net, as an alternative to

giving each such net a unique name.

Except the reserved names all net names must be unique.

It is recommended to attach a .N attribute to all copper objects, also those without net. The

absence of the .N attribute does not mean there is no net and is therefore ambiguous.

Normally an object is fully connected and consequently belongs to a single net. However, if an

object consists of different disconnected parts or is split in several disconnected parts by clear

(LPC) objects it may belong to different nets. Then the .N attribute value must include all net

names involved. It is recommended to avoid creating disconnected objects: one object, one net.

5.6.13.1 Etched Components

Etched components are embedded inductors, transformers and capacitors which are etched

into the PCB copper. The following illustration shows two etched inductors.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

They are identified by the .AperFunction attribute value ‘EtchedComponent’ on to the aperture

used to create them. See

EtchedComponent.

For the CAD netlist these are components like others: the net names are different on both sides.

(However, for bare-board electrical test they may be conducting copper and simply connect the

nets on both sides.)

Etched components do not need and normally do not have pads. There is no .P associated with

them. The net on each side is different however.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

.P (Pin)

The .P object attribute attaches the reference descriptor and pin number of a component pin to

a pad on an outer copper layer or a ComponentPin in a component layer. The syntax is:

<.P Attribute> = .P,<refdes>,<number>[,<function>]

.P fields

Usage

The component reference descriptor. It can take any

value conforming to the field syntax.

The pin number. It can take any value conforming to

the field syntax. It is normally simply a number.

The pin function. It can take any value conforming to

the field syntax. It is strongly recommended to include

both pin number and pin function. The pin function is

less prone to error than the pin number, and the

redundancy provides extra security This is especially

important for diodes and transistors.

Example, for netlist only:

D13* Select aperture 13 for the pads for R5

%TO.P,R5,1*%

X5600000Y1200000D03* The pad for R5, pin 1

%TO.P,R5,2*%

X5600000Y1202500D03* The pad for R5, pin 2

Example, with pin function:

Take the following integrated circuit:

The pin attributes could be as follows:

D13* Select aperture 13 for the pads for IC12

%TO.P,IC12,1,GND*%

X5600000Y1200000D03*

%TO.P,IC12,2,TRIG*%

X5600000Y1202500D03*

…

The .P attribute can be attached to any pad belonging to a component, and only those. The pin

number must be a non-empty field, with one exception: if the pad is part of the component

footprint but not connected to the component circuitry the name may be an empty field, e.g.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

defined by %TO.P,U3,*%; pads with an empty name are normally not part of a net and

therefore also have an empty net name attached defined by

%TO.N,*%.

Consequently, it can only be used in copper layers that carry the components. Typically, these

are the outer layers and then the .P attribute can only be used in the outer layers. Embedded or

etched components can be on inner layers and then these inner layers can also carry the .P

attribute.

A single component pad can consist of multiple flashes. Each flash then carries the same

reference descriptor and pin number.

It is technically possible to create a single object representing multiple pads. For example, a

single macro aperture can describe a complete component footprint. This is possible but not

allowed. (It would be a neat way to make life miserable for CAM engineers though.)

The .P attribute can be attached to flashed pads only, not to painted pads.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

.C (Component)

The .C object attribute attaches the component reference to an object. It indicates that the

object belongs to the given component. The attribute can be attached to objects on any layer. It

is intended to identify e.g. which objects on a legend belong to which components.

The syntax is:

<.C Attribute> = .C,<refdes>

.C field

Usage

The component reference descriptor. It can take any

value conforming to the field syntax.

Example in a legend layer:

D21* Select aperture 21, used for component symbols

%TO.C,R2*%

Select reference descriptor R2

X5600000Y1200000D02*

Move to the start of the symbol

X5600000Y1202500D01*

Draw the symbol

X5605000Y1205000D01*

X5605000Y1220000D01*

…

The attribute .C,R2 is attached to all tracks drawing the resistor symbol.

5.6.15.1 Component Characteristics

These attributes can be attached to the component objects in component layers. They provide

information needed for assembly.

Object attributes

Usage

.CRot,<decimal>

The rotation angle of the component.

The rotation angle is consistent with the one for

graphical objects. Positive rotation is counterclockwise

viewed from the top side, even if the component is on

the bottom side. The zero-rotation orientation of a top

side component as in IPC-7351. The base orientation of

a bottom side component is the one on the top side,

mirrored around the X axis.

.CMfr,<field>

Manufacturer

.CMPN,<field>

Manufacturer part number

.CVal,<field>

Value, e.g. 220nF

.CMnt,(TH|SMD|Fiducial|Other)

Mount type

.CFtp,<field>

Footprint name

.CPgN,<field>

Package name

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

.CPgD,<field>

Package description

.CHgt,<decimal>

Height, in the unit of the file.

.CLbN,<field>

Name of the component library from where the

component information originates

.CLbD,<field>

Description of the component library from where the

component information originates

.CSup,<SN>,<SPN>,{<SN>,<SPN>}

<SN> is a field with the supplier name. <SPN> is a field

with a supplier part name

All ComponentMain and ComponentOutline objects must have a .C object attribute. The

<RefDes> value for each component should be unique, since it links the ComponentOutline

objects to their ComponentMain object. The other .Cxxx attributes are only valid for

ComponentMain objects. If attached to other objects, they are ignored.

5.7 Text in the Image

Gerber has no native font support – this adds too much complication in relation to the modest

text requirements in PCB fabrication data. Text must be represented as pure image data, best

as regions (contours), see 4.10.

Font definitions often contain splines and Gerber does has linear and circular segments but no

splines. The splines must therefore be approximated to either linear or circular segments.

Circular is more precise with less objects than linear, but mathematically more complicated.

An issue with representing text as image is that the information is lost that this image is text, and

which string it represents. This is easily solved with the attributes .AperFunction (5.6.4.1) and

.FlashText (5.6.4.3). (It may be counterintuitive, but these aperture attributes can be associated

with regions; see 5.3, attributes on regions.) An example; suppose one needs to add the text

‘Intercept’ on the bottom copper layer. Here is how it goes:

%TA.AperFunction,NonConductor*% <- Indicates the copper is not a conductor,

typically text and graphics

%TA.Flashtext,Intercept,C,M*% <- Indicates the copper represents the string

‘Intercept’, as characters and mirrored

G36*

…

<- Draws creating the contours

G37*

%TD.AperFunction*%

<- Deletes the attribute

%TD.FlashText*%

<- Deletes the attribute

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

5.8 Examples

The example below shows the usage of a simple aperture attribute.

Example:

G01*

%ADD13R,200X200*% G04 this aperture has no attribute*

D13*

%TAIAmATA*% G04 add attribute IAmATA in attributes

dictionary*

X0Y0D03* G04 this flash object has no attribute*

%ADD11R,200X200*% G04 this aperture now has attached attribute

IAmATA*

%TDIAmATA*% G04 delete attribute IAmATA from current

attributes dictionary*

%ADD12C,5*% G04 this aperture does not have attribute IAmATA*

D11*

X100Y0D03* G04 this flash object has attribute IAmATA*

X150Y50D02*

D12*

X100Y150D01* G04 this draw object has no attribute*

The next example illustrates an aperture attribute definition and changing value.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Example:

G01*

%TA.AperFunction,SMDPad*% G04 Adds attribute .AperFunction in the

current dictionary with value SMDPad to

identify SMD pads*

%ADD11…*% G04 Aperture with number 11 gets the

.AperFunction,SMDPad attribute attached*

%TA.AperFunction,Conductor*% G04 Changes the value of .AperFunction

attribute to define conductors*

%ADD20…*% G04 Aperture with number 20 gets the

.AperFunction,Conductor attribute attached*

%TACustAttr,val*% G04 Adds attribute CustAttr in the current

attributes dictionary and sets its value to

val*

%ADD21…*% G04 Aperture with number 21 is a conductor

with attached attribute CustAttr = val*

%TD.AperFunction*% G04 Deletes the .AperFunction attribute from

the attributes dictionary*

%ADD22…*% G04 Aperture with number 22 has no attached

.AperFunction attribute, but has attribute

CustAttr = val*

%TDCustAttr *% G04 Deletes the CustAttr attribute from the

attributes dictionary*

%ADD23…*% G04 Aperture with number 23 has no attached

aperture attributes*

…

D11* G04 Set current aperture to aperture 11*

X1000Y1000D03* G04 Flash an SMD pad*

D20* G04 Use aperture 20 for graphical objects &

attach it to regions*

X2000Y1500D01* G04 Draw a conductor*

%TA.AperFunction,Conductor*% G04 Changes the value of .AperFunction

attribute to define conductors*

G36* G04 Start a conductive region. IT TAKES ON

THE ATTRIBUTE VALUES FROM THE DICTIONARY*

….

G37*

%TD*% G04 Clear attribute dictionary*

G36* G04 Start a region, without attributes*

….

G37*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

6 PCB Fabrication and Assembly Data

6.1 Structure

PCB Fabrication data is a set of Gerber files and possibly files in other portable formats such as

PDF. The files can either be in a directory or combined in a zip file. Other archive formats such

as rar, 7z are not allowed.

6.2 Mandatory Attributes

A single Gerber file defines a single 2D layer image. A PCB, however, is a 3D object. To define

a PCB one must not only define each layer, but also its position in the layer structure. What a

layer does in the layer structure is defined by the file attributes .FileFunction and .FilePolarity.

These two attributes are therefore mandatory in PCB fabrication data.

6.3 Alignment

All data files in a fabrication data set must align – same offset, no mirroring, seen from the top to

bottom. Data must of course not be scaled, but one to one.

6.4 Pads

The fabricators must be able to distinguish between pads and other copper. For example, SMD

pads often have stricter tolerances than other copper, pads are the test points for electrical test,

and pads must be clear of legend. To identify pads all pads must be flashed (D03), and all

flashes must be pads. Pads embedded in copper pours must also be flashed, although the flash

does not affect the image – its purpose is to transfer information, namely the location and shape

of the pad.

6.5 The Profile

The profile defines the physical extent of the PCB in a machine-readable manner.

A fabrication data set must contain a separate file with the profile. Other layers may contain a

replica of that outline.

Ideally the outline is represented by a contour (G36/G37). However, often the outline is defined

by draws and arcs with a zero-size or small aperture. This is a valid alternative if the draws and

arcs form a cleanly connected closed path, obeying the same rules as for contour segments

(see 4.10.3). In case if a non-zero aperture the center line must represent the outline.

A roughly drawn outline, where lines do not connect cleanly, is not good enough. Corner marks

are not good enough as they are only suitable for manual processing. Fabrication drawings can

and should contain an outline drawing, but that is not a substitute for machine readable data,

just as a drill map is not a substitute for drill data.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

6.6 Drill/rout files

The image represents which material to remove. This specification does not differentiate

between drilling and routing: the fabricator will determine what to drill and what to rout.

A drill rout file can only use the circular aperture. Rectangle, obround, polygon and macro are

not allowed. Only the following constructs can be used.

• For drill holes: flashes with a circular aperture.

• For slots: draws and arcs with a circular aperture; it can be a single draw/arc or a non-

closed chain of draw/arcs

• For milling (openings with a general shape): use the region (G36/G37)

The drill/rout file image represents the end diameter of the hole; this is the diameter after

plating, also known as the inner diameter.

Each drill span (from-to layers) must be put in a separate Gerber file. PTH and NPTH must be

split in two separate files.

Note: In fabrication data Gerber is more suitable to transfer drill/rout format than the NC

formats, and mixing formats is asking for problems in registration and accuracy. It is the same

format as for the copper, mask, legend etc. It is much more precisely defined. It can contain

attributes. The objection is sometimes raised that a Gerber file cannot be sent to a drill machine.

While this is true, it is irrelevant in fabrication data. No fabricator uses his client’s incoming

design files directly on his equipment. The design files are always read in a CAM system, and it

is the CAM system that will output drill files in the appropriate NC format, including feeds and

speeds and all the information exactly as needed by the driller.

6.6.1.1 Backdrilling

An example explains best how to structure a job with backdrilling. Suppose we have an 8 layer

job with backdrilling to remove via plating between layers 8 and 7. We need two files:

One file contains the via’s. It has .FileFunction Plated,1,8,PTH. The drill tool has the via end

diameter. Its .AperFunction value is Via.

The second file contains the backdrills. It has .FileFunction NonPlated,8,7,Blind. The drill tool

has the same diameter as the via – the manufacturer will determine the tool diameter. Its

.AperFunction value is Backdrill.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

6.6.1.2 Example Drill File

47. Example: drill file

Syntax

Annotation

%FSLAX36Y36*%

Format specification:

Leading zero’s omitted

Absolute coordinates

3 integer and 6 fractional digits

%MOMM*%

Unit is mm

%TF.FileFunction,Plated,1,8,PTH*%

This file describes plated-through holes

%TF.Polarity,Positive*%

Always positive polarity for drill files

%TF.Part,Single*%

This file is part of a single PCB

%TA.DrillTolerance,0.02,0.01*%

Set the drill tolerance attribute to 0.02 mm in

plus and 0.01 mm in minus in the attribute

dictionary. It will be attached to all aperture

definitions until changed or deleted

%TA.AperFunction,ComponentDrill*%

Attribute indicates that the following apertures

define component drill holes.

%ADD10C,0.14000*%

Define the aperture to create holes with 0.14 mm

end diameter. The AD command picks up the

attributes in the attribute dictionary, which

defines the as a component hole, with a 0.02

mm positive and 0.01 mm negative tolerance.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

%TA.AperFunction,Other,Special*%

Attribute indicates that the following apertures

are special drill holes

%ADD11C,0.24000*%

Define the aperture: a plated hole for a special

purpose, with 0.24 mm end diameter with a

tolerance of +0.02 mm and -0.01mm.

%TA.DrillTolerance,0.15,0.15*%

Changes the drill tolerance attribute for the

following apertures to 0.15 mm in both directions

%TA.AperFunction,MechanicalDrill*%

Change the tool function attribute in the

dictionary to mechanical

%ADD12C,0.43000*%

Define aperture 12 as a plated mechanical drill

tool with 0.43 mm end diameter, and a tolerance

of 0.15 mm in both directions.

%ADD13C,0.22000*%

Define aperture12, a tool with the same

attributes but an end diameter of 0.22 mm

%TD.AperFunction*%

Remove the .AperFunction aperture attribute

from the attributes dictionary

%TD.DrillTolerance*%

Remove the .DrillTolerance aperture attribute

from the attributes dictionary

G01*

Set linear interpolation mode

D10*

Set aperture 10 as the current aperture.

X2420000Y2750000D03*

Create flash graphical objects with aperture 10: drill

plated component holes with diameter 0.14 mm

at the indicated coordinates

Y3250000D03*

X2170000Y3000000D03*

X1920000Y3250000D03*

X2920000Y2750000D03*

X1920000D03*

X2920000Y3250000D03*

X2670000Y3000000D03*

D11*

Set the current aperture to drill tool 11

X1240000Y0D03*

Create flash graphical objects with aperture 11: drill

plated special drill holes with diameter 0.24 mm

at the indicated coordinates

X0Y-1240000D03*

X-1240000Y0D03*

X880000Y880000D03*

X-880000D03*

X0Y1240000D03*

X880000Y-880000D03*

X-880000D03*

D12*

Set the current aperture to drill tool 12

X7920000Y3500000D03*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

X4920000Y-3500000D03*

Create flash graphical objects with aperture D12: drill

plated mechanical drill holes with diameter 0.43

mm at the indicated coordinates

D13*

Set the current aperture to drill tool 13

X7670000Y-6000000D03*

Create flash graphical objects with aperture D13: drill

plated mechanical drill holes with diameter 0.22

mm at the indicated coordinates

X5670000D03*

X-2330000Y2000000D03*

Y4000000D03*

Y0D03*

Y-2000000D03*

Y-6000000D03*

Y-4000000D03*

X-330000Y-6000000D03*

X1670000D03*

X3670000D03*

M02*

End of file

Some will be surprised to see drill and rout files in the Gerber format. And indeed, one cannot

send a Gerber file to a drilling machine. However, this is not the purpose here. The purpose is

to transfer the design information from CAD to CAM and for that Gerber is the best format,

because of its consistency with the copper layer data, its rigorous specification, its metadata.

Gerber is a format to transfer design information, whereas the often-used NC formats are

indeed nothing more than primitive NC control formats. For more information, see 5.6.2.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

6.7 Drawings and Data

Gerber files in PCB fabrication data contains two types of images.

• Drawings, such as a drill map, a fabrication drawing or an assembly drawing. Such

images are intended to be looked at by humans, and may contain vital fabrication

instructions.

• Digital data representing the patterns of the copper, the solder mask, legend, drills. This

digital data is intended to be processed by CAM software.

Unfortunately, the two are sometimes mixed, and drawing elements added to copper files etc.

as in the example below.

48. Confusing a drawing and digital data

Such a file is no longer machine readable. An operator must first manually remove the drawing

elements. Before doing so he must check if these elements do not contain vital information and

write this down somewhere for future reference. Keep data files pure. The drawings must

contain all information that belongs to drawing. If need be, information that belongs to a specific

file can be put in attributes. Less manual work, less risk of error. Simpler and cleaner.

6.8 The CAD Netlist

The CAD netlist describes which component pins are connected. Pins are identified by their

component reference descriptor and pin number or name. Nets are identified by the net name.

Here is an example of a CAD netlist; The first line lists all pins of net Clk3.

Clk3: U1-4,U2-3,U5-9,U6-9,U7-9

Sig11: U1-3,U5-12

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Data8: U2-4,U5-10,U6-10,U7-8,U8-1

GND: U1-1,U2-1,U3-8,U4-16,U5-16,U6-1,U7-8,U8-8

…

The CAD netlist links component pads to nets. It specifies the function of the PCB and is the

basis for the layout.

In Gerber the CAD netlist is defined by attaching both the pin and the net attribute to each

component pad. This defines a pad – net entry in the CAD netlist, and at the same time

associates a pad location and shape to it. For instance, the first entry in the CAD netlist above is

given by the following sequence:

%TO.P,U1,4*%

%TO.N,Clk3*%

X…Y…D03* The flash that creates the pad

…

It is recommended to add .P attribute to all electrical end points, not only physical component

leads but edge connectors and test points. Although vias are part of a net, they are not

component pads and cannot have a .P attached. Washer pads or any pads that are not part of a

component cannot have a .P attached.

6.8.1.1 Benefits of Including the CAD Netlist.

For the assembly process the location and orientation of each component must be known. This

can easily be extracted from the Gerber file.

The netlist and component names facilitate the communication between the parties involved in

design and fabrication. Viewers show more complete PCB information.

More importantly, the netlist information dramatically increases the security of the design to

fabrication data transfer. If the image CAM reads from a Gerber file significantly differs from the

image intended by CAD, due to bugs, operator errors or transmission errors, the inevitable

result is scrap. Such a difference in image results in a difference in board netlist, which can be

detected by comparing the calculated board netlist with the supplied CAD netlist. The CAD

netlist therefore provides a very powerful redundancy check against image errors. To be

precise, the following assert must be valid:

- Interpret all N/C’s as unique names

- Flashes with the same reference descriptor and pad are deemed connected

- Etched components are removed before connection is calculated

- Assert 1: pads with the same net name must be connected

- Assert 2: pads with different net names must be isolated.

Lastly, a bare board PCB fabricator is expected to perform an electrical test on the bare PCB

and guarantee the PCB conforms to the CAD netlist. It then is logical to provide him with the

netlist to test against. Without providing the netlist the fabricator is expected to reverse engineer

the netlist and must test against a reverse engineered net – hardly a secure procedure.

6.8.1.2 IP Considerations

Net names such as Clk13 provide information about the design. This may be a concern. A

solution is to replace the meaningful names with obfuscated names such a sequential number.

This still allows to compare the design netlist with the image netlist as a redundancy check –

meaningful names are not needed for that. The obfuscated names are a little less convenient

when communicating between creator and receiver of the Gerber file, but both can still identify

the same net as long as the creator can identify the net corresponding to the obfuscated name

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

he created. Obfuscated names are sometimes a sensible balance between IP protection and

data transfer security.

It is sometimes alleged that even a net list with obfuscated names pose an IP security risk as it

still shows the connections between the pads. This is an obvious fallacy as the connections

between the pads can be worked out from the image. In fact, if this were not true, a fabricator

would be unable to perform a bare board electrical test without netlist information.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

6.9 PCB Assembly Data

6.9.1.1 Overview

The purpose of the component layers in Gerber data is to transfer the component information

held in CAD which is needed in manufacturing to:

• visualize the component placement to check for errors and set up the assembly,

• generate the manufacturing tools, such as the paste stencils and the pick and place

machine programs,

• assist in the procurement of the components.

Component information is all too often transferred as separate, non-standardized drawings, pick

& place and BOM files. The component layers transfer this in a standardized, unequivocal and

machine-readable manner. Component location is geometrical data: the centroid, outline,

fiducial locations and the footprints; geometric data fits naturally in a Gerber image file.

Combining bare board and component data in Gerber files allows a holistic review of the final

board.

The intended workflow is that the CAD Gerber output data is read into an assembly CAM

system, which analyzes the incoming data, allows for visual inspection and generates the

outputs tuned to the specific assembly equipment.

The scope of this specification is intentionally limited to technical product information of a single

physical PCB. It is not mixed with commercial information such as order quantities – the same

physical PCB can be ordered or sold under different commercial terms, and this must not affect

the product model.

It is natural to put the components in two new Gerber files: the top and bottom component file.

By placing the component data in separate files, full compatibility is maintained: if one does not

like the new files, simply ignore them. The new standard is therefore compatible with existing

workflows. Legacy software handles the CAD data with the new assembly information without

change, of course also without benefiting from it. Great care is taken to minimize the

development effort by keeping the existing fabrication outputs in place and sticking to an

existing syntax. Benefits:

o Compatible with installed base

o Minimal implementation work.

o Any decent legacy viewer displays the new component layers.

6.9.1.2 Assembly Data Set

To transfer component information one can simply add component layers to the full bare board

fabrication data set. This may raise concerns about the confidentiality of the design. As inner

layer information is not needed for assembly one can omit the inner layers; the data does then

not implicitly contain the netlist. As an example, a typical data set for a four-layer board is:

%TF.FileFunction,Component,L1,Top*%

%TF.FileFunction,Legend,Top*%

%TF.FileFunction,Soldermask,Top*%

%TF.FileFunction,Copper,L1,Top*%

%TF.FileFunction,Copper,L4,Bot*%

%TF.FileFunction,Soldermask,Bot*%

%TF.FileFunction,Legend,Bot*%

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

%TF.FileFunction,Component,L4,Bot*%

%TF.FileFunction,Plated,1,4,PTH*%

%TF.FileFunction,NonPlated,1,4,NPTH*% (If there are NPTH.)

The top and bottom component layers specify component information needed for the assembly

process. A set of attributes identify each component's location, orientation, identification, and its

properties such as manufacturer part number. The outer copper layers, mask, legend and drill

layers serve to verify component placement and provide registration information for pick-and-

place machines. An assembly drawing can contain useful information not in the component

layers.

The pin locations are included in the component layer to unequivocally specify location and

rotation of the components, with the aperture function ComponentPin and .P attribute. The .P

attribute is mandatory for each ComponentPin flash. Any .Cxxx attributes attached to a pin are

ignored.

The component layer can include fiducials. If they are added a zero-size aperture must be used,

with .AperFunction value the existing value FiducialPad,Local, and object attribute .C to identify

the component.

6.9.1.3 Annotated Example Component Layer

Commands Annotation

%TF.GenerationSoftware,KiCad,Pcbnew,(5.99.0-

190-g0fd48dd4f-dirty)*%

%TF.CreationDate,2019-10-02T18:52:55+02:00*%

%TF.ProjectId,kit-dev-coldfire-

xilinx_5213,6b69742d-6465-4762-9d63-

6f6c64666972,2*%

%TF.SameCoordinates,PX3e22018PY8d89728*%

%TF.FileFunction,Component,L1,Top*%

This file is the top

component layer

%TF.FilePolarity,Positive*%

%FSLAX46Y46*%

%MOMM*%

%LPD*%

G04 Aperture begin list*

%TA.AperFunction,ComponentMain*%

%ADD10C,0.3*%

The aperture for the flash

with the main component

information

%TA.AperFunction,ComponentOutline,Courtyard*%

%ADD11C,0.1*%

The aperture to draw the

outline

%TA.AperFunction,ComponentPin*%

%ADD12P,0.36X4X0.0*%

The aperture to flash the

pin 1 location

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Commands Annotation

%ADD13C,0*%

The aperture for the other

pin locations

%TD*%

G04 Aperture end list*

G04 Begin component info*

D10*

Select main component

aperture

%TO.C,R301*%

Attach reference descriptor

R301

%TO.CFtp,R_0805_2012Metric*%

Attach footprint

%TO.CVal,4K7*%

Attach value

%TO.CMnt,SMD*%

Attach mount type

%TO.CRot,-90*%

Attach rotation

X218250000Y-73000000D03*

Flash at reference point

D11*

Select outline aperture

X219250000Y-71310000D02*

Draw outline

X217250000Y-71310000D01*

Draw outline

X217250000Y-74690000D01*

Draw outline

X219250000Y-74690000D01*

Draw outline

X219250000Y-71310000D01*

Draw outline

D12*

Select key pin aperture

%TO.P,R301,1*%

Attach ref. desc and pin

number

X218250000Y-72045000D03*

Flash at key pin location

D13*

Select subsequent pin

aperture

%TO.P,R301,2*%

Attach pin 2 ident

X218250000Y-73955000D03*

Flash at key pin location

%TD*%

Clear attributes before next

component

G04 Next component*

…

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

7 Errors and Bad Practices

7.1 Errors

Poor implementation of the Gerber format can give rise to invalid Gerber files or – worse – valid

Gerber files that do not represent the intended image. The table below lists the most common

errors.

Symptom

Cause and Correct Usage

Standard Gerber or RS-274-D Standard Gerber is revoked and is therefore no

longer valid Gerber. It was designed for a

workflow that is as obsolete as the mechanical

typewriter. It requires manual interpretation and

is therefore error-prone. Do not use it. See 8.5.

Always use Gerber X!

Clearances in planes disappear. This is often the consequence of invalid cut-ins

resulting in self-

intersecting contours. The root

cause is usually sloppy rounding aggravated by

low-resolution output. Use 6 digits precision.

See 4.10.3.

Rotating aperture macros using primitive 21

gives unexpected results.

Some CAD systems incorrectly assume that

primitive 21 rotates around its center. This is

wrong, it rotates around the origin.

See 4.5.1.5.

Unexpected image after an aperture change

or a D03.

Coordinates have been used without an explicit

D01/D02/D03 operation code. This practice is

deprecated because it leads to confusion about

which operation code to use.

Coordinate data must always be combined

with an explicit D01/D02/D03 operation code.

See 8.1.10.

Objects unexpectedly appear or disappear

under holes in standard apertures.

Some CAD systems incorrectly assume the hole

in an aperture clears the underlying image. This

is not so, the hole has no effect on the

underlying image.

See 4.4.6.

Objects unexpectedly appear or disappear

under holes in macro apertures.

Some systems incorrectly assume that

exposure off in a macro aperture clears the

underlying objects under the flash. This is

wrong, exposure off creates a hole in the

aperture and that hole has no effect on the

image.

See 4.5.1.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Polygons are smaller than expected. Some CAD syst

ems incorrectly assume the

parameter of a Regular Polygon specifies the

inside diameter. This is wrong

: it specifies the

outside diameter.

See 4.4.5.

The result of the MI command is not as

expected.

The MI command mirrors coordinate data but

not apertures. A number of implementations

unfortunately also mirror apertures making MI

unsafe to use. It is therefore deprecated. Do not

use the MI command but apply the

transformation directly in the coordinate data.

See 8.1.7.

The result of the SF command is not as

expected.

The SF command scales coordinate data but no

other sizes in the file. A number of

implementations unfortunately also scale other

elements making SF unsafe to use. It is

therefore deprecated. Do not use the SF

command but apply the transformation directly

in the coordinate data.

See 8.1.9

A single Gerber file contains more than one

image, separated by M00, M01 or M02

This is invalid. A Gerber file can contain only one

image.

One file, one image. One image, one file.

Sending a PCB layer as several

positive/negative files that must be merged

together.

This is invalid in Gerber X. See 2.1. (It was valid

in Standard Gerber but became obsolete with

the introduction of LPD/LPC in Gerber X.) Apart

from being invalid this obnoxious practice

requires manual work and is error prone. One

wonders why someone in his right mind would

use this archaic method, which has a serious

risk of scrap.

One file = one layer

Strange error message. Some files contain the strange pseudo

command %ICAS*%. One wonders what this is

supposed to achieve. Anyhow, it is invalid.

Error message; not the intended image. Invalid format specification %FSD….*%

The only valid zero omission options in the %FS

are L and T. D is invalid. See 8.2.1.1.

Strange error message. *Presence of %FSLAN2X26Y26*%

The N2 in the format specification is invalid. See

4.1 One wonders what it is supposed to do.

Strange error message. …X5555Y5555IJ001

Missing zero after the “I”. The number after I

must have at least one digit, see 13.5

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Reported errors

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

7.2 Bad Practices

Some Gerber files are syntactically correct but are needlessly cumbersome or error-prone. The

table below summarizes common poor practices and gives the corresponding good practice.

Bad Practice

Problems

Good Practice

PCB fabrication data sets

without proper profile layer.

The profile is an essential part of

the fabrication data. It must be

accurately defined, in a machine-

readable manner. All too often only

a drawing is provided, or corner

marks, or the profile is only present

merged in copper layers etc.

Always include a

profile layer with a

clean, accurately

constructed profile.

See 6.5

Painted pads (aka stroking or

vector-fill)

See painted copper pours above.

Painting is even more damaging for

pads. as the fabricator needs to

know where the pads are. The only

practical way to identify them is to

use flashes for pads exclusively.

Always use flashed

pads. Define pads,

including SMD pads,

with the AD and AM

commands.

Painted copper pours (aka

stroking or vector-fill)

Painted copper pours produce the

intended image, but the file size

explodes and getting rid of the

painting require time consuming

and error-prone manual work by

CAM operators. Painting was

needed for vector photoplotters in

the 1960s and 1970s, devices now

as outdated as the mechanical

typewriter. There is not a single

reason left to use painting.

Always define

copper pours with

contours (G36/G37)

PCB fabrication data sets

without netlist.

PCB fabrication data is complex

geometric data with an infinite

number of variations. Differences in

the interpretation of image data is

very rare but does happen and then

is costly. A netlist is a powerful

check on the image data – it is akin

to the redundancy checks used in

all data transfer protocols. Omitting

a netlist is omitting a basic security

check.

Always include a

netlist in a PCB

fabrication data set.

A netlist can be

provided in IPC-D-

356A file or with

Gerber attributes –

see 6.8.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Low resolution (numerical

precision)

Poor registration of objects between

PCB layers; loss of accuracy; self-

intersecting contours; invalid arcs;

small arcs turning in full circles,

missing clearances. Poor numerical

accuracy is the main cause for

errors in geometric software. Low

resolution is the root cause for most

problems with Gerber files and

sometimes leads to scrap.

Why would one use low resolution?

To save a few bytes? It is

sometimes argued some Gerber

readers can only handle low

resolutions. This may have been

true in a distant past it no longer is

true now. And anyhow, ask yourself,

will you risk scrap to cater for a few

antiquated implementations?

Use 6 decimals in

mm units. See 4.1

and 8.2.1.

Cutting a single copper pour

in pieces, typically through the

clearances to avoid regions

with holes.

The information what the copper

pour is and where the clearances

are is lost in a tangle of data, made

worse by rounding error. The reader

must attempt to laboriously reverse

engineer the copper pour and

clearances. Risk of scrap.

See section 4.10.5.

Imprecisely positioned arc

center points

An imprecisely positioned center

makes the arc ambiguous and open

to interpretation. This can lead to

unexpected results.

See 4.7.2

Always position arc

center points

precisely.

Pads as contours instead of

flashes

See above. Always use flashed

pads. Define pads,

including SMD pads,

with the AD and AM

commands.

Non-standard file extensions When you use a non-standard file

extension the reader must open the

file to know what format it is and

which application to use.

See 3.5.

Please use “.gbr” or

“.GBR” as file

extension for all

your Gerber files.

Writing files with deprecated

constructs.

Each construct was deprecated for

a reason. Many carry the risk of a

misinterpretation. Continuing to use

deprecated constructs is bad

corporate citizenship as it blocks the

industry from taking the next steps.

Generated files with

current constructs

only. (Note: it is OK

for readers to handle

deprecated constructs

to cater for legacy

files.)

Bad/good practices

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

8 Deprecated Format Elements

8.1 Deprecated Commands

Overview

Current Gerber writers must not use the deprecated commands. Gerber readers may implement

them to support legacy applications and files. The next table lists deprecated commands.

Code

Function

Comments

G54 Select aperture This historic code optionally precedes an aperture

selection Dnn command. It has no effect.

Sometimes used. Deprecated in 2012.

G55 Prepare for flash This historic code optionally precedes D03 code. It

has no effect.

Very rarely used nowadays. Deprecated in 2012.

G70

Set the ‘Unit’ to inch

These historic codes perform a function handled by

the MO command. See 4.2.1.

Sometimes used. Deprecated in 2012

G71 Set the ‘Unit’ to mm

G90 Set the ‘Coordinate format’ to ‘Absolute

notation’

These historic codes perform a function handled by

the FS command. See 4.1.

Very rarely used nowadays. Deprecated in 2012.

G91 Set the ‘Coordinate format’ to ‘Incremental

notation’

M00 Program stop This historic code has the same effect as M02. See

4.13.

Very rarely, if ever, used nowadays. Deprecated in

2012.

M01 Optional stop This historic code has no effect.

Very rarely, if ever, used nowadays. Deprecated in

2012.

IP Sets the ‘Image polarity’ graphics state

parameter

This command has no effect in CAD to CAM

workflows. Sometimes used, and then usually as

%IPPOS*% to confirm the default and then it

then has no effect. As it is not clear how

%IPNEG*% must be handled it is probably a

waste of time to try to fully implement it, and

sufficient to give a warning on a %IPNEG*% and

skip it.

Deprecated in 2013

AS Sets the ‘Axes correspondence’ graphics

state parameter

Deprecated in 2013. Rarely, if ever, used

nowadays.

If used it was nearly always, if not

always, to confirm the default value and then

these commands have no effect.

IR Sets ‘Image rotation’ graphics state

parameter

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

MI Sets ‘Image mirroring’ graphics state

parameter

It is a waste of time to fully implement these

commands. The simplest is simply to ignore these

commands. Theoretically safer is to skip them if

they confirm the default and throw an error on any

other use; chances are you will never see the

error.

Sets ‘Image offset’ graphics state parameter

Sets ‘Scale factor’ graphics state parameter

IN Sets the name of the file image. Has no

effect. It is comment.

This is just a comment. Use G04 for comments.

See 4.1. Ignore it.

Sometimes used. Deprecated in 2013.

LN Loads a name. Has no effect. It is a

comment.

This is just a comment. Use G04 for comments.

See 4.1. Ignore it.

Sometimes used. Deprecated in 2013.

G74 Sets single quadrant mode Rarely used, and then usually to confirm a

default, but without practical effect.

Sometimes used. Deprecated in 2020.

Deprecated Gerber Commands

Axis Select (AS)

The AS command is deprecated since revision I1 from December 2012.

The historic AS command sets the correspondence between the X, Y data axes and the A, B

output device axes. It does not affect the image in computer to computer data exchange. It only

has an effect how the image is positioned on an output device.

The order of execution is always MI, SF, OF, IR and AS, independent of their order of

appearance in the file.

The AS command can only be used once, at the beginning of the file.

8.1.2.1 AS Command

The syntax for the AS command is:

AS = '%' (AS' ('AXBY'|'AYBX')) '*%';

Syntax

Comments

AS for Axis Select

AXBY Assign output device axis A to data axis X, output device axis B to

data axis Y. This is the default.

AYBX Assign output device axis A to data axis Y, output device axis B to

data axis X.

8.1.2.2 Examples

Syntax

Comments

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

%ASAXBY*%

Assign output device axis A to data axis X and output device axis B

to data axis Y

%ASAYBX*%

Assign output device axis A to data axis Y and output device axis B

to data axis X

Image Name (IN)

The IP command is deprecated since revision I4 from October 2013.

The historic IN command gives a name to the image contained in the Gerber file. The name

must comply with the syntax rules for a string as described in section 3.4.3. This command can

only be used once, at the beginning of the file.

IN has no effect on the image. A reader can ignore this command.

The informal information provide by IN can also be put a G04 comment.

8.1.3.1 IN Command

The syntax for the IN command is:

IN = '%' ('IN' name) '*%';

Syntax

Comments

IN for Image Name

<Name>

Image name

8.1.3.2 Examples

Syntax

Comments

%INPANEL_1*%

Image name is ‘PANEL_1’

Image Polarity (IP)

The IP command is deprecated since revision I4 from October 2013.

IP sets positive or negative polarity for the entire image. It can only be used once, at the

beginning of the file.

8.1.4.1 Positive Image Polarity

Under positive image polarity, the image is generated as specified elsewhere in this document.

(In other words, the image generation has been assuming positive image polarity.)

8.1.4.2 Negative Image Polarity

The purpose of negative image polarity is to create a negative image, clear areas in a dark

background. The entire image plane in the background is initially dark instead of clear. The

effect of dark and clear polarity is toggled. The entire image is simply reversed, dark becomes

white and vice versa.

In negative image polarity, the first graphical object encountered must have dark polarity.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

8.1.4.3 IP Command

The syntax for the IP command is:

IP = '%' ('IP' ('POS'|'NEG')) '*%';

Syntax

Comments

IP for Image Polarity

POS

Image has positive polarity

NEG

Image has negative polarity

8.1.4.4 Examples

Syntax

Comments

%IPPOS*%

Image has positive polarity

%IPNEG*%

Image has negative polarity

Image Rotation (IR)

The IR command is deprecated since revision I1 from December 2012.

IR rotates the entire image counterclockwise in increments of 90° around the image origin (0, 0).

All image objects are rotated. The IR command affects the entire image. It must be used only

once, at the beginning of the file. The order of execution is always MI, SF, OF, IR and AS,

independent of their order of appearance in the file.

8.1.5.1 IR Command

The syntax for the IR command is:

IR = '%' ('IR' ('0'|'90'|'180'|'270')) '*%';

Syntax

Comments

IR for Image Rotation

Image rotation is 0° counterclockwise (no rotation)

Image rotation is 90° counterclockwise

180

Image rotation is 180° counterclockwise

270

Image rotation is 270° counterclockwise

8.1.5.2 Examples

Syntax

Comments

%IR0*%

No rotation

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

%IR90*%

Image rotation is 90° counterclockwise

%IR270*%

Image rotation is 270° counterclockwise

Load Name (LN)

The IP command is deprecated since revision I4 from October 2013.

This historic command has no effect on the image and can be ignored.

LN assigns a name to the subsequent part of the file. It was intended as a human-readable

comment. Use the normal G04 command for human-readable comment. The LN command can

be used multiple times in a file.

8.1.6.1 LN Command

The syntax for the LN command is:

LN = '%' ('LN' name) '*%';

Syntax

Comments

LN for Load Name

<Name>

The name must comply with the syntax for a string, see

section

3.4.3.

8.1.6.2 Examples

Syntax

Comments

%LNVia_anti-pads*%

The name ‘Via_anti-pads’ is to the subsequent file section

Mirror Image (MI)

The MI command is deprecated since revision I1 from December 2012.

MI sets the mirroring for the coordinate data. All the coordinate data – and only coordinate data

- are mirrored according to the specified factor. Step and repeat distances are not

coordinate data – see 4.9 - and hence are not mirrored. Apertures are not mirrored.

This command affects the entire image. It can only be used once, at the beginning of the file.

The default is no mirroring. The order of execution is always MI, SF, OF, IR and AS,

independent of their order of appearance in the file.

Quite a number of implementations incorrectly also mirror apertures and/or

step and repeat distances. These incorrect implementations make the MI

too risky to use. We strongly recommend not to use MI on output as you do

know how the reader will interpret the file. If an image must be mirrored,

write out the mirrored coordinates and apertures.

8.1.7.1 MI Command

The syntax for the MI command is:

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

MI = '%' (['A'('0'|'1')]['B'('0'|'1')]) '*%';

Syntax

Comments

MI for Mirror image

A(0|1) Controls mirroring of the A-axis data:

A0 – disables mirroring

A1 – enables mirroring (the image will be flipped over the B-axis)

If the A part is missing, then mirroring is disabled for the A-axis data

B(0|1) Controls mirroring of the B-axis data:

B0 – disables mirroring

B1 – enables mirroring (the image will be flipped over the A-axis)

If the B part is missing, then mirroring is disabled for the B-axis data

8.1.7.2 Examples

Syntax

Comments

%MIA0B0*%

No mirroring of A- or B-axis data

%MIA0B1*%

No mirroring of A-axis data

Mirror B-axis data

%MIB1*%

No mirroring of A-axis data

Mirror B-axis data

Offset (OF)

The OF command is deprecated since revision I1 from December 2012.

OF moves the final image up to plus or minus 99999.99999 units from the imaging device (0, 0)

point. The image can be moved along the imaging device A or B axis, or both. The offset values

used by OF command are absolute. If the A or B part is missing, the corresponding offset is 0.

The offset values are expressed in units specified by MO command. This command affects the

entire image. It can only be used once, at the beginning of the file. The order of execution is

always MI, SF, OF, IR and AS, independent of their order of appearance in the file.

8.1.8.1 OF Command

The syntax for the OF command is:

OF = '%' (['A' decimal]['B' decimal]) '*%';

Syntax

Comments

OF for Offset

A<Offset>

Defines the offset along the output device A axis

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

B<Offset>

Defines the offset along the output device B axis

The <Offset> value is a decimal number n preceded by the optional sign (‘+’ or ‘-’) with the

following limitation:

≤ n ≤ 99999.99999

The decimal part of n consists of not more than 5 digits.

8.1.8.2 Examples

Syntax

Comments

%OFA0B0*%

No offset

%OFA1.0B-1.5*%

Defines the offset: 1 unit along the A axis, -1.5 units along the B axis

%OFB5.0*%

Defines the offset: 0 units (i.e. no offset) along the A axis, 5 units along

the B axis

Scale Factor (SF)

The SF command is deprecated since revision I1 from December 2012.

SF sets a scale factor for the A- and/or B-axis coordinate data. All the coordinate data – and

only coordinate data - are multiplied by the specified factor for the corresponding axis. Step and

repeat distances – see 4.9 - are not coordinate data and hence are not scaled. Apertures

are not scaled.

This command affects the entire image. It can only be used once, at the beginning of the file.

The default scale factor is ‘1’. The factor values must be between 0.0001 and 999.99999. The

scale factor can be different for A and B axes. The order of execution is always MI, SF, OF, IR

and AS, independent of their order of appearance in the file.

Quite some legacy readers incorrectly also scale step and repeat distances.

These incorrect implementations make the SF too risky to use. Current

readers simply do not support the We strongly recommend not to use SF on

output as you do know how the reader will interpret the file. If an image must

be scaled, write out the scaled coordinates.

8.1.9.1 SF Command

The syntax for the SF command is:

SF = '%' ('SF' ['A' decimal]['B' decimal]) '*%';

Syntax

Comments

SF for Scale Factor

A decimal

The scale factor for the A-axis data.

B defimal

The scale factor for the B-axis data.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

The scale factor is an unsigned decimal number n where 0.0001 ≤ n ≤ 999.99999.

8.1.9.2 Examples

Syntax

Comments

%SFA1B1*%

Scale factor 1. A decimal.

%SFA.5B3*%

Defines the scale factor: 0.5 for the A-axis, 3 for B. Decimals.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Single-quadrant arc mode (G74)

Historically, there were two arc quadrant modes:

 Single quadrant mode, set by G74 command

 Multi quadrant mode, set by G75 command

The single-quadrant mode G74 was deprecated in 2021. Already in 2020 it occurred in <1/1000

files. In the vast majority its presence had no effect: a G75 set multi-quadrant mode before any

arc was effectively constructed. Implementors of Gerber input software that wish to support

legacy files will get a very long way without fully implementing G74 mode but give an error when

an attempt is made to create an arc in G74 – this error will exceedingly rarely occur.

Quadrant mode

Comments

Single quadrant (G74)

Deprecated

In single quadrant mode the arc is not allowed to extend over

more than 90°. The following relation must hold:

0° ≤ A ≤90°, where A is the arc angle

If the start point of the arc is equal to the end point, the arc has

length zero, i.e. it covers 0°. A separate operation is required for

each quadrant. A minimum of four operations is required for a full

circle.

Multi quadrant (G75)

Current

In multi quadrant mode the arc is allowed to extend over more

than 90°. To avoid ambiguity between 0° and 360° arcs the

following relation must hold:

0° < A ≤ 360°, where A is the arc angle

If the start point of the arc is equal to the end point, the arc is a full

circle of 360°.

Quadrant modes

The syntax of the G74 commands is:

G74 = :('G74') '*';

Example:

G74*

The syntax of the D01 command in single quadrant circular interpolation mode is:

D01 = (['X' x_coordinate] ['Y' y_coordinate] 'D01' 'I' x_distance 'J' Y_distance ) '*';

Syntax

Comments

X x_coordinate X_coordinate defines the X coordinate of the end point of the arc.

arc. It is of the coordinate data type. The default is the X coordinate

of the current point.

Y y_coordinate

As above, but for the Y axis.

I x_distance The x_distance defines the distance between the arc start point and

the center parallel to the X axis. Distance is ≥ 0. It is of the

coordinate data type.

J<Distance>>

As above, but for the Y axis.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Syntax

Comments

D01

Interpolate operation code

49. Circular interpolation example

In single quadrant mode, awkwardly, the sign of the offsets is omitted, converting them to

unsigned distances. There are four candidates for the center: (<Current X> +/- <X distance>,

<Current Y> +/- <Y distance>). The center is the candidate that results in an arc with the

specified orientation, not greater than 90° and with the least deviation. The reason for this oddity

is purely historic, from a very distant past.

Example:

Syntax

Comments

G74*

D10*

X1100Y600D02*

G03*

X700Y1000I400J0D01*

X300Y600I0J400D01*

X700Y200I400J0D01*

X1100Y600I0J400D01*

X300D02*

G01*

X1100D01*

X700Y200D02*

Y1000D01*

Set single quadrant mode

Select aperture 10 as current aperture

Set the current point to (11, 6)

Set counterclockwise interpolation mode

Create quarter arc object (radius 4) to (7, 10)

Create quarter arc object (radius 4) to (3, 6)

Create quarter arc object (radius 4) to (7, 2)

Create quarter arc object (radius 4) to (11, 6)

Set the current point to (3 ,6)

Set linear interpolation mode

Create draw object to (11, 6)

Set the current point to (7, 2)

Create draw object to (7, 10)

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

50. Single quadrant mode example: arcs and draws

51. Single quadrant mode example: resulting image

8 10

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

In important difference between G74 and G75 arcs is what happens when start point and end

point coincide. For G75 this represents a full 360° arc, in G75 a zero-degree arc. Some

examples.

Syntax

Comments

D10*

G01*

X0Y600D02*

G74*

G02*

X0Y600I500J0D01*

Select aperture 10 as current aperture

Set linear interpolation mode

Set the current point to (0, 6)

Set single quadrant mode

Set clockwise circular interpolation mode

Create arc object to (0, 6) with radius 5

The resulting image is small dot, an instance of the aperture, at position (0, 6)

Syntax

Comments

D10*

G01*

X0Y600D02*

G75*

G02*

X0Y600I500J0D01*

Select aperture 10 as current aperture

Set linear interpolation mode

Set the current point to (0, 6)

Multi quadrant mode

Set clockwise circular interpolation mode

Create arc object to (0, 6) with center (5,6)

The resulting image is a full circle.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

8.2 Deprecated Command Options

Format Specification (FS) Options

This section describes deprecated options of the FS command (see 4.1).

The FS command could also be used to specify the following format characteristics:

 Trailing zero omission

 Incremental coordinate notation

 Low resolution (less than 6 decimals in inch units and less than 5 in mm units).

8.2.1.1 Trailing Zero Omission

Trailing zero omission is deprecated since revision 2015.06.

Trailing zero omission some or all trailing zero’s can be omitted but all leading zero’s are

required. To interpret the coordinate string, it is first padded with zero’s at the back until its

length fits the coordinate format. For example, with the “23” coordinate format, “15” is padded to

“15000” and therefore represents 15.000.

The coordinate data must contain at least one digit. Zero therefore should be encoded as “0”.

Trailing zero omission is specified by ‘T’ after the FS code. (The normal leading zero omission is

specified by ‘L’ after the FS code.)

Example:

%FSTAX25Y25*%

Trailing zero omission is rarely found in legacy files. Gerber readers will go a long way without

supporting it.

8.2.1.2 Incremental Notation

Incremental notation is deprecated since revision I1 from December 2012.

Incremental notation means that coordinate values are as the incremental distances from the

previous coordinate position. It is specified by the "I" in the FS command, after the "L" or "T" for

leading or trailing. (The normal absolute notation is specified by ‘A’ in the FS command.)

Example:

%FSLIX25Y25*%

%FSTIX36Y36*%

Incremental notation was sometimes used as a simplistic compression when saving a few bytes

was a fantastic advantage, and before the invention of Lempel–Ziv–Welch (LZW) and other

lossless compression methods. The problem is that the accumulation of rounding errors leads to

significant loss or precision. This results in poor registration, invalid arcs, self-intersecting

contours, often resulting in scrap. Avoid incremental notation like the plague.

Incremental notation is fortunately but rarely used in legacy files. Gerber readers will go a long

way without supporting it.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

8.2.1.3 Low resolution

Low resolution, this is using less than 6 decimals in inch units and less than 5 decimals in mm

units is deprecated since revision 2015.06.

Low resolution was introduced in the 1960's as a simplistic compression method when saving a

few bytes was of paramount importance, and computers were too feeble for proper lossless

compression methods such as Lempel–Ziv–Welch (LZW).

Low resolution loses numerical precision and poor numerical precision is the main cause of

often obscure bugs in geometric software. It leads to poor registration of objects between PCB

layers; loss of accuracy; self-intersecting contours; invalid arcs; small arcs turning in full circles,

missing clearances. Low resolution is the main cause of problems with Gerber files, sometimes

leading to scrap.

Unfortunately, low resolution files are still quite common. There are even files in inch with 3

decimals, or a resolution of 1 mil; this is asking for problems.

It is sometimes recommended to use low resolution because some Gerber readers allegedly

only handle low resolutions. Do not listen. This may have been true in a distant past, but it no

longer true, if it ever was. Ask yourself: does it make sense to risk scrap to save a few bytes or

to cater for a few rumored stone-age implementations? The days that saving a few bytes was

important are long gone. The risks of low resolution remain. Avoid low resolution like the plague.

Low resolution files are unfortunately quite common in legacy files. Gerber readers that do not

support low resolution will fail to read a significant fraction of Gerber files.

Rectangular Hole in Standard Apertures

Rectangular holes in standard apertures are deprecated since revision 2015.06. They occur

very rarely in legacy files.

In addition to the round hole described in section 4.4 older versions of this

specification also allowed rectangular holes. Rectangular holes do not rotate

with the aperture, according to these historic specifications. This is very

counterintuitive and a source of errors. Rectangular holes were deprecated

because of this problem, and because rectangular holes are not very useful

in the first place. Do not use them. If you need a rectangular hole construct a macro aperture.

The syntax of a rectangular hole was common to all standard apertures:

hole = x_hole_size Y y_hole_size

The parameters specify the X and Y sizes of the hole. Decimals >

The hole must strictly fit within the standard aperture. It is centered on the aperture.

Example:

%FSLAX26Y26*%

%MOMM*%

%ADD10C,10X5X5*%

%ADD11C,1*%

G01*

%LPD*%

D11*

X-25000000Y-1000000D02*

X25000000Y1000000D01*

D10*

X0Y0D03*

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

M02*

52. Standard (circle) aperture with a rectangular hole above a draw

Note that the draw is visible through the hole.

Rectangular holes appear very rarely in legacy files.

Draws and Arcs with Rectangular Apertures

The effect of stroking a line segment with a rectangular aperture is illustrated below. If the

rectangle aperture is aligned with the line being stroked the result is a draw with line endings

which have right angles:

53. Creating a draw: the aperture is aligned with line

If the rectangle is not aligned the result is as in the illustration below. The rectangle is not

automatically rotated to align with the line being stroked.

54. Creating a draw: the aperture is not aligned with line

Line being stroked Aperture Draw

Line being stroked

Aperture Draw

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

This was only allowed with the solid rectangle standard aperture. Other standard apertures or

macro apertures that fortuitously have a rectangular shape are not allowed.

This option was deprecated in 2020.09. Drawing with rectangular was never used often, even

less at other angles than multiples of 90º. A developer of Gerber input will get a long way if he

only implements a warning on interpolations with rectangular apertures.

Macro Primitive Code 2, Vector Line

Primitive 2 was deprecated in 2015. It occurs but very rarely in legacy files.

Primitive 2 is identical to primitive 20. See 4.5.1.4.

Macro Primitive Code 22, Lower Left Line

Primitive 22 was deprecated in 2015. It occurs but very rarely in legacy files.

A lower left line primitive is a rectangle defined by its width, height, and the lower left point.

Modifier number

Description

Exposure off/on (0/1))

Rectangle width

, a decimal ≥ 0

Rectangle height

, a decimal ≥ 0.

A decimal defining the

X coordinate of lower left point.

A decimal defining the

Y coordinate of lower left point.

A decimal defining the r

otation angle around the origin (rotation is not

around the center of the object)

1. Line (lower left) primitive

Example:

%AMLINE2*22,1,6.8,1.2,0,0,0*%

4, 5 3

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Macro Primitive Code 6, Moiré

This primitive was deprecated in 2021. It is very rarely, if ever, used in legacy files.

The moiré primitive is a cross hair centered on concentric rings. Exposure is always on.

Parameter

number

Description

Center point X coordinate.

Center point Y coordinate.

Outer diameter of outer concentric ring ≥ 0.

Ring thickness ≥ 0.

Gap between rings ≥ 0.

6 Maximum number of rings. An integer ≥ 0. The effective number of

rings can be less if the center is reached. If there is not enough space

for the inner ring it becomes a full disc.

Crosshair thickness ≥ 0. If the thickness is 0 there are no crosshairs.

Crosshair length ≥ 0. If the length is 0 there are no crosshairs.

9 Rotation angle, in degrees counterclockwise. The primitive is rotated

around the origin of the macro definition, i.e. the (0, 0) point of macro

coordinates.

2. Moiré primitive

1, 2

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Below there is an example of an AM command that uses the moiré primitive.

Example:

%AMMOIRE*

6,0,0,5,0.5,0.5,2,0.1,6,0*%

8.3 Deprecated Syntax Variations

Combining G01/G02/G03 and D01 in a single command.

This construction is deprecated since revision 2015.06.

The command codes G01, G02, G03 could be put at the beginning of the word containing a D01

command. The graphics state is then modified before the D01 is executed.

Example:

G01X100Y100D01*

G01 sets the interpolation mode to linear and this used to process the coordinate data

X100Y100 from the same word as well as the coordinate data X200Y200 from the next word.

The syntax was as follows:

GnnD01 = ('G' ('01'|'02'|'03') coordinate_data 'D01') '*'

This construction is a useless variation and is deprecated since revision 2015.06. However, it

happens quite frequently in legacy files, so readers may want to support it.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Coordinate Data without Operation Code

Coordinate data without explicit operation code after a D01, on other words the modal use of

D01, is deprecated since revision I1 from December 2012.

A D01 code sets the deprecated operation mode to interpolate. It remains in interpolate mode

till any other D code is encountered. In sequences of D01 operations this allows omitting an

explicit D01 code after the first operation.

Example:

D10*

X700Y1000D01*

X1200Y1000*

X1200Y1300*

D11*

X1700Y2000D01*

X2200Y2000*

X2200Y2300*

The operation mode is only defined after a D01. The operation mode after a D02, D03 or an

aperture selection (Dnn with nn≥10) is undefined. Therefore a file containing coordinates without

operation code after a D02, D03 or an aperture selection (Dnn with nn≥10) is invalid.

Warning: Coordinate data without explicit operation code saves a few bytes but its exact

use is not intuitive in relation to D03. The risk of scrap far outweighs the meager benefit.

Style Variations in Command Codes

Sometimes a word command such as G01 was spelled as G1, or g01, or G001. These

variations were discouraged but tolerated. These variations were finally revoked in 2020.09 –

only G01 style is allowed.

Deprecated usage of SR

These constructions are deprecated since revision 2016.01.

The command %SRX1Y1I0J0*% strictly speaking starts a step and repeat of 1x1, i.e. no step

and repeat at all. It is historically sometimes used as an alternative for an %SR*% to close an

SR statement. This is still used quite frequently.

Sometimes an SR command other than 1x1 such as %SRX2Y3I1,5J2.2*% is put seemingly

inside an SR statement. Its effect is then to terminate the current SR statement and start a new

one with its parameters. This is used rarely.

Another deprecated variation is that an SR statement at the end of a file is not closed. The end

of file M02* is then an implicit close. This is used rarely.

Another variation is that the file header contains a %SRX1Y1I0J0*%. This does not mean a

futile 1x1 step and repeat is started. It just indicates that the file does not start with a step and

repeat, which is obvious. This command can be ignored. This is used quite frequently.

8.4 Deprecated Attribute Values

The following values for the .AperFuntion attribute were deprecated in 2019.06. They were very

rarely, if ever, used.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

CutOut

PCB cut-outs. This is the generic term for a hole other

than a drill hole.

Slot

PCB slots. This is a subset of the cut-outs. Which cut-

outs are called slots is subjective. In case of doubt use

the value CutOut.

Cavity

Cavities in a PCB.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

8.5 Standard Gerber (RS-274-D)

The current Gerber layer format is also known as RS-274X or Extended Gerber. There was also

a historic format called Standard Gerber or RS-274-D format.

Standard Gerber is technically obsolete. It and was revoked in revision I1 from December 2012

and superseded by RS-274X.

Standard Gerber is revoked and superseded by Extended Gerber, which is the current Gerber

format. Consequently, Standard Gerber no longer complies with the Gerber specification. Files

in that format can no longer be correctly called Gerber files. Standard Gerber files are not only

deprecated, they are simply invalid.

It differs from the current Gerber format (RS-274X), in that it:

• did not support G36 and G37 codes

• did not support any extended commands

• did not support attributes

Standard Gerber did not allow defining the coordinate format or aperture shapes. It was

incomplete as an image description format. It lacked the imaging primitives needed to

unequivocally transfer information from PCB CAD to CAM.

The word “standard” is misleading here. Standard Gerber was standard NC format. It was not a

standard image format: image generation needs a so-called wheel file, and that wheel file was

not governed by a standard. The interpretation of a wheel files, and consequently of a Standard

Gerber files, was subjective. In Extended Gerber (RS-274X) image generation is fully governed

by the standard. Extended Gerber is the true image standard.

Standard Gerber had major drawbacks compared to the current Gerber format and did not offer

a single advantage. Standard Gerber is obsolete. There is not a single valid reason to use

standard Gerber rather than Extended Gerber.

Always use Extended Gerber (RS-274X). Never use Standard Gerber.

Warning: The responsibility of errors or misunderstandings about the wheel file when

processing a Standard Gerber file rests solely with the party that decided to use revoked

Standard Gerber, with its informal and non-standardized wheel file, rather than Extended

Gerber, which is unequivocally and formally standardized.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

9 References

American National Standard for Information Systems — Coded Character Sets — 7-Bit

American National Standard Code for Information Interchange (7-Bit ASCII), ANSI X3.4-1986

https://en.wikipedia.org/wiki/MD5

https://en.wikipedia.org/wiki/Unicode

https://en.wikipedia.org/wiki/UTF-8

http://en.wikipedia.org/wiki/ISO_8601

https://en.wikipedia.org/wiki/Binary_image

https://en.wikipedia.org/wiki/Zip_(file_format)

https://tools.ietf.org/html/rfc4122

https://msdn.microsoft.com/en-us/library/windows/desktop/aa378623(v=vs.85).aspx

https://developer.apple.com/library/mac/documentation/Foundation/Reference/NSUUID_Class

The Inventor's Dilemma: The Remarkable Life of H. Joseph Gerber, by David Gerber.

https://tatsu.readthedocs.io/en/stable/

. Documentation for the TatSu PEG parser generator.

https://en.wikipedia.org/wiki/Parsing_expression_grammar

https://bford.info/packrat/ Bryan Fords page on parsing expression grammars.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

10 History

The Gerber format derives its name from the former Gerber Systems Corp. A leading supplier of

vector photoplotters from the 1960s onwards, Gerber based its plotter input on a subset of the

EIA RS-274-D NC format, and in1980, it published a well-written specification titled “Gerber

Format: a subset of EIA RS-274-D; plot data format reference book”. The format was so well

suited for its task that it was widely adopted and became the de-facto standard format for vector

plotters, known as Standard Gerber.

Vector photoplotters are NC machines, and Standard Gerber, which is dedicated to vector

photoplotters, is an NC format. As of the 1980s, vector photoplotters started losing ground to

raster plotters. Based on bitmap technology, these newer devices demanded rather more than a

simple NC format, so Gerber extended the original NC format with so called “Mass Parameters”,

converting it to a fully-fledged image file formats. This resulted in a family of effective image

description formats designed specifically to drive Gerber's PCB devices and raster plotters. In

1998 Gerber Systems Corp. was taken over by Barco and incorporated into its PCB division –

Barco ETS, now Ucamco. At this point, Barco drew all the variants in Gerber's family of formats

into a single standard image format.

On September 21, 1998 Barco-Gerber published the Gerber RS-274X Format User's Guide.

The format became known as Extended Gerber or GerberX. This is a full image description

format, which means that an Extended Gerber file contains the complete description of a PCB

layer, providing everything needed for an operator to generate a PCB image, and enabling any

aperture shape to be defined. Unlike Standard Gerber, it does not need the support of additional

external files, and it specifies planes and pads clearly and simply without the need for painting

or vector-fill. The Extended Gerber format quickly superseded Standard Gerber as the de facto

standard for PCB image data, and is sometimes called "the backbone of the electronics

industry". A sequence of revisions clarifying the specification was published over the years,

culminating in revision H of January 2012.

During 2012, Ucamco reviewed the entire format in depth in “the great reform”. Over 10.000

files from all over the world were gathered into a representative library to help establish current

practice. Rarely used and historic format elements were deprecated. Format elements with

conflicting interpretations in the market were either deprecated or clarified. The specification

document itself was re-organized, the quality of the text and the drawings improved and many

new drawings were added. This resulted in The Gerber Format Specification, revision I1

published in December 2012. Revisions I2, I3 and finally I4 from November 2013 further

improved the document. The result was a powerfully clear and simple format, without needless

embellishments, focused on the current needs of the PCB industry. This version of the Gerber

Format was developed by Karel Tavernier and Rik Breemeersch. They were assisted by an

advisory group including Ludek Brukner, Artem Kostyukovich, Jiri Martinek, Adam Newington,

Denis Morin, Karel Langhout and Dirk Leroy. Grateful thanks are extended to all those who

helped the development of the revision by posting their questions, remarks and suggestions on

the Ucamco website. Particular thanks are due to Paul Wells-Edwards whose insightful

comments contributed substantially to the revision.

Until this point, Gerber was purely an image description format. Recognizing that a PCB image

must be supported with meta-information that describes, say, the function of an image file in the

layer structure, Ucamco realized that it could convey that information clearly and unequivocally

using attributes. Accordingly, and in June 2013, the company publicly proposed to extend the

Gerber format using attributes, and invited feedback on its proposal from the Gerber user

community. The outcome of this was revision J1, completed in February 2014, during which

Gerber got its attributes. It was a major step forward for the format, at least on a par with the

changes made when Standard Gerber became Extended Gerber. Sometimes called the second

extension, the latest version of the Gerber format is known as Gerber version 2, or X2 (as

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

opposed to X1, which is Gerber without attributes). Gerber version 2 is fully backward

compatible as attributes do not affect the image at all. Subsequent revisions, J2 to J4, clarified

the specification and added new standard attributes. Gerber version 2 was developed by Karel

Tavernier, Ludek Brukner and Thomas Weyn. They were assisted by an advisory group

including Roland Polliger, Luc Samyn, Wim De Greve, Dirk Leroy and Rik Breemeersch.

In September 2014 Ucamco published an open letter declaring Standard Gerber obsolete and

revoking it.

In August 2015, Ucamco published a draft specification adding nested step and repeat and

block apertures to make panel descriptions more efficient, calling for comments from the user

community. In November 2016 the review process was closed after substantial input and

modifications and the final version included in revision 2016.12. This revision was developed by

Karel Tavernier and Rik Breemeersch.

Early in 2015, the entire specification was reviewed once again by Karel Tavernier, Thomas

Weyn and Artem Kostyukovich focused on making the specification easier to read and

understand, while taking great care to ensure consistent and precise terminology. Some further

elements were identified as superfluous and were deprecated. Not least, special attention was

given to the 'Overview' chapter, with the aim of turning it into a tutorial that can be understood

by non-experts. The result of this work is revision 2015.06.

In July 2016 Karel Tavernier from Ucamco published a draft specification to include netlist

information in Gerber for public review. Several revisions of the draft were triggered by input

from users. The final version was in included in revision 2016.11 from November 2, 2016.

In March 2017 Karel Tavernier from Ucamco published a draft specification to include fab

documentation in Gerber for public review.

In May 2020 Karel Tavernier from Ucamco published a specification for including component

information in Gerber, aka X3.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

11 Revisions

11.1 Revision 2021.02

Deprecated single quadrant mode (G74) and macro primitive code 6 (moiré).

Now includes a formal grammar for the complete format. See 3.5.

Several typo's were fixed; thanks to Nick Meeker and Kevin Shi for their careful review. The

term 'data block' was replaced by 'word' to eliminate confusion with aperture blocks.

11.2 Revision 2020.09 – X3

In March 2020 a specification for including component information – Gerber X3 2020.03 – was

published. Gerber X3 was developed in discussion with a team of people. Karel Tavernier

developed a prototype specification which was circulated privately with Wim De Greve, Jean-

Pierre Charras, Thiadmer Riemersma, Bruce McKibben and Rafal Powierski in December 2018.

In intense discussion among this group the draft went through five revisions until a first public

draft was published in October 2019, calling for input from the user community. The review

process was closed in February 2020 with the publication of the separate X3 specification, now

merged in this document.

This separate specification on components is now merged into this main specification.

Gerber now accepts Unicode characters for attribute values that contain user-defined meta-

information, and therefore may require special characters and other languages than English.

Draws with rectangular apertures were deprecated, see 8.2.3, as were some style variations in

word commands, see 8.3.3.

Clarified the semantics of the .GenerationSoftware attribute. Specified more clearly how drill

files must be constructed, as suggested by Wim De Greve and Luc Samyn.

Fixed errors and oversights pointed out by Greg Huangqi and Jim J. Jewett. Especially Jim J.

Jewett reviewed the specification in great detail. Replaced the unusual term 'modifier' with the

more usual term 'parameter'.

Revision 2020.09 was developed by Karel Tavernier.

11.3 Revision 2019.09

Replaced the option [Filled|NotFilled] on the ViaDrill value of the .AperFunction attribute with the

more specific IPC-4761 types, see 5.6.10.

Revision 2019.09 was developed by Karel Tavernier.

11.4 Revision 2019.06

The .AperFunction values CutOut, Slot and Cavity were deprecated. See 8.3.

Made it more explicit that macro aperture names cannot be reused, see Error! Reference

source not found.. Corrected an error in the examples pointed out by Abe Tusk, and in 2.1,

pointed out by Radim Halíř.

Revision 2019.06 was developed by Karel Tavernier.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

11.5 Revision 2018.11

Removed the .PF attribute, and replaced its content by an additional optional field to the .P

attribute. See 5.6.14.

Fixed a number of typos and minor errors pointed out by Jörg Naujoks, Rik Breemeersh and

Radim Halíř.

Revision 2018.11 was developed by Karel Tavernier.

11.6 Revision 2018.09

Corrected an error in the polygon aperture, section 4.4.5, and polygon primitive, section 4.5.1.7.

Clarified the rotation of the deprecated rectangular holes in apertures, section 8.2.2 These

issues were pointed out by Remco Poelstra.

Corrected an error in the moiré primitive specification, section 8.2.6. The error was pointed out

by Vasily Turchenko.

Clarified how object attributes are attached to regions, triggered by remarks from Radim Halíř.

Defined allowed range of the scale factor in 4.9.5, as suggested by Andreas Weidinger.

Defined orientation of text mirroring in section 5.6.12. Triggered by Nicholas Meeker.

Nicholas Meeker, Andreas Weidinger, Radim Halíř and Denis Morin carefully proofread the

document, which resulted in many text corrections.

Revision 2018.09 was developed by Karel Tavernier.

11.7 Revision 2018.06

Removed PressFit option from the ComponentPad attribute value; it is also a ComponentDrill

option and that is sufficient.

Clarified pad attribute values for via, component, SMD, BGA on inner layers. Clarified FS

command, see 4.1 and 8.2.1. Fixed broken links to references indicated by Vasily Turchenko.

Revision 2018.06 was developed by Karel Tavernier.

11.8 Revision 2018.05

Added .PF attribute, as suggested by Matthew Sanders.

Corrected errors in an example in 4.9.1 pointed out by Erik Forwerk. Corrected errors in the SR

definition and Backus-Naur form pointed out by Remco Poelstra, see 4.11. Simplified the

Backus-Naur form of the region statement, see 4.10.2. Corrected an error in 5.4 pointed out by

Dries Soentjens.

Revision 2018.05 was developed by Karel Tavernier.

11.9 Revision 2017.11

Allow the .N attribute not only on copper layers but also on plated drill layers, see 5.6.13.

Remove .FileFunction value Keep-out. Use Profile instead.

Specified that to combine files zip is the only allowed archive format, as suggested by Rafal

Powierski.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Simplified the Backus-Naur form of aperture blocks, see 4.11.2. Added synoptic table with

macro primitives in 4.5.1.1. Added synoptic table one with standard apertures in 4.4.1. Added

Backus-Naur form of the region statement. Added link to the Reference Gerber Viewer in 1.3.

Fixed typos pointed out by Forest Darling. Fixed a number or typos pointed out by Radim Halíř.

Revision 2017.11 was developed by Karel Tavernier.

11.10 Revision 2017.05

Added the new file attribute .SameCoordinates, see 5.6.5.

Added file functions Depthrout, Viafill, Vcut, and Vcutmap.

Created section 5.6.15.1 with guidelines on the use of attributes in fabrication data; added

guidelines on how to define the PCB profile in 6.2.

Reorganized and edited the chapter Overview. Clarified section on zero-size apertures.

Corrected an error in the comment in example 6.6.1.2 pointed out by Nav Mohammed.

Corrected errors in the examples in 5.6.5 pointed out by Rik Breemeersch,

Revision 2017.05 was developed by Karel Tavernier.

11.11 Revision 2017.03

Added section 5.6.15.1, specifying how to put text in the image.

Changed file function Gluemask to Glue; added explanation; see 5.6.3.

Reorganized chapter 3.5. Extended section 4.10.5.

Corrections in 4.9.1, 4.9.5, 4.10.1 and in Aperture Attributes on Regions triggered by remarks

from Remco Poelstra. Corrected an error in example 0 pointed out by Danilo Bargen.

Revision 2017.03 was developed by Karel Tavernier.

11.12 Revision 2016.12 – Nested step and repeat

This is a major revision with powerful new imaging functions: 4.11, 0, 4.9.4 and 4.9.5. These

allow nested step and repeat to define panels efficiently, see 4.11.3 and 4.11.4.

Thera are fixes for errors in examples, pointed out by Danilo Bargen and Urban Bruhin.

Revision 2016.12, and especially the new imaging function for panels was developed by Karel

Tavernier and Rik Breemeersch. The first draft of these functions was published in August 2016.

During the public review process. Thomas Weyn, Bruce McKibben, Masao Miyashita and

Remco Poelstra provided essential input.

11.13 Revision 2016.11

This major revision allows to include the CAD netlist to Gerber files by adding three new

standard object attributes – see 5.6.15.1 above. The goal of the Gerber CAD netlist is to

facilitate upfront communication between the different parties involved in design, assembly and

automation. The X2 attributes proposed include CAD netlists in Gerber fabrication data and

allow to:

• Attach the component reference designator, pin number and net name to the component

pads in the outer copper layers. This information is essential for a complete board

display and for a complete board display. More importantly, the netlist provides a

powerful checksum to guarantee PCB fabrication data integrity.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

• Attach the netlist name to any conducting object on any copper layer. Lightweight

viewers can then display netlists without the need for an algorithm to compute

connectivity

• Attach the component reference to any object, e.g. to identify all the legend objects

belonging to a given component, for example.

Several text improvements. Section 4.10.3 on regions clarified triggered by deep questions

asked by Remco Poelstra.

Revision 2016.11 was developed by Karel Tavernier. Jean-Pierre Charras provided essential

input on the CAD netlist, and further remarks by Remco Poelstra and Wim De Greve were

included.

11.14 Revision 2016.09

New or modified attribute values – see 5.6.10:

• Replaced file function Drawing with OtherDrawing.

• Added the optional field Filled|NotFilled to ViaDrill.

• Added aperture function EtchedComponent.

Added object attributes – see 5.4. Object attributes attach information to individual graphical

objects.

Corrected an error in example 4.10.4.6. The error was pointed out by Thomas van Soest and

Siegfried Hildebrand. Clarified the syntax of attaching aperture attributes to regions. Added Perl

script to show precisely how to calculate the .MD5. Several other clarifications.

Revision 2016.09 was developed by Karel Tavernier.

11.15 Revision 2016.06

Added a section on back-drilling job triggered by questions from Alexey Sabunin. See 6.6.1.1.

The .ProjectID UUID was changed to RFC4122; rewritten by Remco Poelstra. See 5.6.8.

Aperture function attributes were clarified triggered by remarks from John Cheesman. Drill sizes

were clarified triggered by remarks from Jeff Loyer.

11.16 Revision 2016.04

Added PressFit label to component drill and pad attributes; see ComponentPad and

ComponentDrill. Revoked default on current point.

Text improvements that do not change the format: Removed superfluous concept of level and

replaced the name ‘Level Polarity’ by ‘Load Polarity. Various other text improvements.

11.17 Revision 2016.01

Added drill and pad functions for castellated holes. Added optional types break-out and tooling

on MechanicalDrill.

Deprecated closing an SR with the M02.

Text improvements that do not change the format: Clarified .AperFunction attribute values.

Clarified when to use of standard or user attributes. Clarified how aperture attributes can be set

on regions.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

11.18 Revision 2015.10

Added items to section Errors and Bad Practices.

Added file function attribute .FilePolarity.

Refined drawing .FileFunction attributes Replaced Mechanical by FabricationDrawing and

Assembly by AssemblyDrawing. Added definitions to the drawing types. Added mandatory

(Top|Bot) to .AssemblyDrawing, as suggested by Malcolm Lear. Added ArrayDrawing.

11.19 Revision 2015.07

The superfluous and rarely, if ever, used macro primitives 2 and 22 were revoked. The

.AperFunction aperture attribute was simplified:

• Filled / NotFilled option is removed for the ViaDrill function

• ImpC / NotC option is removed from the Conductor function

11.20 Revision 2015.06

New file attributes were specified: .GenerationSoftware (5.6.5), .CreationDate (5.6.5) and

.ProjectId (5.6.8).

The mistakenly omitted rotation parameter of the circle macro primitive was restored. Unicode

escape sequences in strings are now defined.

Operation syntax combining the G and D codes in a single word were deprecated. The

rectangular hole in standard apertures was deprecated. Usage of low resolutions and trailing

zero omission in the FS command was deprecated.

The entire document was revised for clarity. The readability of the text was improved. The

terminology was made consistent. The glossary was expanded. A number of additional images

were added, including the Gerber file processing diagrams, command types diagram, aperture

macro rotation illustration. Some of existing images were recreated to improve the quality.

Several new tables were added to explain the relation between D code commands and graphics

state parameters. The glossary was updated. The sections were rearranged.

From now the revision numbering follows the year.month scheme as in 2015.06.

11.21 Revision J3 (2014 10)

The .FileFunction values for copper and drill layers were extended to contain more information

about the complete job.

11.22 Revision J4 (2015 02)

The .AperFunction values “Slot”, “CutOut” and “Cavity” were added. The text on standard

attributes was made more explicit. An example of a poorly constructed plane was added.

11.23 Revision J2 (2014 07)

Attaching aperture attributes with regions was much simplified. A section about numerical

accuracy was added.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

11.24 Revision J1 (2014 02) – X2

This revision created Gerber X2 by adding attributes to what was hitherto a pure image format.

See chapter 5. X2 is Gerber version 2, with “X1” being Gerber version 1, without attributes.

Gerber X2 is backward compatible as attributes do not affect image generation.

11.25 Revision I4 (2013 10)

The commands LN, IN and IP were deprecated. The possibility of re-assigning D codes was

revoked.

The regions overview section 4.10.1 was expanded and examples were added different places

in 4.10 to further clarify regions. The chapters on command codes and syntax were

restructured. The constraints on the thermal primitive parameters were made more explicit.

Wording was improved in several places. The term ‘(mass) parameter’ was replaced by

‘extended command’.

11.26 Revision I3 (2013 06)

Questions about the order and precise effect of the deprecated commands MI, SF, OF, IR and

AS were clarified. Coincident contour segments were explicitly defined.

11.27 Revision I2 (2013 04)

The “exposure on/off” parameter in macro apertures and the holes in standard apertures are

sometimes incorrectly implemented. These features were explained in more detail. Readers and

writers of Gerber files are urged to review their implementation in this light.

11.28 Revision I1 (2012 12)

General. The entire specification was extensively reviewed for clarity. The document was re-

organized, the text and the drawings have been improved and many new drawings were added.

Deprecated elements. Elements of the format that are rarely used and superfluous or prone to

misunderstanding have been deprecated. They are grouped together in the second part of this

document. The first part contains the current format, which is clean and focused. We urge all

creators of Gerber files no longer to use deprecated elements of the format.

Graphics state and operation codes. The underlying concept of the graphics state and

operation codes is now explicitly described. See section 2.5 and 2.5. We urge all providers of

Gerber software to review their implementation in the light of these sections.

Defaults. In previous revisions the definitions of the default values for the modes were scattered

throughout the text or were sometimes omitted. All default values are now unequivocally

specified in an easy-to-read table. See 2.5. We urge all providers of Gerber software to review

their handling of defaults.

Rotation of macro primitives. The rotation center of macro primitives was clarified. See 4.5.3.

We urge providers of Gerber software to review their handling of the rotation of macro

primitives.

G36/G37. The whole section is now much more specific. We urge providers of Gerber software

to review their contour generation in this light.

Having a question or remark about the spec? Please contact us at gerber@ucamco.com

Coordinate data. Coordinate data without D01/D02/D03 in the same word can lead to

confusion. It therefore has been deprecated. See 8.1.10. We urge all providers of Gerber

software to review their output of coordinate data in this light.

Maximum aperture number. In previous revisions the maximum aperture number was 999.

This was insufficient for current needs and numerous files in the market use higher aperture

numbers. We have therefore increased the limit to the largest number that fits in a signed 32-bit

integer.

Standard Gerber. Standard Gerber is revoked because it has many disadvantages and not a

single advantage. We urge all users of Gerber software not to use Standard Gerber any longer.

Incremental coordinates. These have been deprecated. Incremental coordinates lead to

rounding errors. Do not use incremental coordinates.

Name change: area and contour instead of polygon. Previous revisions contained an object

called a polygon. This caused confusion between this object and a polygon aperture. These

objects remain unchanged but are now called areas, defined by their contours. This does not

alter the Gerber files.

Name change: level instead of layer. Previous revisions of the specification contained a

concept called a layer. These were often confused with PCB layers and have been renamed as

levels. This is purely narrative and does not alter the Gerber files.