Reference manual

This document is Copyright © 2010-2015 by its contributors as listed below. You may distribute it and/or modify it under the terms of either the GNU General Public License (, version 3 or later, or the Creative Commons Attribution License (, version 3.0 or later.

All trademarks within this guide belong to their legitimate owners.


Jean-Pierre Charras, Fabrizio Tappero.


Please direct any bug reports, suggestions or new versions to here:

Publication date and software version

2015, May 21.

1. Introduction

1.1. KiCad

KiCad is an open-source software tool for the creation of electronic schematic diagrams and PCB artwork. Beneath its singular surface, KiCad incorporates an elegant ensemble of the following software tools:

  • KiCad: Project manager

  • Eeschema: Schematic editor and component editor

  • Pcbnew: Circuit board layout editor and footprint editor

  • GerbView: Gerber viewer

3 utility tools are also included:

  • Bitmap2Component: Component maker for logos. It creates a schematic component or a footprint from a bitmap picture.

  • PcbCalculator: A calculator that is helpful to calculate components for regulators, track width versus current, transmission lines, etc.

  • Pl Editor: Page layout editor.

These tools are usually run from the project manager, but can be also run as stand-alone tools.

At the time of writing, KiCad is considered mature and can be used for the successful development and maintenance of complex electronic boards.

KiCad does not present any board-size limitation and it can handle up to 32 copper layers, 14 technical layers and 4 auxiliary layers.

KiCad can create all the files necessary for building printed circuit boards, including:

  • Gerber files for photo-plotters

  • drilling files

  • component location files

Being open source (GPL licensed), KiCad represents the ideal tool for projects oriented towards the creation of electronic hardware with an open-source flavour.

KiCad is available for Linux, Windows and Apple macOS.

1.2. KiCad files and folders

KiCad creates and uses files with the following specific file extensions (and folders) for schematic and board editing.

Project manager file:


Small file containing a few parameters for the current project, including the component library list.

Schematic editor files:


Schematic files, which do not contain the components themselves.


Schematic component library files, containing the component descriptions: graphic shape, pins, fields.


Schematic component library documentation, containing some component descriptions: comments, keywords, reference to data sheets.


Schematic component library cache file, containing a copy of the components used in the schematic project.

Board editor files and folders:


Board file containing all info but the page layout.


Footprint library folders. The folder itself is the library.


Footprint files, containing one footprint description each.


Board file in the legacy format. Can be read, but not written, by the current board editor.


Footprint library in the legacy format. Can be read by the footprint or the board editor, but not written.


Footprint library list (footprint libraries table): list of footprint libraries (various formats) which are loaded by the board or the footprint editor or CvPcb.

Common files:


Page layout description files, for people who want a worksheet with a custom look.


Netlist file created by the schematic, and read by the board editor. This file is associated to the .cmp file, for users who prefer a separate file for the component/footprint association.

Special file:


Association between components used in the schematic and their footprints. It can be created by Pcbnew, and imported by Eeschema. The purpose is a back import from Pcbnew to Eeschema, for users who change footprints inside Pcbnew (for instance using Exchange Footprints command) and want to import these changes in schematic.

Other files:

They are generated by KiCad for fabrication or documentation.


Gerber files, for fabrication.


Drill files (Excellon format), for fabrication.


Position files (ASCII format), for automatic insertion machines.


Report files (ASCII format), for documentation.


Plot files (Postscript), for documentation.


Plot files (PDF format), for documentation.


Plot files (SVG format), for documentation.


Plot files (DXF format), for documentation.


Plot files (HPGL format), for documentation.

2. Installation and configuration

2.1. Display options

Pcbnew needs the support of OpenGL v2.1 or higher.

2.2. Initialization of the default configuration

A default configuration file named is supplied in kicad/template. It serves as a template for any new project and is used to set the list of library files loaded by Eeschema. A few other parameters for Pcbnew (default text size, default line thickness, etc.) are also stored here.

Another default configuration file named fp-lib-table may exist. It will be used only once to create a footprint library list; otherwise the list will be created from scratch.

2.3. Modifying the default configuration

The default file can be freely modified, if desired.

Verify that you have write access to kicad/template/

Run KiCad and load project.

Run Eeschema via KiCad. Modify and update the Eeschema configuration, to set the list of libraries you want to use each time you create new projects.

Run Pcbnew via KiCad. Modify and update the Pcbnew configuration, especially the footprint library list. Pcbnew will create or update a library list file called footprint library table. There are 2 library list files (named fp-lib-table): The first (located in the user home directory) is global for all projects and the second (located in the project directory), if it exists, is specific to the project.

2.4. Initialization of external utilities

When using KiCad, choosing a text editor and a PDF viewer is useful.

These settings are accessible from the Preference menu:


2.5. Configuration of paths

In KiCad, one can define paths using an environment variable. A few environment variables are internally defined by KiCad, and can be used to define paths for libraries, 3D shapes, etc.

This is useful when absolute paths are not known or are subject to change, and also when one base path is shared by many similar items. Consider the following which may be installed in varying locations:

  • Eeschema component libraries

  • Pcbnew footprint libraries

  • 3D shape files used in footprint definitions

For instance, the path to the connect.pretty footprint library, when using the KISYSMOD environment variable, would be ${KISYSMOD}/connect.pretty

This option allows you to define a path with an environment variable, and add your own environment variables to define personal paths, if needed.

KiCad environment variables:


Templates used during project creation. If you are using this variable, it must be defined.


Frequently used in example footprint lib tables. If you are using this variable, it must be defined.


Base path of 3D shapes files, and must be defined because an absolute path is not usually used.


Base path of footprint library folders, and must be defined if an absolute path is not used in footprint library names.


Note also the environment variable KIPRJMOD is always internally defined by KiCad, and is the current project absolute path.

For instance, ${KIPRJMOD}/connect.pretty is always the connect.pretty folder (the pretty footprint library) found inside the current project folder.

If you modify the configuration of paths, please quit and restart KiCad to avoid any issues in path handling.

2.6. Selection of text editor

Before using a text editor to browse/edit files in the current project, you must choose the text editor you want to use.

Select Preferences → Set Text Editor to set the text editor you want to use.

2.7. Selection of PDF viewer

You may use the default PDF viewer or choose your own.

To change from the default PDF viewer use Preferences → PDF Viewer → Set PDF Viewer to choose the PDF viewer program, then select Preferences → PDF Viewer → Favourite PDF Viewer.

On Linux the default PDF viewer is known to be fragile, so selecting your own PDF viewer is recommended.

2.8. KiCad principles of use

In order to manage a KiCad project of schematic files, printed circuit board files, supplementary libraries, manufacturing files for photo-tracing, drilling and automatic component placement files, it is recommended to create a project as follows:

  • Create a working directory for the project (using KiCad or by other means).

  • In this directory, use KiCad to create a project file (file with extension .pro) via the "Create a new project" or "Create a new project from template" icon.

Use a unique directory for each KiCad project. Do not combine multiple projects into a single directory.

KiCad creates a file with a .pro extension that maintains a number of parameters for project management (such as the list of libraries used in the schematic). Default names of both main schematic file and printed circuit board file are derived from the name of the project. Thus, if a project called was created in a directory called example, the default files will be created:

Project management file.


Main schematic file.


Printed circuit board file.

Netlist file.


Various files created by the other utility programs.


Library file automatically created and used by the schematic editor containing a backup of the components used in the schematic.

3. Using KiCad manager

The KiCad Manager (kicad or kicad.exe) is a tool which can easily run the other tools (schematic and PCB editors, Gerber viewer and utility tools) when creating a design.

Running the other tools from KiCad manager has some advantages:

  • cross probing between schematic editor and board editor.

  • cross probing between schematic editor and footprint selector (CvPcb).

However, you can only edit the current project files. When these tools are run in stand alone mode, you can open any file in any project but cross probing between tools can give strange results.

3.1. Main window


The main KiCad window is composed of a project tree view, a launch pane containing buttons used to run the various software tools, and a message window. The menu and the toolbar can be used to create, read and save project files.

3.2. Utility launch pane

KiCad allows you to run all stand alone software tools that come with it.

The launch pane is made of the 8 buttons below that correspond to the following commands (1 to 8, from left to right):




Schematic editor.



Component editor and component library manager.



Board layout editor.



Footprint editor and footprint library manager.



Gerber file viewer. It can also display drill files.



Tool to build a footprint or a component from a B&W bitmap image to create logos.


Pcb Calculator

Tool to calculate track widths, and many other things.


Pl Editor

Page layout editor, to create/customize frame references.

3.3. Project tree view


Double-clicking on the Eeschema icon runs the schematic editor, in this case opening the file pic_programmer.sch.

Double-clicking on the Pcbnew icon runs the layout editor, in this case opening the file pic_programmer.kicad_pcb.

Right clicking on any of the files in the project tree allows generic file manipulation.

3.4. Top toolbar


KiCad top toolbar allows for some basic file operations:


Create a project file. If the template is found in kicad/template, it is copied into the working directory.


Create a project from a template.


Open an existing project.


Update and save the current project tree.


Create a zip archive of the whole project. This includes schematic files, libraries, PCB, etc.


Rebuild and redraw the tree view, sometimes needed after a tree change.

4. Project templates

A template facilitates the easy creation of a new project, based on a template definition. Templates may contain pre-defined board outlines, connector positions, schematic elements, design rules, etc. Complete schematics and/or PCBs used as seed files for the new project may even be included.

4.1. Using Templates

The File → New Project → New Project from Template menu will open the Project Template Selector dialog:


A single click on a template’s icon will load that template’s information, and a further click on the OK button creates the new project. The template files will be copied to the new project location and renamed to reflect the new project’s name.

After selection of a template:


4.2. Template Locations:

The list of available templates are gathered from the following sources:

  • System templates: <kicad bin dir>/../share/kicad/template/

  • User templates:

    • Unix: ~/kicad/templates/

    • Windows: C:\Documents and Settings\username\My Documents\kicad\templates

    • Mac: ~/Documents/kicad/templates/

  • When the environment variable KICAD_PTEMPLATES is defined there is a third tab, Portable Templates, which lists templates found at the KICAD_PTEMPLATES path.

4.3. Creating templates

The template name is the directory name under which the template files are stored. The metadata directory, in a subdirectory named meta, contains files which describe the template.

All files and directories in a template are copied to the new project path when a project is created using a template, except meta.

All files and directories which start with the template name will be renamed with the new project file name, excluding the file extension.

The metadata consists of one required file, and may contain optional files. All files must be created by the user using a text editor or previous KiCad project files, and placed into the required directory structure.

Here are project files for a raspberrypi-gpio template:


And the metadata files:


4.3.1. Required File:


HTML-formatted information describing the template.

The <title> tag determines the actual name of the template that is exposed to the user for template selection. Note that the project template name will be cut off if it’s too long. Due to font kerning, typically 7 or 8 characters can be displayed.

Using HTML means that images can be easily in-lined without having to invent a new scheme. Only basic HTML tags can be used in this document.

Here is a sample info.html file:

<!DOCTYPE HTML PUBLIC "-//W3C//DTD HTML 4.0 Transitional//EN">
<TITLE>Raspberry Pi - Expansion Board</TITLE>
<META NAME="GENERATOR" CONTENT="LibreOffice 3.6 (Windows)">
<META NAME="CHANGED" CONTENT="20121015;19015295">
<P>This project template is the basis of an expansion board for the
<A HREF="" TARGET="blank">Raspberry Pi $25
ARM board.</A> <BR><BR>This base project includes a PCB edge defined
as the same size as the Raspberry-Pi PCB with the connectors placed
correctly to align the two boards. All IO present on the Raspberry-Pi
board is connected to the project through the 0.1&quot; expansion
headers. <BR><BR>The board outline looks like the following:
<P><IMG SRC="brd.png" NAME="brd" ALIGN=BOTTOM WIDTH=680 HEIGHT=378
<P>(c)2012 Brian Sidebotham<BR>(c)2012 KiCad Developers</P>

4.3.2. Optional Files:


A 64 x 64 pixel PNG icon file which is used as a clickable icon in the template selection dialog.

Any other image files used by meta/info.html, such as the image of the board file in the dialog above, are placed in this folder as well.