KiCad Nightly Reference Manual
Copyright
This document is Copyright The KiCad Documentation Contributors. You may distribute it and/or modify it under the terms of either the GNU General Public License (http://www.gnu.org/licenses/gpl.html), version 3 or later, or the Creative Commons Attribution License (http://creativecommons.org/licenses/by/3.0/), version 3.0 or later.
Todas las marcas mencionadas en esta guía pertenecen a sus legítimos propietarios.
Contribuidores
Jean-Pierre Charras, Fabrizio Tappero, Jon Evans, Graham Keeth.
Traducción
Antonio Morales <[email protected]>, 2015
Realimentación
The KiCad project welcomes feedback, bug reports, and suggestions related to the software or its documentation. For more information on how to submit feedback or report an issue, please see the instructions at https://www.kicad.org/help/report-an-issue/
Software and Documentation Version
This user manual is based on KiCad 10.99. Functionality and appearance may be different in other versions of KiCad.
Documentation revision: 37fef10f.
Introducción
KiCad is an open-source software suite for creating electronic circuit schematics and printed circuit boards (PCBs). KiCad supports an integrated design workflow in which a schematic and corresponding PCB are designed together, as well as standalone workflows for special uses. KiCad also includes several utilities to help with circuit and PCB design, including a PCB calculator for determining electrical properties of circuit structures, a Gerber viewer for inspecting manufacturing files, and an integrated SPICE simulator for inspecting circuit behavior.
KiCad runs on all major operating systems and a wide range of computer hardware. It supports PCBs with up to 32 copper layers and is suitable for creating designs of all complexities. KiCad is developed by a volunteer team of software and electrical engineers around the world with a mission of creating free and open-source electronics design software suitable for professional designers.
The latest version of this documentation is available at https://docs.kicad.org.
System Requirements
KiCad is capable of running on a wide variety of hardware and operating systems, but some tasks may be slower or more difficult on lower-end hardware. For the best experience, a dedicated graphics card and display with 1920x1080 or higher resolution is recommended.
Please check the KiCad website for the latest system requirements: https://kicad.org/help/system-requirements/
Installing and Upgrading KiCad
First time setup
The first time you run a new major version of KiCad, a Welcome window will appear to ask you how to initialize your settings. Each major release of KiCad has its own configuration, so that you may run multiple KiCad versions on the same computer without the configurations interfering.
Configuration setup
You always have the option to start with default settings for the new version. If a previous version of KiCad is detected, you will have the option to import the settings from that version. The location of the previous configuration files is detected automatically, but you may override it to choose another location if desired.
Hotkey configurations are not imported from previous versions.
You can manually import hotkey configurations by using the Import Hotkeys… button on the Hotkeys page of Preferences,
then browsing to the .hotkeys file from the old version’s configuration directory.
If you do so, please note that this will replace the current version’s hotkey settings.
|
KiCad stores the settings files in a folder inside your user directory. Each KiCad version will use a different versioned subfolder. For KiCad 10, those folders are:
Windows |
|
Linux |
|
macOS |
|
Libraries setup
You also have options for how to initialize your symbol, footprint, and design block libraries.
If you are setting up KiCad for the very first time, you should select the first option, Start with the built-in KiCad libraries. This initializes your library tables to include all of the libraries that come with KiCad.
If you have used an older version of KiCad and are updating it to the newest version, and therefore already have a library setup that worked in the old version, you can instead the select the second option, Import tables from the previous version. In this case, it is recommended to also select the option Migrate built-in libraries to the latest version, which replaces references to the old-version built-in libraries with references to the updated libraries.
You also have the option to start with no libraries and do all of the configuration yourself. Refer to the Schematic Editor and PCB Editor documentation for details on how to manually configure libraries.
Depending on your system and how KiCad was installed, some options may not be available. KiCad may also not be able to locate any libraries installed on your system. In this case, you should ensure you have installed the libraries, or you can manually configure the libraries after completing setup.
| On some systems the KiCad libraries are installed as a separate package. |
The location of the default library table files depends on operating system and may vary based on installation location. Below are the defaults for each operating system:
Windows |
|
Linux |
|
macOS |
|
Updates & Privacy setup
You can also choose whether to be notified about updates to the KiCad application and to third party packages you may have installed through KiCad’s Plugin and Content Manager (plugins, themes, libraries, etc.). On Windows, you also have the option to enable anonymous crash reporting, which helps the KiCad team diagnose and fix critical issues in the application.
Migrating design files from previous versions
Modern versions of KiCad can open files created in earlier versions, but can only write files in the latest formats. This means that in general, there are no special steps to migrate files from a previous version besides opening the files. In some cases, the file extension for a file has changed from one KiCad version to the next. After opening these files, they will be saved in the new format with the new file extension. The old files will not be deleted automatically.
The schematic editor documentation describes several particular considerations for opening legacy schematics.
In general, files created or modified by one version of KiCad cannot be opened by older versions of KiCad. For this reason, it is important to keep backup copies of your projects when testing a new KiCad release, until you are confident that you will not need to use the older KiCad version anymore.
Using the KiCad project manager
The KiCad project manager is the window that opens when you start KiCad. The project manager creates and opens KiCad projects and launches the other KiCad tools:
-
the Schematic Editor
-
the Symbol Editor
-
the PCB Editor
-
the Footprint Editor
-
the Gerber Viewer
-
the Image Converter
-
the Calculator Tools
The KiCad project manager window is composed of a tree view on the left showing the files associated with the open project, and a launcher on the right containing shortcuts to the various editors and tools.
The tree view shows a list of the files inside the project folder. This includes the KiCad schematic and board design files as well as other files and folders in the project folder. If the project contains multiple schematic sheets, only the root sheet is shown in the tree view.
| Only files that KiCad understands how to open are displayed in the project tree view. |
Double-clicking on a file in the tree view will open it in the associated editor. Right-clicking on a file will open a context menu with some file manipulation commands.
If the project is part of a Git repository, the tree shows the version control status of each file. It also shows the current branch after the project name. Usually, the tree shows only the root sheet of the schematic. In a Git repository, the tree shows all the sheets, so that you can see the status of each sheet.
KiCad projects contain at least a project file, a schematic, and a board design. Schematics may contain multiple sheets, each in its own file, but a project can only contain a single board. KiCad expects the project file, schematic root sheet file, and board file to all have the same name.
The toolbar on the left side of the window provides shortcuts for common project operations:
|
Create a new project. |
|
Open an existing project. |
|
Create a zip archive of the whole project. This includes schematic files, libraries, PCB, etc. |
|
Extract a project zip archive into a directory. Files in the destination directory will be overwritten. |
|
Refresh the tree view, to detect changes made on the filesystem. |
|
Open the project working directory in a file explorer. |
Standalone mode
You can also run the KiCad editor tools in standalone mode, by launching them directly from your operating system’s application launcher rather than from the project manager. It is usually not recommended to run the tools in standalone mode, except for some specific situations where it is necessary, such as when importing projects from other EDA tools. When running in standalone mode, some project features are not available, including:
-
cross probing between the schematic editor and the board editor
-
design synchronization between the schematic and the board
Creating a new project
Most KiCad designs start with the creation of a project. When you create a new project, you always begin by choosing a project template, even if that template is the default, blank project template.
To create a new project, use the New Project… command in the File menu, click the New Project button in the top toolbar, or use the keyboard shortcut (Ctrl+N by default).
The right side of this dialog shows a list of all installed project templates. The Default template is always available for you to create an empty project. Clicking one of these templates will show the template’s description in a new panel. The left side of the dialog shows a list of your recently used project templates.
| Creating new project templates is covered in the Project Templates section. |
| Creating your own project templates is a good way to easily create new projects that are preconfigured with your preferred drawing sheets, design rules, PCB outlines, logos, etc. |
When you have chosen a template, click the OK button to create a new project from that template.
You will be prompted for a name to give your project. By default, a directory will be created for your project with the same name. For example, if you enter the name MyProject, KiCad will create the directory MyProject and the project file MyProject/MyProject.kicad_pro inside it.
If you already have a directory to store your project files in, you can uncheck the Create a new directory for the project checkbox in the New Project dialog.
| It is strongly recommended that you store each KiCad project inside its own directory. |
Once you select the name of your project, KiCad will create the following files inside the project directory:
|
KiCad project file. |
|
Main schematic file. |
|
Printed circuit board file. |
Other files may also be created, depending on the contents of the template.
Importing a project from another EDA tool
KiCad is able to import files created by some other software packages. Some software formats can be imported as complete projects. Others can only be imported as standalone schematics or boards, and must be manually linked together into a KiCad project. The following types of projects are supported:
| Source EDA Tool | File Extension(s) |
|---|---|
Altium Designer |
|
CADSTAR archive format |
|
Eagle 6.x or newer (XML format) |
|
EasyEDA (JLCEDA) Standard Backup |
|
EasyEDA (JLCEDA) Pro Project |
|
PADS ASCII Project |
|
gEDA / Lepton EDA Project |
|
To import a project from one of these tools, choose the appropriate option from the Import Non-KiCad Project submenu of the File menu.
Depending on the format, you will be prompted to select either a project, schematic, or a board file in the import file browser dialog. The imported schematic and board files should have the same base file name (e.g. project.sch and project.brd). Once the requested files are selected, you will be asked to select a directory to store the resulting KiCad project.
A greater number of formats can be imported as either schematics or boards, rather than complete projects. The following schematic formats can be imported into the Schematic Editor:
| Source EDA Tool | File Extension(s) |
|---|---|
Altium Designer |
|
Eagle (Autodesk) |
|
LTspice |
|
PADS Logic |
|
CADSTAR Schematic Archive |
|
gEDA / Lepton EDA |
|
EasyEDA (JLCEDA) Standard |
|
EasyEDA (JLCEDA) Professional |
|
Importing these schematic formats is explained in more detail in the Schematic Editor documentation.
The following PCB formats can be imported into the PCB Editor:
| Source EDA Tool | File Extension(s) |
|---|---|
Altium Designer |
|
Altium Circuit Maker |
|
Altium Circuit Studio |
|
Cadence Allegro |
|
CADSTAR PCB Archive |
|
Eagle (Autodesk) |
|
EasyEDA / JLCEDA Standard |
|
EasyEDA / JLCEDA Professional |
|
Fabmaster |
|
gEDA / Lepton EDA |
|
P-CAD 200x |
|
PADS (ASCII) |
|
Solidworks PCB |
|
Importing these PCB formats is explained in more detail in the PCB Editor documentation.
Project backups and autosave
KiCad can automatically create backups of your projects. When enabled, KiCad will automatically create backups of the entire current project in two situations:
-
When you manually save in any editor.
-
When there are unsaved changes after a few seconds of inactivity (an autosave).
You can enable and configure project backups in KiCad’s Project Backup preferences.
KiCad can create project backups in two ways: incremental backups or Zip archives.
Incremental backups
When configured for incremental backups, project backups are saved as incremental snapshots of project files.
You can view each of these snapshots in the Local History panel (View → Panels → Local History).
The Local History panel shows each snapshot event and when the snapshot was taken. If you hover over an event, a tooltip shows the files that changed in the snapshot.
To restore from a snapshot, right click the snapshot in the Local History panel and choose Restore Commit.
Behind the scenes, the incremental backup system uses a Git repository in a hidden .history folder. KiCad manages this Git repository automatically.
If you use a version control system to track your project’s changes, you may want to exclude the .history folder.
|
Zip archives
When configured for Zip archives, project backups are saved as a Zip archives of the project directory and its contents. Each backup is a separate Zip file.
You can restore from these archives by using the Unarchive tool or by manually extracting the archive and loading the project.
Saving and loading project archives
You can archive your project’s files into a zip archive with the Archive tool (File → Archive Project…).
You can also unarchive a project using the Unarchive tool (File → Unarchive Project…). When you unarchive a project into the currently loaded project directory, the project will be reloaded automatically to reflect any changes that were in the archived version of the project.
The archive tool saves the following files from your project folder into the archive:
|
KiCad design files |
|
Legacy KiCad design files |
|
3D models |
|
Gerber files |
|
Manufacturing files |
|
Netlists |
|
Python scripts |
|
Documentation files |
|
SPICE models |
|
IBIS models |
Version control with Git
KiCad has a built-in interface to the Git version control system. You can use it to record the history of a project, share the project with other designers, and get their changes. The Version Control panel gives access to the most frequent tasks: commit, push and get changes. The Advanced Git window gives access to history, branches, remotes, stashes and tags.
You do not need a separate Git program to use these tools. If you also use other Git programs, KiCad uses the same repository and settings.
Version control concepts
A Git repository holds the files of a project and a history of all the changes to them. The repository is a hidden .git folder in the project folder or in one of its parent folders. The project folder that you edit is the working folder.
When you save a schematic or a board, KiCad writes the file to the working folder. A save does not record a version. When you commit, Git records the saved state of the files that you select as a new version in the repository. Each commit has a summary, an author and a date. You can compare commits and return to a commit later.
A commit is local to your computer. A remote is a copy of the repository on a server or in a shared folder. Usually, the remote has the name origin. When you push, KiCad sends your commits to the remote. When you get changes, KiCad gets the commits of other designers from the remote and adds them to your project.
A branch is a separate line of commits. You can use a branch to try a design change without affecting the main line of the project. The current branch is the branch that your working folder shows.
A conflict occurs when you and another designer change the same file, and Git cannot combine the two changes. KiCad shows each conflict and lets you select the version to keep. For schematics and boards, KiCad can show the conflicts item by item. Refer to Resolving conflicts.
The Version Control panel commands correspond to these Git operations:
| KiCad command | Git operation |
|---|---|
Commit |
|
Commit and Push |
|
Get Changes |
|
Fetch (Advanced Git window) |
|
Undo Last Commit |
|
Discard Changes |
|
Stash Changes… |
|
The Git integration has these limits:
-
KiCad cannot read or write files that the repository keeps in Git LFS. If a project uses Git LFS, KiCad does not commit, get changes or switch branches. Use a different Git program for that repository.
-
KiCad does not push tags.
-
KiCad cannot rebase, cherry-pick, revert or bisect. If another program starts one of these operations, KiCad can only abandon it.
-
KiCad cannot rename branches or remotes, and it cannot delete a branch on the remote.
-
KiCad does not sign commits or tags.
-
KiCad cannot make a repository on a server. Make the repository with the tools of your server, then add it to the project as a remote.
Where to find the version control tools
The version control tools are in these locations:
-
The Version Control panel is in the project manager, the Schematic Editor and the PCB Editor. In the project manager, the panel is below the project files tree and is visible by default. In the editors, the panel is hidden by default. To show or hide the panel, click View → Panels → Version Control.
-
The project files tree shows the version control status of each file and the name of the current branch. Right click in the tree to show the Version Control menu. Use this menu to add version control, set the default remote and show the history. You can also switch branches and disable the integration for the project.
-
File → Clone Project from Repository… copies a project from a remote. Refer to Cloning a project from a repository.
-
The Advanced Git window has the tools for history, branches, remotes, stashes and tags.
-
Tools → Compare Project Branches… shows the files that are different between two branches. Refer to Comparing project branches.
-
The Version Control page of the Preferences dialog enables or disables the Git integration for all projects.
KiCad finds an existing repository automatically. If the project folder is in a Git repository, the tools are available when you open the project.
The Version Control panels in the project manager and in the editors use the same repository. A commit in one panel updates the other panels. For the tasks that are specific to each editor, refer to the Schematic Editor manual and the PCB Editor manual.
Putting a project under version control
You can put a project under version control in two ways:
-
If the project is on a server, clone it. Refer to Cloning a project from a repository.
-
If the project is on your computer, add version control to it. Refer to Adding version control to an existing project.
Before your first commit, KiCad asks for your name and email address if Git does not have them. Refer to Setting the commit author.
Cloning a project from a repository
To make a copy of a project that is in a remote repository:
-
Click File → Clone Project from Repository…. The Clone Project from Git Repository dialog opens.
-
In Location, type or paste the address of the repository. If the clipboard holds a repository address, KiCad pastes it for you. The address determines the connection type:
-
An address that starts with
https://uses HTTPS. -
An address that starts with
ssh://, or that has the formuser@host:path, uses SSH. -
A folder path uses a local connection, which needs no authentication.
-
-
Type the authentication data that the server needs:
-
For HTTPS, type your User name and your Password. Many servers need a personal access token in place of a password.
-
For SSH, select SSH private key and select your private key file. If KiCad finds a key in your SSH configuration or
.sshfolder, it selects that key automatically. If the key has a passphrase, type it in SSH key password.
-
-
Optionally, click Test Connection to make sure that KiCad can connect to the repository.
-
Click OK.
-
Select the folder for the project, then click Save.
KiCad copies the repository and opens the first project that it finds in it. If the repository has no KiCad project, KiCad tells you where it put the files.
| The File → Clone Project from Repository… menu item is available only when Enable Git tracking is selected in the Version Control preferences. |
Adding version control to an existing project
To make a new repository for a project that is not under version control:
-
In the project files tree, right click the project.
-
Click Version Control → Add Project to Version Control…. KiCad makes a repository in the project folder. The Set default remote dialog opens.
-
If you have a remote repository for the project, type its address and the authentication data. The fields are the same as in the clone dialog. Then click OK. KiCad connects to the remote and gets its branches.
-
If you do not have a remote repository yet, click Skip. You can add a remote later with Version Control → Configure Default Remote… or on the Remotes page.
KiCad does not make a commit. Your first commit starts the history of the project. If the remote has one branch with a different name, for example main, your first commit goes on that branch.
When KiCad makes a repository, it also adds these files to the project folder:
-
A
.gitignorefile that tells Git to ignore backups, autosave files, lock files, the footprint cache and the.kicad_prlfile. KiCad makes this file only if the project folder does not have one. -
A
.gitattributesfile that tells Git to use the KiCad merge tool for schematics, boards and libraries. Refer to Merging KiCad files with other Git programs.
Commit these files with your first commit.
The .kicad_prl file holds settings for your computer only, such as the visible layers.
Do not commit it.
|
Configuring the default remote
The default remote is the remote named origin. KiCad pushes to it and gets changes from it, unless the current branch tracks a different remote.
To change the address or the authentication data of the default remote:
-
In the project files tree, right click the project.
-
Click Version Control → Configure Default Remote….
-
Change the address or the authentication data, then click OK.
To add or remove other remotes, use the Remotes page of the Advanced Git window.
Credentials and SSH keys
If a server rejects your user name, password or key, the Git Authentication Required dialog opens. The dialog shows the address of the remote and the reason for the rejection.
-
For an HTTPS remote, type your Username and your Password / token.
-
For an SSH remote, select the SSH key and type the Key passphrase. If the key has no passphrase, leave the passphrase empty. If the address of the remote includes a user name, for example
git@, you cannot change the user name. -
To keep the password or the passphrase, select Save credentials. This option is selected by default.
-
Click OK. KiCad tries the operation again.
KiCad keeps saved credentials in the Windows Credential Manager, in the macOS Keychain, or in the secret storage of your Linux desktop. To remove saved credentials, use the tool of your operating system.
For an SSH remote, KiCad tries the keys in this order:
-
The keys in your SSH agent.
-
The key that you selected for the project.
-
The key that connected to this remote the last time.
-
The keys that your SSH configuration file sets with
IdentityFilefor the server. -
The keys with the standard names in your
.sshfolder, and up to four other keys in that folder.
You can select a .pub file in place of a private key. KiCad then uses the private key that is next to it.
Verifying a server
The first time that you connect to an SSH server, the Verify Server dialog opens. The dialog shows the key fingerprint of the server.
-
Compare the fingerprint with the fingerprint that your server administrator or your Git service publishes.
-
If the fingerprints are the same, click Connect. KiCad adds the key of the server to your
known_hostsfile. -
If the fingerprints are different, click Cancel.
If the key of a known server changes, KiCad does not connect and shows an error. A changed key can show that a different computer uses the address of the server.
Speak to your server administrator before you remove the old key from your known_hosts file.
KiCad does not remove or replace keys in this file.
|
Repositories that belong to a different user
Git does not open a repository that belongs to a different user account on your computer. For example, this occurs if you copied the project from a different computer, or if an administrator made the folder.
The Version Control panel reports that the repository belongs to another user. It also shows a git config --global --add safe.directory command.
-
Click Copy to copy the command.
-
Run the command in a terminal.
-
Close the project and open it again.
KiCad does not show this message for a repository that contains your home folder. It ignores that repository and shows that the project is not under version control.
Setting the commit author
Each commit records the name and email address of its author. KiCad uses the name and email address in the Git settings of the repository. If the repository has no name or email address, KiCad uses your global Git settings.
If Git has no name and email address for you, the Set Author dialog opens before your first commit. The dialog shows the author from the Version Control preferences if you set one there. Type or check your Name and Email, then click OK. KiCad saves them in the settings of the repository.
To change the author of a repository later, click the gear button in the Version Control panel. Then click Set Author….
Version control status in the project tree
When a project is in a Git repository, the project files tree shows the name of the current branch after the project name. The tree also shows all the schematic sheet files, so that you can see the status of each sheet. An icon next to each file shows its status:
| Icon | Status | Meaning |
|---|---|---|
|
Unchanged |
The file is the same as in the last commit, and the remote has no newer version. |
|
Modified |
The file has changes that are not committed. |
|
New |
The file is not in the repository yet. Commit it to add it. |
|
Deleted |
The file was deleted, and the deletion is not committed. |
|
Committed, not pushed |
The file has committed changes that are not on the remote. Push them to share them. |
|
Changed on the remote |
The remote has a newer version of the file. Use Get Changes to get it. |
|
Conflict |
The file has a conflict that is not resolved. |
KiCad checks the remote for new commits at an interval that you set in the Version Control preferences. This check does not change your files. If the check fails, KiCad shows a warning in the status bar of the project manager.
The Version Control panel
The Version Control panel shows the files that you changed and lets you commit, push and get changes.
The panel has these areas, from top to bottom:
-
The name of the current branch, next to Commit to. To switch to a different branch, use the project files tree or the Branches page of the Advanced Git window.
-
The Recent messages list. Select a message to use it again.
-
The gear button. It opens a menu with Open Advanced Git Window… and Set Author….
-
The summary and the description of the commit. When 10 or fewer characters remain before the 72-character limit, a number shows how many you can add.
-
The commit options. Refer to Commit options.
-
The Show Diff button. It shows the changes to the selected file.
-
A status line. It tells you what the project needs next, or why a command is not available.
-
The Undo Last Commit button, if you can undo the last commit. Refer to Undoing the last commit.
-
The list of changed files, with a check box for each file and its status: Modified, New, Deleted or Conflict. The panel shows only the files in the project folder. It does not show untracked backups, autosave files, lock files and other temporary files. It shows these files if Git already tracks them.
-
The Commit button and the Get Changes button.
-
The History… link, which opens the History page of the Advanced Git window.
The Commit button changes to Amend when you amend the last commit. It changes to Push when you have commits that are not on the remote and no files to commit.
Committing changes
To commit changes:
-
In the list of changed files, select the check box of each file that you want to commit. KiCad selects new files automatically. Clear the check box of a file that you do not want to commit.
-
Type a summary of the changes. Optionally, type a longer description.
-
Click Commit. You can also press Ctrl+Enter while you type in the summary or the description.
If the Schematic Editor or the PCB Editor has unsaved changes, the Unsaved Changes dialog opens:
-
Click Save and Review to save the editors. KiCad updates the list of changed files and does not commit. Examine the list, then click Commit again.
-
Click Commit Anyway to commit the files as they are on disk now. The unsaved changes are not in the commit.
-
Click Cancel to stop.
After the commit, the Commit button changes to Push if the project has a remote.
Committing and pushing
To commit and push in one step, click the arrow on Commit, then click Commit and Push. You can also press Ctrl+Shift+Enter while you type in the summary or the description.
To push commits that you made before, click Push.
If another designer pushes changes first, KiCad asks whether to get their changes and push again. Click Yes to get the changes, resolve any conflicts, and push.
| On macOS, use Cmd+Return and Cmd+Shift+Return. |
Commit options
Amend last commit: Replaces the last commit with a new commit that includes the selected files and the new message. KiCad shows this option only if the last commit is not on the remote yet. When you select it, KiCad loads the message of the last commit if the summary is empty.
Sign off (add Signed-off-by): Adds a Signed-off-by line with your name and email address to the commit message.
Create a new branch: Makes a new branch, switches the project to it, and commits to it. Type the name of the branch in the field below the option. If the commit fails, KiCad deletes the new branch.
Undoing the last commit
You can undo the last commit if it is not on a remote yet. When this is possible, the Undo Last Commit button shows in the Version Control panel.
Click Undo Last Commit. KiCad removes the commit but keeps its changes in your files. The changed files reappear in the list. The panel also shows the commit message. You can then change the files or the message and commit again.
If the commit is already on a remote, KiCad does not undo it, because other designers can have it. Make a new commit that corrects the problem.
Getting changes from the remote
To get the commits of other designers:
-
Commit or stash your changes. KiCad does not get changes while you have uncommitted changes. This prevents the changes from the remote from replacing your work.
-
Save or close the editors that have unsaved changes.
-
Click Get Changes.
KiCad gets the commits from the remote and adds them to the current branch. If you have local commits that are not on the remote, KiCad merges the two lines of commits and makes a merge commit. If the Git setting pull.rebase is true, KiCad places your commits after the remote commits without a merge commit. If the open editors show files that changed, they load the new versions.
While the transfer runs, the Get Changes button changes to Cancel. Click Cancel to stop the transfer.
If the remote has new commits, the status line tells you to use Get Changes. The project files tree shows the
icon for the files that changed.
Resolving conflicts
A conflict occurs when you and another designer change the same file, and Git cannot combine the two changes. For example, you change the value of a resistor and commit. At the same time, a colleague changes the value of the same resistor and pushes. When you get changes, the two values are in conflict.
When you get changes, KiCad combines changes to a board item by item. For schematics, symbol libraries and footprints, a file that both of you changed is always a conflict. The merge tool can then combine the changes to a schematic item by item.
KiCad shows the Resolve Conflict dialog for each file that has a conflict. The dialog tells you what happened to the file on each side.
Select one of these choices, then click OK:
-
Open the merge tool: Shows each conflict in the file and lets you select the version to keep. The merge tool is available for schematics and boards.
-
Keep my version: Keeps your version of the file and discards the changes from the remote.
-
Use the remote version: Uses the version from the remote and discards your changes to the file.
If a file was deleted or added on one side, the dialog shows choices to keep the file or to delete it.
The Resolve Merge Conflicts dialog shows the conflicts in a schematic or a board:
-
In the Conflicts list, select a conflict. KiCad highlights the item.
-
Under Pick a side, select the version to keep:
-
Ours: your version.
-
Theirs: the version from the remote.
-
Ancestor: the version before the two changes.
-
Merge both changes: KiCad combines the two changes. If both sides changed the same property, KiCad keeps your value. When this choice is available, it is selected by default.
-
-
Do steps 1 and 2 for each conflict.
-
Click Apply.
If you click Cancel in the merge tool, the Resolve Conflict dialog opens again for that file.
After you resolve all the files, KiCad completes the merge. It copies each version it replaces to a merge-<date and time> folder in the project backup folder. The status line shows the name of this folder.
| If an older version of KiCad saved one of the files, the merged file uses the current file format. You cannot open the merged file in the older version of KiCad. |
If you click Cancel in the Resolve Conflict dialog, KiCad stops and your files do not change. If you already resolved a file in the merge tool, KiCad asks you to confirm, because it discards that result. Click No to go back to the Resolve Conflict dialog.
If the Git setting pull.rebase is true and a conflict occurs, KiCad asks if it can make a merge commit. KiCad can resolve conflicts only with a merge.
| A merge, rebase, cherry-pick or revert can start outside KiCad or stop before it completes. Then the Get Changes button changes to Abandon Merge, Abandon Rebase, Abandon Cherry-pick or Abandon Revert. Click it to go back to the last commit. This discards the changes that the operation made to your files. To complete the operation, use the program that started it. |
Examining and discarding the changes to a file
To see what changed in a file, select the file in the list and click Show Diff. You can also double click the file. For schematics and boards, the Compare Files dialog opens and shows the changed items. For text files, KiCad shows the changed lines.
Right click a file in the list to show these commands:
-
Show History for This File: Opens the History page of the Advanced Git window with only the commits that changed the file.
-
Discard Changes: Removes your changes to the file after you confirm. For a file that is in the repository, KiCad replaces it with the version of the last commit. For a new file, KiCad moves it to the trash. For a file with a conflict, KiCad keeps the version that the project had before you got changes.
Save or revert the changes in the open editors before you discard a file. If an editor has unsaved changes, KiCad does not discard the file.
The Advanced Git window
The Advanced Git window has all the version control tools for the project. Use one of these methods to open it:
-
Click the gear button in the Version Control panel and then click Open Advanced Git Window….
-
Click History… in the Version Control panel.
-
In the project files tree, right click and then click Version Control → Version History….
KiCad opens only one Advanced Git window at a time.
The top of the window shows the repository and the current branch. To switch branches, select a branch in the Branch list. The Fetch, Pull and Push buttons are also at the top:
-
Fetch gets the commits from the remote but does not change your files. After a fetch, the History and Branches pages show the commits on the remote.
-
Pull is the same as Get Changes in the Version Control panel.
-
Push sends your commits to the remote.
Use the list on the left to select a page: Changes, History, Branches, Remotes, Stashes, Tags or Repository.
Changes page
The Changes page has the same controls as the Version Control panel, in a larger layout. The commit message is the same in the panel and on this page. When you change it in one location, KiCad changes it in the other location.
The summary at the right tells you how many files the commit includes and how many lines change. When you select a file, KiCad shows its changes below the list:
-
For a schematic or a board, KiCad shows the version in the last commit and your version side by side. Colors show the added, removed and modified items. Turn the mouse wheel to zoom, and drag to move the view. The two sides move together.
-
For a text file, KiCad shows the changed lines.
-
For symbol libraries and footprints, double click the file to open the Compare Files dialog.
History page
The History page shows the commits of the project, with the newest commit first.
-
Type in the search field to find commits by summary, author, email address or commit identifier.
-
Select a branch in the list to show only the commits of that branch. All Branches shows the commits of all branches.
-
Show refs shows the branches and tags of each commit in the Refs column.
Select a commit to see its message, its parent commits and the files that it changed. Select a file to see its changes, as on the Changes page. Double click a commit or a file to open the Compare Files dialog.
When you open the page with Show History for This File, it shows only the commits that changed that file. Click Show All Commits to show all the commits again.
Right click a commit to show these commands:
-
Restore This Version: Makes the project files the same as in the selected commit. KiCad records the restoration as a new commit to preserve the history. Files outside the project folder do not change. Commit or stash your changes before you restore a version.
-
Amend Last Commit…: Opens the Changes page in amend mode with the message of the last commit. This command is available only for the last commit of the current branch, and only if that commit is not on the remote.
Branches page
The Branches page shows the local branches and the branches on the remote. The Status column shows current for the current branch and remote for the branches on the remote. Type in the search field to find a branch by its name.
Select a branch to see its last commit. The details show how many commits it is ahead of or behind the branch it tracks.
To switch the project to a different branch, double click a local branch. KiCad asks you to confirm, then replaces the project files with the version on that branch. Commit or stash your changes before you switch.
To make a new branch:
-
Select the branch to start from. You can select a local branch or a branch on the remote.
-
Click New Branch….
-
Type the name of the new branch, then click OK.
KiCad makes the branch but does not switch to it. To switch to it, double click it. When you push the branch for the first time, KiCad makes it on the remote.
To delete a local branch, select it and click Delete Branch. If the branch has commits that are not on the current branch, KiCad tells you how many commits you lose.
Force Push replaces the current branch on the remote with your local branch.
| Force Push deletes the commits that are only on the remote. Other designers lose these commits. Use it only if you know that nobody needs those commits. |
Remotes page
The Remotes page shows the remotes of the repository and their addresses. Select a remote to see the time of the last fetch.
-
To add a remote, click Add Remote…, type a Name and a URL, then click OK.
-
To change the address of a remote, select it and click Edit URL….
-
To remove a remote, select it and click Remove Remote. This does not change the repository on the server.
Stashes page
A stash saves your uncommitted changes and removes them from the working folder. Use a stash when you must get changes or switch branches, but your work is not ready for a commit.
To stash your changes:
-
Click Stash Changes…. If the editors have unsaved changes, KiCad asks you to save them first.
-
Optionally, type a description.
-
Click OK.
A stash includes only the files that are already in the repository. New files that you never committed stay in the working folder.
To get your changes back, select the stash and click one of these buttons:
-
Apply Stash: Puts the changes back in the working folder and keeps the stash.
-
Pop Stash: Puts the changes back in the working folder and removes the stash.
Before you apply a stash, commit or discard your current changes. If the stash conflicts with the current files, KiCad keeps it and leaves your files unchanged.
Drop Stash deletes the stash. You cannot get a dropped stash back.
Tags page
A tag is a name for a commit, for example the commit that you sent to fabrication.
To make a tag on the current commit:
-
Click Create Tag….
-
Type a Tag name.
-
Optionally, type a Message. A tag with a message records the author and the date of the tag.
-
Click OK.
Tags are local. KiCad does not push them to the remote.
To see the project as it was at a tag, select the tag and click Check Out. The project then shows an old version and is not on a branch. You cannot commit or push in this state from the Version Control panel. To go back, double click a branch on the Branches page.
To delete a tag, select it and click Delete Tag.
Repository page
The Repository page shows the name and the email address that KiCad uses for your commits in this repository. To change them, click Edit Author…. The change applies only to this repository.
Comparing project branches
The Compare Branches dialog shows the files that are different between two branches, tags or commits. To open it, click Tools → Compare Project Branches….
When the dialog opens, Head ref shows the current branch. Base ref shows main or master if that branch is not the current branch. If it is the current branch, Base ref shows the remote branch that the current branch tracks.
-
In Base ref, select or type the older branch, tag or commit.
-
In Head ref, select or type the newer branch, tag or commit. You can type any name that Git accepts, for example
origin/main,v3.3or a commit identifier. -
Click Compare.
The list shows each changed file’s repository path and status. It also shows the old path for renamed or copied files. The comparison uses only committed files. Changes in your working folder are not included.
Double click a schematic, board, symbol library or footprint to open the Compare Files dialog for that file.
| The Compare Branches dialog shows the files of the whole repository, not only the files of the project. |
Merging KiCad files with other Git programs
When KiCad adds version control to a project or clones a project, it configures the repository for other Git programs. Then these programs can merge KiCad files item by item. Without this configuration, Git merges schematics and boards line by line. A conflict can then produce a file that KiCad cannot open.
KiCad makes these changes:
-
It adds lines to the
.gitattributesfile of the project. These lines connect.kicad_sch,.kicad_pcb,.kicad_symand.kicad_modfiles to the KiCad merge drivers. KiCad does not change lines that are already in the file. -
It adds the KiCad merge drivers and the KiCad merge tool to the Git settings of the repository. These settings point to the
kicad-cliprogram of the KiCad installation that made them. KiCad does not change settings that are already present.
With this configuration, git merge and git pull merge KiCad files item by item. If items are in conflict, Git keeps your version of those items and marks the file as conflicted. Git does not write conflict markers into the file. You can still open the file in KiCad.
To resolve the conflicts, run git mergetool. For schematics and boards, the Resolve Merge Conflicts dialog opens. Select a side for each conflict as described in Resolving conflicts, then click Apply. Git then marks the file as resolved, and you can commit the merge.
The configuration is in the repository on your computer only.
Other clones of the repository need the same configuration.
KiCad cannot add this configuration to a clone that another program made.
For such a clone, copy the merge.kicad-, mergetool.kicad. and merge.tool settings from a clone that KiCad made.
|
If you move or update KiCad, the merge driver settings can point to an old kicad-cli program.
Correct the merge.kicad-*.driver and mergetool.kicad.cmd settings in the repository configuration.
|
Disabling the Git integration
To disable the Git integration for one project:
-
In the project files tree, right click the project.
-
Click Version Control → Disable Git Integration.
KiCad then does not show the status of files and does not use the repository for this project. The repository and its history do not change, so you can continue to use other Git programs with the project. To enable the integration again, click Version Control → Enable Git Integration.
To disable the Git integration for all projects, clear Enable Git tracking in the Version Control preferences.
Ficheros y directorios en KiCad
KiCad crea y utiliza archivos (y directorios) con las siguientes extensiones de archivos específicas para la edición de esquemas y placas.
Many of these files include important design information, especially the project file (.kicad_pro), the schematic file(s) (.kicad_sch), and the board file (.kicad_pcb). Other files may also be necessary. Such files should always be included when distributing the project. Some files are not necessary to distribute with the project, such as the project-local settings file (.kicad_prl) or the fp-info-cache file. Files that are unnecessary to distribute are noted in the table below.
Project files
|
Project file, containing settings that are shared between the schematic and PCB |
|
Legacy (KiCad 5.x and earlier) project file.
Can be read and will be converted to a |
Schematic editor files and folders
|
Schematic files, containing all symbol and connection information. |
|
Schematic symbol library file, containing the symbol descriptions: graphic shape, pins, fields. This is a packed library, i.e. all of the symbols in the library are in a single file. This can also be an individual symbol in an unpacked library,
where the library is a folder containing individual |
|
Schematic symbol library folder.
The folder itself is the library, and contains individual |
|
Simulator workbook file containing SPICE simulation setup information. |
|
Legacy (KiCad 5.x and earlier) schematic file.
Can be read and will be converted to a |
|
Legacy (KiCad 5.x and earlier) schematic library file. Can be read but not written. |
|
Legacy (KiCad 5.x and earlier) schematic library documentation. Can be read but not written. |
|
Legacy (KiCad 5.x and earlier) schematic component library cache file.
Required for proper loading of a legacy schematic ( |
|
Symbol library table: list of symbol libraries available in the schematic editor. |
|
Design block library table: list of design block libraries available in the schematic editor. |
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. |
|
Design rules file, containing custom design rules for a certain |
|
Legacy (KiCad 4.x and earlier) board file. Can be read, but not written, by the current board editor. |
|
Legacy (KiCad 4.x and earlier) footprint library file. Can be read by the footprint or the board editor, but not written. |
|
Footprint library table: list of footprint libraries available in the board editor. |
|
Cache to speed up loading of footprint libraries. Does not need to be distributed with the project or put under version control. |
Common files
|
Local settings for the current project; helps KiCad remember the last used settings such as layer visibility or selection filter. Does not need to be distributed with the project or put under version control. |
|
Page layout (drawing border and title block) description file. |
|
Jobset definition file containing output jobsets. |
|
Design block library folders. The folder itself is the library. Design blocks can contain both schematic and layout fragments. |
|
Design block folder for defining a reusable design.
The folder is the design block,
and contains a |
|
Netlist file created from the schematic, and read by the board editor. Note that the recommended workflow for transferring information from the schematic to the board does not require the use of netlist files. |
|
Association between components used in the schematic and their footprints.
It can be created by the Board Editor and imported by the Schematic Editor.
Its purpose is to import changes from the board to the schematic, for users
who change footprints in the Board Editor (for instance using Exchange
Footprints command) and want to import these changes back to the schematic.
Note that the
recommended
workflow for transferring information from the board to the schematic does not
require the use of |
Fabrication and documentation files
|
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. |
Storing and sending KiCad files
KiCad schematic and board files contain all the schematic symbols and footprints used in the design, so you can back up or send these files by themselves with no issue. Some important design information is stored in the project file (.kicad_pro), so if you are sending a complete design, make sure to include it.
Some files, such as the project-local settings file (.kicad_prl) and the fp-info-cache file, are not necessary to send with your project. If you use a version control system such as Git to keep track of your KiCad projects, you can add these files to the list of ignored files so that they are not tracked.
Paths and libraries configuration
In KiCad, one can define paths using a path variable. A few path 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 (e.g. when you transfer a project to a different computer), and also when one base path is shared by many similar items. Consider the following which may be installed in varying locations:
-
Schematic symbol libraries
-
Footprint libraries
-
3D model files used in footprint definitions
For instance, the path to the connect.pretty footprint library, when using the KICAD10_FOOTPRINT_DIR path variable, would be defined as ${KICAD10_FOOTPRINT_DIR}/connect.pretty.
The Preferences → Configure Paths… menu allows you to define paths for some built-in KiCad path variables, and add your own path variables to define personal paths, if needed.
KiCad will automatically resolve versioned path variables from
older versions of KiCad to the value of the corresponding variable from
the current KiCad version, as long as the old variable is not explicitly
defined itself. For example, ${KICAD9_FOOTPRINT_DIR} will
automatically resolve to the value of ${KICAD10_FOOTPRINT_DIR} if there
is no KICAD9_FOOTPRINT_DIR variable defined.
|
KiCad path variables
|
Base path of KiCad’s standard 3D footprint model library files. |
|
Location for plugins, libraries, and color themes installed by the Plugin and Content Manager. |
|
Base path of KiCad’s standard footprint library files. |
|
Base path of KiCad’s standard symbol library files. |
|
Location of KiCad’s standard project template library files. |
|
Location of personal project templates. |
|
Location of personal simulation model libraries. This variable is not defined by default. |
|
Absolute path to the current project directory. This variable is set automatically and cannot be redefined. |
Paths set in the Configure Paths dialog are internal to KiCad and are not visible as environment variables outside of KiCad. They are stored in KiCad’s user configuration files.
Paths can also be set as system environment variables outside of KiCad, which will override any settings in the user’s configuration.
| You cannot override a system environment variable that has been set outside of KiCad by using the Configure Paths dialog. Any variable that has been set externally will be shown as read-only in the dialog. |
Note also that the path variable KIPRJMOD is always internally defined by KiCad, and expands to the current project absolute path. For instance, ${KIPRJMOD}/connect.pretty is always the connect.pretty folder (the footprint library) inside the current project folder. The KIPRJMOD variable cannot be changed in the Configure Paths dialog or overridden by an external environment variable.
Advanced environment variables
Some advanced environment variables can be set to customize where KiCad expects certain files to be located. By default, these locations are set based on your platform, but they can be overridden by system environment variables. These variables are not shown in the Configure Paths dialog and cannot be used in path substitutions.
Changing these variables will not result in KiCad moving any files from the default location to the new location, so if you change these variables you will need to copy any desired settings or files manually.
|
Base path of KiCad configuration files. Subdirectories will be created within this directory for each KiCad minor version. |
|
Base path of KiCad user-modifiable documents, such as projects, templates, Python scripts, libraries, etc. Subdirectories will be created within this directory for each KiCad minor version. This directory is provided as a suggested user data location, but does not need to be used. |
|
Base path of KiCad stock data, including default libraries. The data in this directory is managed by the KiCad installer or system package manager, and is not intended for user-writeable data. |
| If you modify the configuration of paths, please quit and restart KiCad to avoid any issues in path handling. |
Libraries configuration
The Preferences → Manage Symbol Libraries… menu lets you manage the list of symbol libraries (symbol library table).
Likewise, use the Preferences → Manage Footprint Libraries… menu to manage the list of footprint libraries (footprint library table).
For each type of library (symbol and footprint), there are 2 library tables: global and project specific. The global library table is located in the user configuration directory and contains a list of libraries available to all projects. The project-specific library table is optional and contains a list of libraries specific to the project. It is located in the project directory.
Jobsets
KiCad lets you configure a list of outputs that are all generated with a single click. The list of output jobs and the destinations where they will be saved is called a jobset. For example, a jobset might contain jobs to generate Gerber files, assembly data, a bill of materials, PDF plots of the schematic and PCB, while also running ERC and DRC checks, with all of the outputs saved to a compressed archive. The full list of available jobs is given below.
Each job in a jobset defines a single type of generated output, such as a bill of materials or a set of Gerbers. A job can be configured in the same way as if the output was manually generated from the schematic or board editor. The configuration for each job is stored in the jobset and remembered when you load the jobset later. Jobs are configured individually, so if you include the same type of job multiple times in a single jobset, each job will have its own independent configuration. For example, this lets you generate PDF outputs in color as well as black and white.
In addition to the jobs, jobsets also contain destinations, which define a list of jobs to run and how to store their outputs. A jobset destination can simply store the chosen jobs' output files in a specified location, or it can add the output files to a compressed archive. Each jobset destination can select a different subset of jobs from the full list of jobs in the jobset. You can run each jobset destination individually or run all jobset destinations at once. As an example, you could set up one jobset destination that generates PDFs of the board and schematic and copies them to an external location, while another destination generates the fabrication files and compresses them in a zip archive to send to the board manufacturer.
Projects can have multiple jobsets, with each jobset defining a different list of jobs and output configurations. Each jobset is stored in a .kicad_jobset file, which can be specific to a single project, copied between projects, or even stored in a central location and shared between projects.
To use a jobset, first create a new jobset file in the KiCad project manager (File → New Jobset File…) and choose a name and location for it. Alternatively, you can open an existing jobset file with File → Open Jobset File…. Jobset files that are stored in the project directory are considered part of the project and are displayed in the project file tree. You can open a jobset file in the project file tree by double clicking on it.
Once you create or open a jobset, it is displayed in a new tab in the project manager. The list of jobs is shown in the middle and the list of jobset destinations is shown on the right. New jobsets will not contain any jobs, but a destination is automatically created to save outputs to a folder. When you make changes to a jobset, you can save the changes by clicking the Save Jobset button.
Defining jobs
To add a new job, click the
button under the Jobs list. In the Add New Job dialog that appears, select the desired type of job. You can filter which types of jobs are shown in the list by typing in the Filter textbox at the bottom.
When you select a job and press OK, the settings dialog for that type of output will appear. Each job settings dialog provides the same options you would have if you manually generated that type of output from the schematic or board editor.
Output filenames and paths specified in job settings are relative to the jobset destination folder or archive root. You can use certain text variables, like ${PROJECTNAME}, ${CURRENT_DATE}, and project text variables.
|
When you accept the job settings dialog, the job is added to the list of jobs, where you can optionally change the new job’s description from its default. To change a job’s description or settings later, right click the job in the list and select Edit Job Description or Edit Job Settings…. Double clicking on a job also edits its settings. To remove a job, select the job and click the
button. To reorder the list, select a job and move it up or down using the
or
buttons.
Defining jobset destinations
You cannot generate any outputs from a jobset until you add a jobset destination. One destination is created automatically when a jobset is created, but you can add as many destinations as you need.
To add a jobset destination, click the
button under the Destinations list. When the Add New Destination dialog appears, select a type of destination:
-
Archive saves the outputs generated by the jobs in a compressed zip archive.
-
Folder saves the outputs generated by the jobs uncompressed in a folder.
Once you have selected a type of output, the Destination options dialog appears.
Here you can select which jobs will be run as part of this jobset destination, as well as the folder or archive name that will be used to store them. By default all jobs are enabled. You can also set a description for the destination to be displayed in the Destinations list. The output path controls where the files generated by the jobs will be saved. The path here can be absolute or relative to the project directory, and it can use path variables or certain text variables (${PROJECTNAME}, ${CURRENT_DATE}, and project text variables). Filenames defined in job configurations are relative to the jobset destination directory or archive root.
When you click OK in this dialog, the new jobset destination is added to the Destinations list. You can modify an existing jobset destination by clicking its
button, or remove it by clicking its
button.
After configuring your jobs and destinations, you can generate an individual set of outputs by clicking the Generate button for the desired destination. You can run all destinations at once by clicking the Generate All Destinations button.
If a jobset destination runs and generates its outputs successfully, a blue check is shown that indicates the last run was successful. If a jobset destination fails to complete successfully, a red exclamation point is shown to indicate the run was not successful. Clicking on the success/failure indicator will display the Jobset Run Log dialog, which displays the status of each job in the jobset destination. Clicking on a specific job will display the logged output from that job, if there is any.
After a jobset destination runs successfully, you can click the destination’s Open Output button to open a file browser in the destination location. This button is disabled if the jobset destination has not run or hasn’t successfully finished.
Jobset destination details
When jobs run, output files are initially generated in a temporary folder. After all jobs in a jobset destination are completed, the output files are moved from the temporary folder to the folder or archive specified by the jobset destination. None of the outputs are moved until all of the jobs finish. Therefore, if a job needs to access files that are generated by another job in the same jobset destination, these files will be located in the temporary folder, not the final jobset destination.
KiCad defines the ${JOBSET_OUTPUT_WORK_PATH} environment variable while jobs are running and sets it to the temporary path for the current jobset destination. You can use this environment variable if a job needs to be aware of the temporary folder’s actual location. For example, if an Execute Command job runs a script that renames the outputs of another job, the script needs to know the temporary location of the outputs being renamed, before they are moved to the jobset destination. ${JOBSET_OUTPUT_WORK_PATH} provides this location.
Available job types
The following types of jobs are available:
Job |
Description |
PCB: Export 3D Model |
Exports a 3D model of the board. The model format can be STEP, GLB (binary glTF), XAO, BREP (OCCT), PLY, STL, STPZ, U3D, or PDF. |
PCB: Export Board Statistics |
Generates a Board Statistics report in either JSON or text report format. |
PCB: Export Drill Data |
Exports a drill file from the board. |
PCB: Export DXF |
Exports the board design to a DXF file. |
PCB: Export Gencad |
Exports the board design in GenCAD format. |
PCB: Export Gerbers |
Exports the board design to Gerber files, with one file per selected layer. |
PCB: Export IPC-2581 |
Exports the board design in IPC-2581 format. |
PCB: Export ODB++ |
Exports the board design in ODB++ format. |
PCB: Export PDF |
Exports the board design to PDF files, with one file per selected board layer. You can also generate a single PDF with multiple layers depending on the plot configuration. |
PCB: Export PNG |
Exports the board design to PNG files, with one file per selected board layer. |
PCB: Export Position Data |
Exports a position (component placement) file from the board. |
PCB: Export PostScript |
Exports the board design to a PostScript file. |
PCB: Export SVG |
Exports the board design to a SVG file. |
PCB: Perform DRC |
Performs a Design Rule Check on the board and generates a report. If DRC violations are found, this job can optionally report a job failure. |
PCB: Render |
Generates a raytraced rendering of the 3D model of the board as a PNG or JPG file. |
Schematic: Export DXF |
Exports the schematic to a DXF file. |
Schematic: Export Netlist |
Exports a netlist from the schematic, with various formats available. |
Schematic: Export PDF |
Exports the schematic to a PDF file. |
Schematic: Export PNG |
Exports the schematic to a PNG file. |
Schematic: Export Postscript |
Exports the schematic to a PostScript file. |
Schematic: Export SVG |
Exports the schematic to a SVG file. |
Schematic: Generate Bill of Materials |
Exports a bill of materials from the schematic. |
Schematic: Perform ERC |
Performs an Electrical Rule Check on the schematic and generates a report. If ERC violations are found, this job can optionally report a job failure. |
Special: Copy Files |
Copies the specified file to the specified location. A failure to copy the files can optionally cause the output job to fail. You can control whether files in the output location should be overwritten or not. |
Special: Execute Command |
Executes an arbitrary command.
Output from the command can optionally be logged to a file.
You can either ignore non-zero output codes or cause them to fail the output job.
The command is executed in the platform’s shell ( Note: Job output files are generated in a temporary folder, then moved to the location specified by the jobset destination after all jobs for that destination are executed. In other words, when an Execute Command job runs, the output from other jobs in the same jobset destination are still in a temporary location and not yet in the ultimate destination folder or archive. You can use the |
Project templates
Using a project template facilitates setting up a new project with predefined settings. Templates may contain pre-defined sheet sizes, drawing sheets, board outlines, connector positions, schematic elements, design rules, logos, etc. Complete schematics and/or PCBs used as seed files for the new project may even be included.
Usando plantillas
Creating a new project (File → New Project…) opens the Project Template Selector dialog. By default, all installed templates are shown in the list of templates, but you can limit the list to system templates or user templates using the dropdown menu above the list.
-
System templates are installed with KiCad and include templates for designs in some common form factors.
-
User templates are any templates created by you. The default, blank KiCad template is also considered a user template.
When you click on a template, information about the template is shown in the right panel.
A further click on the OK button creates a new project based on the selected template. You can pick the name of the new project and where to create it. The template files will be copied to the new project location and renamed to reflect the new project’s name.
Template locations
When you create a new project, the Project Template Selector dialog shows templates from two locations:
-
System Templates are templates in the path defined by the
KICAD10_TEMPLATE_DIRpath variable. These templates are installed with KiCad’s default libraries and generally should not be modified by users. -
User templates are templates in the path defined by the
KICAD_USER_TEMPLATE_DIRpath variable. When you create your own project templates, store them in this location so you can use them when you create a new project.
To change the location of the user template folder, edit the KICAD_USER_TEMPLATE_DIR path variable in your paths configuration.
Template contents
A KiCad template is a directory containing the template project files, as well as some required metadata for the template in a subdirectory named meta. The name of the directory containing the template files determines the name of the template. This means that a KiCad template folder is simply a KiCad project folder with an additional meta subdirectory.
When you create a project from a template, KiCad copies the template files to the new project directory, renaming them to match the new project name as described below. All files in the template are copied, with three exceptions:
-
Files with names beginning with the
.character (dotfiles) are not copied. There is a special case for files named.gitignoreor.gitattributes, which are copied if they exist. -
If there is a
.gitignorefile, any files that are ignored in it are not copied. -
The
metadirectory is not copied.
Other than the exceptions above, all files in the template are copied, even if they are not KiCad design files.
This means you can use templates to create projects that are already set up with non-KiCad files you need to include, such as documentation templates, license files, logos, .gitignore files, etc.
|
Template metadata
A template’s meta directory must contain an HTML file named info.html, which is displayed in the KiCad template browser and should contain basic information describing the template. Basic HTML features are supported, including images. Any images referenced by info.html should also be stored in the meta directory.
The <title> tag determines the name of the template that is displayed during template selection. Note that the project template name will be cut off if it’s too long. This display name does not need to be the same as the template directory name.
Here is a sample info.html file:
<!DOCTYPE HTML PUBLIC "-//W3C//DTD HTML 4.0 Transitional//EN">
<HTML>
<HEAD>
<META HTTP-EQUIV="CONTENT-TYPE" CONTENT="text/html;
charset=windows-1252">
<TITLE>Raspberry Pi - Expansion Board</TITLE>
</HEAD>
<BODY LANG="fr-FR" DIR="LTR">
<P>This project template is the basis of an expansion board for the
<A HREF="http://www.raspberrypi.org/" 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" expansion
headers. <BR><BR>The board outline looks like the following:
</P>
<P><IMG SRC="brd.png" NAME="brd" ALIGN=BOTTOM WIDTH=680 HEIGHT=378
BORDER=0><BR><BR><BR><BR>
</P>
<P>(c)2012 Brian Sidebotham<BR>(c)2012 KiCad Developers</P>
</BODY>
</HTML>
Finally, meta can optionally contain an image named icon.png, which will be used as the template’s icon in the template selection dialog. The icon should be a 64 x 64 pixel PNG image.
Template file renaming
All files and directories in a template are copied to the new project path when a project is created using a template, except meta and dotfiles. Files and directories containing the template directory name will be renamed with the new project file name. Files and directories that don’t contain the template name keep their original name.
For example, using a template named example (left) to create a project named newproject (right), with renamed files shown in bold:
Files in template example directory |
Files created in project newproject directory |
|---|---|
|
|
A template does not need to contain a complete project. If a required project file is missing, KiCad will create the file using the default create project behavior:
Files in template example directory |
Files created in newproject directory |
|---|---|
|
|
As an exception to the template name renaming rule, if the template contains one project file (.kicad_pro) and its name doesn’t match the template name, KiCad will do the renaming based on that project file name instead:
Files in template example directory |
Files created in newproject directory |
|---|---|
|
|
| It is not recommended to create a template with multiple project files. |
Creating new templates
Because a KiCad template is just a Kicad project with an additional metadata folder, the easiest way to create a new template is to start from a project. If you save a project in your user template folder and add a meta folder to it, you can use it as a template.
To find out where your user template folder is, check the value of the KICAD_USER_TEMPLATE_DIR path variable in the Configure Paths dialog (Preferences → Configure Paths…).
|
If you are creating a template from scratch, you can create a new project in the user template folder, then edit the project until you have created your desired template. This new project will be your template, so when you create it you should choose the name based on what you want the template to be called.
If you have an existing project that you want to turn into a template, you can save a copy of that project into your user template folder (File → Save As… from the Project Manager). The name you choose for the re-saved project will be the template name. After saving in the template folder, you can edit the template project so that it exactly matches your desired template.
In either case, templates are required to have a metadata directory, so you must add a meta folder inside the template folder. The metadata folder must also contain an info.html file, which is intended to contain a description of the template. You can copy the sample info.html above as a starting point.
In general, you will also want to remove any files and folders that you don’t want to include each time you use the template. Some examples of things to remove include the *-backups folder, the .history snapshot folder, any unneeded version control files (.git, etc.), and anything else you don’t want to include in new projects.
Plugin and Content Manager
KiCad has a Plugin and Content Manager that lets you browse, install, and manage packages submitted by other users and organizations. Packages can be plugins offering specialized functionality, tools for ordering PCBs from specific manufacturers, libraries of symbols and footprints, or new editor color schemes. You can access the PCM by launching it from the main KiCad Project Manager window.
The PCM downloads packages from repositories on the internet. Each repository is a collection of packages that is managed by an individual or an organization. By default, the PCM uses a single repository managed by the KiCad organization. Users and organizations are free to create their own repositories, which other users can can then add as additional repositories in their own KiCad installation. Third-party repositories can be public or private.
| Packages may install code that runs on your computer. Packages are not developed by the KiCad developers. The KiCad organization does not make any guarantees about the quality or safety of packages installed through the PCM. Make sure you only install packages that you trust. |
| If you have feedback regarding a package, please submit it to the package’s developer, not the KiCad team. Contact information for each package is shown in the package’s description. |
To share a package that you have developed, you can submit it to the KiCad official repository. If it is accepted, it will then be available to other users browsing the KiCad repository. You can also create your own repository or submit your package to a repository managed by another person or group, but in that case users will not see your package unless they have configured that repository in their own installation. More information about creating your own packages and repositories is available below.
Browsing packages
All of the packages in a repository are shown in the PCM’s Repository tab. You can choose which repository to browse by selecting the repository in the dropdown at the top of the tab. By default, only the KiCad official repository is enabled.
Packages are grouped into four categories, each with its own tab within the Repository tab:
-
Plugins are additional tools that can be launched from the PCB Editor. Plugins can have many purposes, for example modifying a board design or generating specific outputs. Footprint wizards can also be distributed as plugins.
-
Fabrication plugins are a sub-category of plugins for ordering your PCBs from specific fabricators. These plugins may be a convenient way to order from a manufacturer, but they are typically not required; you can usually provide manufacturers with normal fabrication outputs instead. Consult with your manufacturer to find out the best way to order from them.
-
Libraries contain symbols, footprints, and/or 3D models. By default, libraries installed by a library package are automatically added to the appropriate symbol and/or footprint library tables when the package is installed, and removed from the table when the package is uninstalled. Libraries installed by a package have configurable library name prefix (
PCM_by default). These settings are configurable in the Packages and Updates section of Preferences. -
Color themes are color themes for the Schematic, Symbol, Board, and Footprint editors. You can select an installed theme in the Colors section of the Preferences for each editor.
The list on the left of the window shows the packages within each category. You can filter the list of packages by typing in the filter box at the top of the package list. Press the Refresh button to reload the list of packages from the online repository.
When you select a package in the list, information about the package is shown on the right. This includes a description of the package, the package’s license, and contact information for the package’s developer, including a place to report bugs and other feedback for the package.
The package information also includes a table of the versions of the package that are currently available. For each version, the table displays the package size, its status, and whether it is compatible with your version of KiCad.
A package’s status can be one of the following, as indicated by the package’s developer:
-
Stable: the package version is suitable for general use.
-
Testing: the package version is in a testing phase; users should be cautious and report any issues they encounter to the package’s developers.
-
Development: the package version is in a development phase; users should not expect it to work fully.
-
Deprecated: the package is no longer maintained.
By default, the version table only shows versions of the package that are compatible with your version of KiCad. You can show all versions of the package, even those that will not work with your KiCad version, by checking the Show all versions box. If multiple versions of a package are available, you can choose which to install.
Installing packages
When you decide to to install a package, click the package’s Install button in the package’s description page. If there are multiple versions of the package available, select the desired version in the version table before installing. You can also install the latest version by clicking the Install button in the list of packages. This does not immediately install the package; the package is instead queued for later installation and is shown in the Pending tab. The package will not be installed until you click the Apply Pending Changes button, which installs all pending packages at once.
To remove a single package from the pending installation list, select it in the Pending tab and press the
button. To cancel the installation of all pending packages, click the Discard Pending Changes button.
Once a package is installed, it is listed in the Installed tab. In this tab you can see the list of installed packages and update or uninstall any of them.
If any packages have new versions available, the PCM icon in the Project Manager displays an indicator showing the number of available updates.
To update to a different version of a package, select the new version in its version table and click the Update button. You can also update a package to the newest version by clicking Update in the dropdown menu next to its Uninstall button in the list of installed packages. To update all installed packages, click the Update All button at the top of the installed package list. A package will not be updated if Pin Package is selected in its dropdown menu.
To uninstall a package, click its Uninstall button in the list of installed packages or in the package’s description page.
As with installation, packages are not updated or uninstalled immediately when you click the Update or Uninstall button. Instead, the operation is queued in the Pending tab until you apply each change individually or click the Apply Pending Changes button.
Finally, you can download a package without installing it by clicking the Download button at the bottom of the package’s description and selecting a location to save the package. This lets you inspect the files in the package before installing it. To install a package that has been downloaded but not yet installed, click the Install from file… button and select the package. The Open Package Directory button opens a file browser in the folder where KiCad installs packages.
Managing repositories
By default, only the KiCad official repository is used by the PCM. You can add a third party repository, or remove existing repositories, by clicking the Manage… button at the top of the Repository tab.
To add a repository, click the
button and specify the full URL to the repository. To remove a repository, select it and press the
button. Use the
and
buttons to reorder repositories in the list.
If you remove the default KiCad official repository, you can easily re-add it by clicking Add Default Repository in the dropdown menu next to the
button.
Creating packages and repositories
To create a package for the PCM, follow the instructions at https://dev-docs.kicad.org/en/addons/index.html. These instructions explain how to create PCM packages for any repository, including but not limited to the KiCad official repository. They also explain the rules for packages included in the KiCad repository and how to submit packages to this repository. Third-party repositories use the same package format but may have different rules and procedures for submitting packages.
To create your own repository, publish a repository JSON file following the schema published at https://go.kicad.org/pcm/schemas/v1.
KiCad preferences
The KiCad preferences can always be accessed from the Preferences menu, or by using the hotkey (default Ctrl+,).
| On macOS, the KiCad preferences are accessed via KiCad → Settings…. |
The Preferences dialog is shared between the KiCad tools. Some preferences apply to all tools, and some are specific to a certain tool (such as the schematic or board editor).
Common preferences
Rendering engine
Accelerated graphics antialising: KiCad can use different methods to prevent aliasing (jagged lines) when rendering using a graphics card. Different methods may look better on different hardware, so you may want to experiment to find the one that looks best to you.
Fallback graphics antialiasing: KiCad can also apply antialiasing when using the fallback graphics mode. Enabling this feature may result in poor performance on some hardware.
Helper applications
Text editor: Choose a text editor to use when opening text files from the project tree view.
PDF viewer: Choose a program to use when opening PDF files.
User interface
Show icons in menus: Enables icons in drop-down menus throughout the KiCad user interface.
| Icons in menus are not displayed on some operating systems. |
Show scrollbars in editors: When enabled, scrollbars are displayed next to the editing canvases in each tool. When disabled, scrollbars are not shown.
Focus follows mouse between schematic and PCB editors: When enabled, the window under the mouse cursor will automatically become focused.
Show popup indicator when toggling settings with hotkeys: When enabled, certain hotkeys that cycle between settings will show a popup indicator briefly to indicate the change in settings.
Use alternating row colors in tables: When enabled, tables (such as the library tables and the Symbol Fields table) will use alternating colors for each row.
Disable custom cursors: When enabled, KiCad will use the system cursors instead of custom context-specific cursors.
Icon theme: Sets whether to use the icon theme designed for light window backgrounds or dark window backgrounds. The default setting of Automatic will choose the theme based on the lightness of the operating system window theme.
| The light icon theme has darker icons that are more visible against light window backgrounds. The dark icon theme has lighter icons designed for dark window backgrounds. |
Icon scale: Sets the size of the icons used in menus and buttons throughout KiCad. Choose Automatic to pick an appropriate icon scale automatically based on your operating system settings.
High-contrast mode dimming factor: Sets how much non-focused items are dimmed in high-contrast display mode.
Scaling
Display PPI: When set to the pixel density of your display, the editing canvas will be scaled so that objects are life sized at 100% zoom. You can press the Detect button to use the pixel density reported by your display, or manually adjust the density until the ruler is displayed at the correct size.
Editing
Warp mouse to origin of moved object: When enabled, the mouse cursor will be repositioned (warped) to the origin of an object when you start a move command on that object.
First hotkey selects tool: When disabled, pressing the hotkey for a command such as Add Wire will immediately start the command at the current cursor location. When enabled, pressing the hotkey the first time will just select the Add Wire tool but will not immediately begin a wire.
Session
Remember open files for next project launch: When enabled, KiCad will automatically re-open any files that were previously open when a project is re-opened.
Project backup
Automatically backup projects: When enabled, KiCad will automatically make backups and autosaves of the current project. A project autosave is automatically saved when there are unsaved changes after a few seconds of inactivity. Backups are also performed each time you manually save.
Format: Controls the backup format.
-
When set to Incremental, project backups are saved using an incremental backup system that stores snapshots of files as they change. These incremental snapshots are shown in the Local History panel (View → Panels → Local History). You can restore from an earlier snapshot by right clicking a snapshot in the Local History panel and choosing Restore Commit. Behind the scenes, the incremental backup system uses a Git repository in a hidden
.historyfolder. -
When sent to Zip archive, project backups are saved as a Zip archives of the project directory and its contents. You can restore from these archives by using the Unarchive tool or by manually extracting the archive and loading the project.
Location: Controls where backups are saved. Backups can be saved in the project directory or in your KiCad user data (configuration) directory.
Maximum total backup size: When creating a new backup file, the oldest backup files will be deleted to keep the total size of the backup files directory below this limit.
Mouse and touchpad preferences
Center and warp cursor on zoom: When enabled, zooming using the hotkeys or mouse wheel will cause the view to be centered on the cursor location.
Use zoom acceleration: When enabled, scrolling the mouse wheel or touchpad faster will cause the zoom to change faster.
Zoom speed: Controls how much the zoom changes for a given amount of scrolling the mouse wheel or touchpad. Use Automatic to set a default value depending on your operating system.
Automatically pan while moving object: When enabled, the view can be panned while moving an object by moving close to the edge of the canvas.
Auto pan speed: Controls how fast the canvas pans while moving an object.
Mouse buttons: You can set the behavior of dragging the middle and right mouse buttons to zoom the view, pan the view, or have no effect. You can also set the behavior of dragging the left mouse button depending on whether or not any objects are already selected in the editing canvas. If a key is configured for Pan on mouse movement with key, you can pan the canvas by holding the configured key and moving the mouse.
| The left mouse button is always used for selecting and manipulating objects. |
Mouse wheel and touchpad scrolling: You can set the behavior of scrolling the mouse wheel or vertical motion of the touchpad while pressing certain modifier keys.
Pan left/right with horizontal movement: When enabled, you can pan the view using the touchpad or horizontal scroll wheel (if present on your mouse).
SpaceMouse preferences
This page contains settings for KiCad’s integration with SpaceMouse peripherals.
Rotation speed and Pan speed control how quickly to rotate and pan in response to a SpaceMouse input.
Reverse rotation direction: When enabled, rotations will go in the opposite direction from the default.
Reverse vertical pan direction: When enabled, vertical pans will go in the opposite direction from the default.
Reverse horizontal pan direction: When enabled, horizontal pans will go in the opposite direction from the default.
Reverse zoom direction: When enabled, zooms will go in the opposite direction from the default.
Hotkey preferences
You can use this dialog to customize the hotkeys used to control KiCad. The hotkeys in the Common section are shared between every KiCad program. You can assign the same hotkey to a different action in different KiCad programs (for example, the schematic editor and the board editor), but you cannot assign a hotkey to more than one action in the same program.
There are many available commands, and so not all of them have a hotkey assigned by default. You can add a hotkey to any command by double-clicking on the command in the list. If you choose a hotkey that is already assigned to a different command, you can choose to use that hotkey on your chosen command, which will remove the hotkey assignment from the conflicting command.
Changes that you have made to hotkey assignments are shown with a * character at the end of the command name. You can undo changes to a specific command by right-clicking that command and selecting Undo Changes, or you can undo all changes with the button below the command list.
Importing hotkeys
Hotkey preferences are stored in .hotkeys files in the KiCad settings directory (see the Settings section for information about where the settings directory is on your operating system). If you have configured KiCad hotkeys the way you like on one computer, you can transfer that configuration to another computer by importing the appropriate .hotkeys file(s).
Version control preferences
This page contains the settings for the Git integration.
Enable Git tracking: Enables the Git tools for all projects. When you clear this option, KiCad does not show the file status and does not check the remote. It also removes the File → Clone Project from Repository… menu item. The Version Control panels tell you that version control is turned off.
Update interval: Sets the number of minutes between checks for new commits on the remote. The range is 0 to 60 minutes. When you set it to 0, KiCad does not check the remote automatically. The project files tree and the Version Control panel show the result of the check.
Use default values: Shows the name and email address from your global Git settings. Clear this option to type a different Author name and Author e-mail. KiCad uses these values only when a repository has no author. Then the Set Author dialog shows them before your first commit in that repository.
Show contributor photos from the web (Gravatar): Shows a photo for each author on the History page of the Advanced Git window. To find the photos, KiCad sends a hash of each author’s email address to the Gravatar service. This option is off by default.
Data collection preferences
This page contains settings that control how KiCad collects usage and crash data from users. Data collection is disabled by default.
| Crash reporting is only supported on Windows and macOS platforms. |
When I agree to provide anonymous reports is enabled, KiCad will send anonymous reports to the KiCad development team when KiCad crashes and in certain other situations. These reports help the KiCad development team fix crashes and other bugs. The reports do not contain your design files, such as schematics or PCBs.
Reports are linked to a random, unique identifier that is shown on this page. This identifier is used to connect reports from the same computer. No personally identifiable information (PII), including IP address, is stored or connected to this identifier. You can reset this identifier at any time by pressing the Reset Unique Id button.
Packages and updates preferences
Check for KiCad updates on startup: If enabled, on startup KiCad will check for updates to the KiCad application. If an update is available, you will be prompted to install it.
Check for package updates on startup: If enabled, on startup KiCad will check for updates to any packages installed through the Plugin and Content Manager. Available updates are shown as a notification in the bottom right of the Project Manager window.
Automatically add installed libraries to global library table: If enabled, libraries that are installed through the Plugin and Content Manager will be automatically added to your library table. The library nickname will use the prefix configured on this page. If not enabled, you will need to manually add them to your library table after they are installed.
Automatically remove uninstalled libraries: If enabled, libraries that are installed through the Plugin and Content Manager will be automatically removed from your library table when they are uninstalled. If not enabled, you will need to manually remove them from your library table after they are uninstalled.
Plugins preferences
Enable KiCad API: When enabled, you can use plugins that interact with KiCad’s IPC API. If this option is not enabled, such plugins will not function.
Path to Python interpreter: This is the location of the Python interpreter that KiCad will use to run Python-based IPC plugins. You can automatically detect a Python interpreter or manually specify a path.
Maintenance preferences
3D cache file duration: KiCad creates a cache of 3D models in order to speed up the 3D viewer. You can configure how long to keep this cache before deleting old files.
Clear "Open Recent" History: Clears the project entries in the File → Open Recent menu.
Reset "Don’t Show Again" Dialogs: Causes dialogs that have been dismissed with the Don’t Show Again setting to be shown again in the next situation where they would otherwise be hidden.
Reset All Dialogs to Defaults: Resets changed settings in all KiCad dialogs.
Reset All Program Settings to Defaults: Resets all KiCad preferences to their defaults.
Actions reference
Below is a list of every available action in the KiCad Project Manager: a command that can be assigned to a hotkey.
KiCad Project Manager
The actions below are available in the KiCad Project Manager. Hotkeys can be assigned to any of these actions in the Hotkeys section of the preferences.
| Action | Default Hotkey | Description |
|---|---|---|
Browse Project Files |
Open project directory in file explorer |
|
Archive Project… |
Archive all project files |
|
Close Project |
||
Image Converter |
Ctrl+B |
Convert bitmap images to schematic or PCB components |
Drawing Sheet Editor |
Ctrl+Y |
Edit drawing sheet borders and title block |
Footprint Editor |
Ctrl+F |
Create, delete and edit PCB footprints |
PCB Editor |
Ctrl+P |
Edit PCB in PCB editor |
Schematic Editor |
Ctrl+E |
Edit schematic in schematic editor |
Symbol Editor |
Ctrl+L |
Create, delete and edit schematic symbols |
Clone Project from Repository… |
||
New Jobset File… |
||
New Project… |
Ctrl+N |
Create a new project based on an existing project |
Open Demo Project… |
||
Open Jobset File… |
||
Open Project… |
Ctrl+O |
|
Open Text Editor |
Launch preferred text editor |
|
Plugin and Content Manager |
Ctrl+M |
Run Plugin and Content Manager |
Restore Project from Local History… |
Restore project files from local history |
|
Calculator Tools |
Run component calculations, track width calculations, etc. |
|
Local History |
Show or hide local history panel |
|
Unarchive Project… |
Unarchive project files from zip archive |
|
Gerber Viewer |
Ctrl+G |
Preview Gerber output files |