Getting Started With LibrePCB

This page will give you a quick introduction into LibrePCB, starting from where to download it and ending with how to generate the production data for the PCB.

Installation

Attention: Unstable file format!

The file format of LibrePCB is still under development, and breaking changes can occur at any time. This means that you may (or will) not be able to open your created libraries and projects with future versions of LibrePCB!

Or in other words: LibrePCB does not yet have an upgrade mechanism for the files created with older LibrePCB versions. We will start providing an upgrade mechanism as soon as we publish the first stable release of LibrePCB.

Download & Start LibrePCB

No stable releases

There are not yet any stable releases available, so at the moment you need to download the nightly builds instead.

For Windows, you can download librepcb-nightly.zip and extract its content. Then double-click the contained file bin\librepcb.exe to run the application.

For Linux, just download LibrePCB-Nightly-Linux-x86_64.AppImage, make it executable and start it:

wget -O LibrePCB-Nightly-Linux-x86_64.AppImage "https://bintray.com/librepcb/LibrePCB-Nightly/download_file?file_path=LibrePCB-Nightly-Linux-x86_64.AppImage"
chmod +x ./LibrePCB-Nightly-Linux-x86_64.AppImage
./LibrePCB-Nightly-Linux-x86_64.AppImage

Create a Workspace

When starting LibrePCB the first time, a wizard asks you to open or create a Workspace. The Workspace is just a directory where settings, libraries and (optionally) projects will be stored. Once created, it can be used from all supported operating systems (i.e. it is platform independent) and in future it will also be usable with different LibrePCB versions.

You can just accept the default Workspace location (you could still move it to another location afterwards, if desired):

choose workspace

After clicking Finish, the Control Panel shows up and you’re ready to start using LibrePCB!

Add Libraries

Before you can start with creating new projects, you need to add some libraries to your Workspace. Libraries contain various kinds of elements which can be added to schematics and boards (e.g. symbols and footprints).

To open the Library Manager, click on the corresponding button in the Control Panel (or on the link in the shown warning, but the warning will disappear after you add a library):

Library Manager

Download Remote Libraries

The Library Manager directly fetches the list of available libraries from the Internet. Most of these libraries are hosted at https://github.com/LibrePCB-Libraries.

The provided libraries currently contain only a few elements, especially because the file format is still not considered as stable.

The most important library is the LibrePCB Base Library because it contains the most commonly used library elements (like resistors or diodes). It is highly recommend to install this library. To do so, just select the checkboxes at the right and click on the Download and install/update all selected libraries button:

Download Libraries

By the way, the same way you can also update already installed libraries to the latest version. You should regularly update all libraries to get more elements and bugfixes/improvements of existing elements.

Dependencies between different libraries are automatically taken into account when changing the selection. So for example if you select LibrePCB Connectors, the LibrePCB Base Library will automatically be selected too because the Connectors library depends on it.

Downloaded (so-called remote-) libraries are always read-only because otherwise local modifications could cause conflicts when updating the library the next time. But this should not be an issue, just follow the guide below to create your own local library. In a local library you can extend, or even overwrite existing library elements (by using a higher version number to enforce higher priority).

If you are familiar with Version Control Systems (e.g. Git) and want to use them to manage your libraries (instead of the Library Manager), just clone the libraries into the subdirectory v0.1/libraries/local/ in your Workspace.

Create Local Libraries

Of course you can also create your own libraries. To do so, enter some metadata in the tab Create local library and click on Create Library:

Create Library

Now you can open the library editor to create some symbols and footprints in your new library. Select your library on the left and then click on the Open Library Editor button:

Open Library Editor

Now we need a crash course to understand the basics of LibrePCB’s library concept ;) A library consists of several different elements:

  • Component Category: These are basically "metadata-only" elements used to categorize the "real" library elements in a category tree. Every Symbol, Component and Device can be assigned to one or more categories so they will appear in the category tree. Examples: Resistors. LEDs, Microcontrollers

  • Symbol: A symbol is the graphical representation of a Component (or parts of it) in a schematic. It consists of electrical pins and graphical objects like lines. Examples: European Resistor, LED, 1x10 Connector

  • Component: A Component basically represents a "generic" kind of electrical part. It’s not a real part which you can buy, it’s just theoretical. The Component defines the electrical interface of a part and how it is represented in the schematic (by referencing one ore more Symbols). But it does not defines how the part looks like in a board. Examples: Resistor, Bipolar Capacitor, 4-channel OpAmp

  • Package Category: Exactly the same as Component Categories, but for Packages instead of Components. Examples: Chip Resistors, Axial Capacitors, DIP

  • Package: As the name suggests, packages represent the mechanical part of a "real" electronic part. It contains the footprint with their electrical pads and graphical objects which is then added to boards. Later a package may also contain a 3D model for the 3D board viewer. Examples: TO220, DIP20, LQFP32

  • Device: The Device now represents a real electronic part which you can buy. It basically combines a Component with a Package to specify how a Component looks like on the board. Examples: 0805 Resistor, LM358D, STM32F103C

The order of this list is actually also the order to follow when creating new library elements. For example a Device always needs to be created after the corresponding Component. The other direction is not possible because of the dependencies.

Ready to create your first library elements? At the top left of the library editor there is the entry point for every new library element. There you can choose which of the six library element type you want to create:

New Library Element

Example: LMV321LILT

Let’s say you want to create the part LMV321LILT from A to Z. We will create now all the necessary library elements for the LMV321LILT, though in practice you only need to create the elements which do not already exist. You can even use elements from other libraries, for example the Symbol from library A, the Component from library B and the Package from library C.

Component Category

First you should create a Component Category for the LMV321LILT (if it doesn’t already exists). Choose a suitable (generic!) name and select a parent category. You may first need to create the required parent categories.

Create Component Category

After clicking on Finish, your first Component Category is ready to be used :)

Symbol

Now we need to create a Symbol for the OpAmp. So this time you click on the Symbol button in the New Library Element wizard. Then fill in some metadata and click on Finish. Now you can place the required pins (choose reasonable names!) and draw the outline. The result could look like this:

Create Symbol

Yeah, the overlapping texts look ugly, but let’s ignore that for the moment ;)

Component

The next element you need to create is the Component for a single OpAmp. Because it is still very generic (beside the LMV321LILT there are many other OpAmps with exactly the same functionality), so you should enter a generic name like Single OpAmp. In addition, it’s really important to choose a Category for the new Component, otherwise it’s hard to find it in the library when you want to add it to a schematic.

Create Component

Then you’re asked to specify some properties of the Component:

  • Schematic-Only: This should be checked if the Component must not appear on a board, but only in the schematics. This is typically used for schematic frames (yes, they are also Components).

  • Prefix: When adding the Component to a schematic, its name (designator) is automatically set to this value, followed by an incrementing number. So if you choose the prefix R, components added to a schematic will have the names R1, R2, R3 and so on. The prefix should be very short and uppercase.

  • Default Value: In addition to the name, Components also have a value assigned to it, which is typically also displayed in the schematic. For example a capacitor has its capacitance (e.g. 100nF) set in its value. When adding a Component to a schematic, its value is initially set to the value specified here. The value can also be a placeholder, for example #PARTNUMBER, #RESISTANCE or #CAPACITANCE. If you are unsure, just leave it empty, you can still change it later.

Now you need to choose the Symbols which represent the Component in schematics. Most Components have only one Symbol, but you can also add more than one, for example an OpAmp can have separate Symbols for power and amplifier.

After adding the OpAmp Symbol, it should look like this:

The next step is to define all so-called Signals of a Component. Signals represent the "electrical interface" of a Component. For example a transistor consists of the Signals base, collector and emitter. For a Component it’s irrelevant whether the "real" transistor has multiple emitter pads, or an additional thermal pad and so on, the Component only specifies the three Signals.

LibrePCB automatically extracts the Signals from the Pins of the specified Symbols, so often we don’t have to do this by hand. But sometimes you still should adjust the names or properties of these Signals. For the OpAmp, we check Required for all Signals, so the ERC will show a warning if these Signals are not connected to a net when the Component was added to a schematic:

These Signals now need to be assigned to the corresponding Symbol Pins, but as they were automatically generated from the Pins, you can just click on the button below to automatically assign all Pins to their Signals:

Component Pin-Signal-Map

That’s it, the Component is now ready to be used:

Component Editor

For this simple example, this procedure may feel a little bit complicated. This is basically caused by the high flexibility of the library concept. The Component which we created now actually uses only the very basic library features, but as soon as you understand the whole library concept, you will be able to easily create much more powerful library elements. We’re sure you will love the flexibility of the library concept ;)

Package Category

Before creating a Package for the LMV321LILT, you should (optionally) create a category for it. This is basically done exactly the same way as you already created the Component Category, so we won’t explain it again. It could look like this:

Create Package Category

Package

Then you need to create the Package for the LMV321LILT, which is called SOT23-5. After specifying some metadata (like you already done for other library elements), you are asked to specify all pads of the Package. The SOT23-5 has 5 pads which we just name from 1 to 5:

Create Package Pads

Packages should be designed as generic as possible to make them usable also for other Devices. So it’s very important to name their pads according to the specifications of the Package (e.g. as defined in IPC-7351), not according to their functionality for your specific Device.

Typical pad names are: 1, 2, 3, THERMAL, …​
Bad pad names are: BASE, EMITTER, COLLECTOR, SDA, SCL, …​

After that, you can start drawing the footprint of the Package. It’s recommended to start with the pads:

Create Package

And then add other graphical items like the outline, name and value:

Create Package Graphics

That is already enough for a simple footprint.

Device

The last library element you need to create is the Device which combines the Component Single OpAmp with the Package SOT23-5. Again, specify some metadata about the Device first. Then you need to choose the Component and Package you want to assign:

Create Device

Then you have to assign the Package pads to Component signals according to the datasheet of the LMV321LILT:

Device Pad-Signal-Map

And that’s it! In the library overview (the first tab in the Library Editor) you can see all the elements you have created:

Library Overview

The LMV321LILT is now ready to be added to schematics and boards. And because the Categories, Symbol, Component and Package are quite generic, they can also be used for many other library elements :)

Create a New Project

In LibrePCB, schematics and boards are always part of a Project, so to draw schematics and boards you first need to create a Project for every PCB you want to design. This is really easy, just follow the New Project wizard:

Create Project

Then fill in some metadata about the Project:

Create Project

For Open-Hardware projects it’s highly recommended to select the license CC0-1.0 as this allows everyone to use your project without restrictions.

Even if it is possible to create the Project outside the Workspace directory, it’s recommended to store all Projects inside the Workspace because these Projects are listed at the left side of the Control Panel. This allows to easily locate and open them. Projects outside the Workspace need to be opened by specifying their location in an open dialog.

Now you can choose whether the Project should be initialized with a first schematic page and board, and how they are named. If you are unsure, just accept the default values:

Initialize Project

After clicking on Finish, the schematic and board editors show up and you’re ready to draw the schematics:

Project Editor

Create Schematics

First, you may want to add a frame to the schematic. Is is done by choosing a schematic frame in the Component Chooser:

Add Schematic Frame

Then let’s add the OpAmp we have created in our own library, again with the Component Chooser:

Add OpAmp

Here you can choose whether you want to add the Component Single OpAmp or the Device LMV321LILT. Yes, you can add either a Component or a Device to a schematic ;) Actually the schematic always contains Components (not Devices), but you can still (optionally) choose the Device which will be used later when adding the Component to the board (boards always contain Devices).

The most commonly used Components are also available in the toolbar on the left side:

Standard Components

Just place some Components and draw the net lines with the corresponding tool in the toolbar at the left side.

Create Boards

Once the schematic is (more or less) complete, you can start adding Devices to the board. For every Component in the schematic, you need to place a Device in the board (except schematic-only Components, like the schematic frame). In the Place Devices dock on the right side of the board editor you can see all unplaced Components. For every Component you can choose its corresponding Device now and add them to the board:

Add Devices to Board

By the way, it’s even possible to replace the Devices after adding them to the board. So for example you can replace a C-1210 capacitor by a C-0805 capacitor just in the context menu of the Device:

Change Device

Then you can start adding vias and traces to connect the pads together.

The functionality of the board editor is still very limited. Some very important features (like copper planes and airwires) are currently under development.

Generate Production Data

Once the board is finished, you can generate the production data for the PCB manufacturer:

Generate Production Data

With a simple button click the Gerber and Excellon files are created inside the project’s output subdirectory:

Production Data Generator

The production data generator is currently very limited in functionality, and also not very mature. It’s highly recommended to cross-check the generated files with 3rd-party tools like gerbv.

LibrePCB is not responsible for any implications caused by wrong production data.

results matching ""

    No results matching ""