KiCad runs on many operating systems, including Microsoft Windows, Apple macOS, and many major Linux distributions.

You can find the most up to date instructions and download links at https://www.kicad.org/download/. These instructions are not included in this manual as they may change over time with the release of operating system updates.

Si tiene ideas, comentarios o preguntas, o si simplemente necesita ayuda:

Typically, the schematic is drawn first. This means adding symbols to the schematic and drawing the connections between them. Custom symbols may need to be created if appropriate symbols are not already available. At this stage footprints are also selected for each component, with custom footprints created as necessary. When the schematic is complete and the design has passed an electrical rules check (ERC), the design information in the schematic is transferred to the board editor and layout begins.

The schematic describes which components are in the design and how they are connected; the board editor uses this information to make layout easier and to prevent mismatches between the schematic and PCB. The layout process requires careful placement of each footprint on the circuit board. After component placement, copper tracks are drawn between components based on the connections in the schematic as well as other electrical considerations, such as trace resistance, controlled impedance requirements, crosstalk, etc.

Often the schematic will need to be updated after layout has begun; the schematic changes can be easily pulled into the board design. The reverse can often happen: any design changes made in the board layout can be pushed back to the schematic to keep the two consistent.

When the board layout is complete and the board has passed the Design Rules Check (DRC), fabrication outputs are generated so that the board can be manufactured by a PCB fabricator.

The first time the schematic editor is opened, a dialog will appear asking how to configure the global symbol library table. The symbol library table tells KiCad which symbol libraries to use and where they are located. If you have installed the default libraries with KiCad, which is recommended, select the default option: Copy default global symbol library table (recommended).

If KiCad cannot find the libraries in their expected installation location, this option will be disabled. In this case, the user should choose the second option, Copy custom global symbol library table. Click the folder button at the bottom, and browse to the location given below. Select the sym-lib-table file.

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:

To pan around the schematic, click and drag with the middle mouse button or right mouse button. Zoom in and out with the mousewheel or F1 and F2. Laptop users may find it useful to change the mouse controls to be better suited to a touchpad; the mouse controls are configurable in Preferences → Preferences…​ → Mouse and Touchpad.

By default, KiCad enables a mouse setting called Center and Warp Cursor on Zoom. When this feature is enabled, the mouse cursor is automatically moved to the center of the screen when the user zooms in or out. This keeps the zoomed region centered at all times. This feature is unusual, but many users find it useful once they get used to it. Try zooming in and out with the mouse cursor in different areas of the canvas. If the default zoom behavior is uncomfortable, disable the feature in the Mouse and Touchpad preferences.

The toolbar at the left side of the screen contains basic display settings. The toolbar at the right side of the screen contains tools for editing the schematic.

Most tools in KiCad either have default hotkeys assigned, or can have custom hotkeys assigned. To view all hotkeys, go to Help → List Hotkeys…​. Hotkeys can be changed in Preferences → Preferences…​ → Hotkeys.

Before drawing anything in the schematic, set up the schematic sheet itself. Click File → Page Settings. Give the schematic a title and date, and change the paper size if desired.

Start making the circuit by adding some symbols to the schematic. Open the Choose Symbol dialog by clicking the Add a Symbol button on the right side of the window or pressing A.

This action will trigger the Footprint Library Table Setup dialog. This dialog is equivalent to the Symbol Library Table Setup dialog explained earlier, but for footprints instead of symbols.

Again, select the default option: Copy default global footprint library table (recommended). If this is option is disabled, select the second option, Copy custom global footprint library table. Click the folder button at the bottom, and browse to the location given in the symbol library table setup instructions. Select the fp-lib-table file and click OK.

The Choose Symbol dialog lists the available symbol libraries and the component symbols contained within them. Basic devices like passive components, diodes, and other generic symbols are found in the Device library. Specific devices, such as a particular LED, may be found in other libraries.

Scroll down to the Device library, expand it, and select the LED symbol. Click OK, and click again to place the symbol in the schematic.

Next, add a current-limiting resistor. Go back to the symbol chooser, but this time try searching for a resistor by entering R in the filter box at the top. Again, it is found in the Device library. The R device is an IEC-style rectangular resistor symbol. An R_US symbol is also available for users who prefer the ANSI-style zigzag symbol. Select a resistor symbol and add it to the schematic.

Finally, add a battery to power the LED. The Device library has a suitable Battery_Cell symbol.

Next, position the symbols correctly relative to each other, as shown in the screenshot. Do this by selecting, moving, and rotating the symbols.

In KiCad 7.0, objects are selected by clicking on them. Additional objects can be added to the selection with Shift+click, or removed with Ctrl+Shift+click (macOS: Cmd+Shift+click). You can toggle an item’s selection state with Ctrl+click (macOS: Cmd+click).

Drag selection is also possible; dragging from left-to-right selects objects that are entirely enclosed by the selection box, while dragging right-to-left also selects objects that are partially enclosed by the selection box. Shift, Ctrl+Shift (Cmd+Shift), and Ctrl (Cmd) can also be used with drag selection to add, subtract, or toggle from the selection, respectively.

Note that it is possible to select an entire symbol (by clicking on the symbol shape itself) or to select one text field in the symbol without selecting the rest of the symbol (by clicking the text). When just a text field is selected, any actions performed will act only on the selected text and not on the rest of the symbol.

Selected objects are moved by pressing M and rotated by pressing R. The G hotkey (drag) can also be used to move objects. For moving unconnected symbols, G and M behave identically, but for symbols with wires attached, G moves the symbol and keeps the wires attached, while M moves the symbol and leaves the wires behind. Selected objects can be deleted with the Del key.

The symbol pins all have small circles on them, indicating that they are not connected. Fix that by drawing wires between symbol pins as shown in the screenshot. Click the Add a Wire button on the right-hand toolbar or use the W hotkey. Click to start drawing a wire, and finish drawing the wire by clicking on a symbol pin or double clicking anywhere. Pressing Escape will cancel drawing the wire.

Another convenient method of drawing wires is to hover over an unconnected pin. The mouse cursor will change to indicate that a wire can be drawn starting from that location. Clicking on the pin will then begin drawing a wire automatically.

Next, add power and ground symbols to the schematic. While not strictly necessary in such a simple schematic, these make it easier to understand large schematics.

A number of power and ground symbols are available in the Power symbol library. However, there is a shortcut for adding these symbols: click the Add a Power Symbol button or use the P hotkey. This brings up the Choose a Symbol dialog, but only displays symbol libraries that contain power symbols.

Add a VCC symbol and GND symbol and then connect them to the circuit with wires.

Finally, add a label to the wire between the LED and resistor. Again, this may not be necessary in a simple circuit, but it is good practice to label important nets. Click the Net Label button in the right toolbar (L), type a label name (led), and place the label into the schematic so that the square attachment point overlaps with the wire. Rotate and align the label as necessary.

Note that labels and power symbols with the same name are connected together. Another GND symbol or wire labeled led on this schematic page would be shorted to the existing one, even without wires visually connecting them.

The last remaining thing to do in the schematic is to check for electrical errors. KiCad’s Electrical Rules Checker (ERC) cannot make sure that the design in the schematic will work, but it can check for some common connection issues such as unconnected pins, two power outputs shorted together, or a power input that isn’t powered by anything. It also checks for some other mistakes like symbols that aren’t annotated and typos in net labels. To see the full list of electrical rules and to adjust their severity, go to File → Schematic Setup…​ → Electrical Rules → Violation Severity. It is a good idea to run ERC before starting layout.

Run an electrical rules check by clicking the ERC button () in the top toolbar and then clicking Run ERC.

Even in this simple schematic, KiCad has found two potential errors. The errors are listed in the ERC window, and arrows point to the violation locations in the schematic. Selecting a violation in the ERC window highlights the corresponding arrow.

You can exclude individual violations or ignore entire classes of violations by right clicking on each error message. However, it’s usually worth addressing the violations, even if they aren’t actual design errors, in order to get a clean ERC report and avoid missing real problems.

In this case, KiCad reports "Input Power pin not driven by any Output Power pins" for both the VCC and GND nets. This is a common KiCad ERC error. Power symbols are set up to require a power output pin, such as the output of a voltage regulator, on the same net; otherwise KiCad thinks the net is undriven. To a human, it is obvious that VCC and GND are driven by the battery, but it’s necessary to explicitly show that in the schematic.

There is a special PWR_FLAG symbol in the Power symbol library that is used to solve this problem by telling KiCad that the nets are actually driven. Add this symbol to the VCC and GND nets and re-run ERC. When ERC passes without any violations, the schematic is complete.

A final optional step is to generate a Bill of Materials listing all components used in the project. Click Tools → Generate BOM…​.

KiCad 7.0 uses Python scripts to generate BOMs. Three BOM scripts are included, and users can also create their own scripts to generate BOMs in whatever format is desired.

Select the bom_csv_grouped_extra script, and click generate. A CSV file containing BOM information is created in the project directory. The BOM generator also generates an intermediate XML file, which can be safely deleted.

Navigation in the PCB Editor is the same as the Schematic editor: pan by dragging with the middle mouse button or right mouse button, and zoom with the scrollwheel or F1/F2.

The main part of the PCB Editor is a canvas where the board will be designed. The toolbar on the left side has various display options for the board, including units and toggles for outline/filled display modes for tracks, vias, pads, and zones. The toolbar just to the right of the canvas contains tools for designing the PCB.

At far right is the Appearance Panel and Selection Filter. The Appearance panel is used to change visibility, colors, and opacity of PCB layers, objects, and nets. The active layer is changed by clicking on the name of a layer.

Below the Appearance Panel is the Selection Filter, which enables and disables selection of various types of PCB objects. This is useful to select specific items in a crowded layout.

Before designing the board, set the page size and add information to the title block. Click File → Page Settings…​, then choose an appropriate paper size and enter a date, revision, and title.

Next, go to File → Board Setup…​ to define how the PCB will be manufactured. The most important settings are the stackup, i.e. what copper and dielectric layers the PCB will have (and their thicknesses), and the design rules, e.g. sizes and spacing for tracks and vias.

To set the stackup, open the Board Stackup → Physical Stackup page of the Board Setup window. For this guide, leave the number of copper layers at 2, but more complicated projects might require more layers.

Next, go to the Design Rules → Constraints page. The settings on this page specify the overriding design rules for everything in the board design. For the purposes of this guide, the defaults are fine. However, for a real project these should be set according to the capabilities of the PCB fab house so that the PCB design is manufacturable.

Finally, open the Design Rules → Net Classes page. A net class is a set of design rules associated with a specific group of nets. This page lists the design rules for each net class in the design and allows assigning nets to each net class.

Track width and spacing can be managed manually by the designer during layout, but net classes are recommended because they provide an automatic way to manage and check design rules.

In this design, no net classes are specified, so all nets will belong to the Default net class. The default design rules for this net class are acceptable for this project, but other designs may have multiple net classes, each with different design rules. For example a board might have a High Current netclass with wide traces, or a 50 ohm netclass with specific width and clearance rules for 50 ohm controlled-impedance traces.

The schematic is complete, but there are not yet any components in the layout. To import design data from the schematic into the layout, click Tools → Update PCB from Schematic…​, or press F8. There is also a button in the top toolbar.

Read through the messages in the Changes To Be Applied window, which will say that the three components in the schematic will be added to the board. Click Update PCB, Close, and click on the canvas to place the three footprints. The location of each footprint relative to the others will be changed later.

In KiCad, updating the PCB with changes in the schematic is a manual process: the designer decides when it is appropriate to update the PCB with modifications in the schematic. Each time the schematic is edited, the designer must use the Update PCB from Schematic tool to keep the schematic and layout in sync.

Now the three components have been placed, but the board itself has not been defined. The board is defined by drawing a board outline on the Edge.Cuts layer.

It’s often useful to draw the board outline with a coarse grid, which makes it easy to get round numbers for the board size. Switch to a coarse grid by selecting 1mm in the Grid dropdown menu above the canvas.

To draw on the Edge.Cuts layer, click Edge.Cuts in the Layers tab of the Appearance panel at right. Choose the rectangle tool in the right toolbar, click on the canvas to place the first corner, then click again to place the opposite corner so that the rectangle roughly surrounds the three footprints. The other graphic tools (line , arc , circle , polygon , or a combination of them) could also be used to define the board outline; the only requirement is that the outline is a single closed shape that doesn’t intersect itself.

The next step in the layout process is to arrange the footprints on the board. In general, there are a several considerations for positioning footprints:

For the purposes of this guide, the only placement goal is to make the routing process as simple as possible.

Start by moving the battery holder BT1 onto the back side of the board. Click it to select it, then press M to move it. Press F to flip it to the opposite side; it now appears mirrored and its pads have changed from red to blue.

All PCB layers are viewed from front side of the board. Footprints on the bottom of the board are therefore upside down and appear mirrored.

Each PCB layer has a unique color, which is shown by the swatches in the Layers tab of the Appearance panel. In the default color scheme, items on the F.Cu (Front Copper) layer are red, while items on the B.Cu (Back Copper) are blue.

Now place the other two components. One at a time, select each component, then move and rotate it with M and R. Watch the ratsnest lines between each pad to choose the simplest arrangement of components; a good arrangement will leave the lines untangled. One possible arrangement is shown in the screenshot below.

With the components in place, it’s time to connect the pads with copper traces.

The first trace will be drawn on the front of the board, so change the active layer to F.Cu in the Layers tab of the Appearance panel.

Click Route Tracks in the right-hand toolbar or press X. Click on the led pad of D1. The ratsnest line indicates there is an unrouted connection to the led pad of R1, so click on that pad to draw a trace connecting the two pads. Clicking on the second pad completes the trace. The ratsnest line between the led pins is no longer drawn because the connection has been made in copper.

Now draw a trace between the GND pads of BT1 and D1, starting with the BT1 pad on the back of the board. Notice that the active layer automatically changed to B.Cu after clicking on the BT1 pad. Click on the D1 pad to finish the track.

While BT1 has surface mount pads that are only on the bottom of the board, D1 has through hole pads that can connect to tracks on both the front and back. Through hole pads are one way to make a connection between multiple layers. In this case, D1 is a component on the front side of the board, but its through hole pads are used to connect to a trace on the back of the board.

Another way to make a connection across layers is with a via. Start routing at the VCC pad of BT1 on the back of the board. Press V and click halfway between BT1 and R1 to insert a via, which also switches the active layer to F.Cu. Complete the track on the top side of the board by clicking on the VCC pad of R1.

At this point, all connections are routed. This can be confirmed by looking at the status screen in the bottom left of the window, where the number of unrouted nets is given as 0.

Copper zones are often used for ground and power connections because they provide a lower impedance connection than traces.

Add a GND zone on the bottom of the board by switching to the bottom copper layer and clicking the Add a filled zone button in the right toolbar. Click on the PCB to place the first corner of the zone.

In the Copper Zone Properties dialog that appears, select the GND net and make sure that the B.Cu layer is selected. Click OK, then click to place the other three corners of the zone. Double click when placing the last corner to complete the zone.

The zone outline is displayed on the canvas, but the zone is not yet filled — there is no copper in the zone area, and therefore the zone is not making any electrical connections. Fill the zone with Edit → Fill All Zones (B). Copper has been added to the zone, but it doesn’t connect to the VCC or led pads and traces, and is clipped by the board edge. It overlaps with the GND trace drawn earlier, and it connects to the GND pads through thin traces. These are thermal reliefs, which make the pads easier to solder. Thermal reliefs and other zone settings can be modified in the zone properties dialog.

In KiCad, zones are not filled automatically when they are first drawn or modified, or when footprints within them are moved. Zones are refilled by manually filling them and when running DRC. Make sure zone fills are up-to-date before generating fabrication outputs.

Sometimes filled zones can make it hard to see other objects in a crowded board design. Zones can be hidden except for their boundaries using the Show only zone boundaries button on the left-hand toolbar. Zones retain their filled status when only their outlines are shown — hiding a zone fill is not the same as unfilling it.

Zones can also be made transparent using the Appearance panel, and inactive layers can also be hidden or dimmed using the Layer Display Options in the Appearance Panel.

Design Rule Checking is the layout equivalent of Electrical Rule Checking for the schematic. DRC looks for design mistakes like mismatches between the schematic and layout, copper regions that have insufficient clearance or are shorted together, and traces that do not connect to anything. Custom rules can also be written in KiCad 7.0. To view the full list of design rules that are checked and to adjust their severity, go to File → Board Setup…​ → Design Rules → Violation Severity. Running DRC and fixing all errors is strongly advised before generating fabrication outputs.

Run a DRC check with Inspect → Design Rules Checker, or use the button in the top toolbar. Click Run DRC. When the checks are complete, no errors or warnings should be reported. Close the DRC window.

Now intentionally cause a DRC error by moving the resistor footprint to overlap the filled area of the zone. Use D (Drag) to move the resistor footprint slightly while keeping the traces attached to its pads. This creates a clearance violation because the VCC and led pads of the resistor are shorted to the GND zone fill. Ordinarily this would be fixed by refilling the zone, but don’t refill the zone yet.

Run DRC again, but make sure to uncheck the Refill all zones before performing DRC checkbox. DRC reports 6 violations: for each pad of R1, there is a clearance violation between the pad and the zone, another clearance violation between the pad’s through hole and the zone, and a third violation where the pad’s solder mask opening exposes the copper of two different nets (the GND fill and the trace connected to the pad). Arrows point to each violation in the canvas. Clicking on each violation message zooms in on the respective violation.

Close the DRC dialog, press B to refill the zone, and re-run DRC. Alternatively, check the Refill all zones before performing DRC checkbox and re-run DRC. All violations are fixed.

KiCad offers a 3D viewer that is useful for inspecting the PCB. Open the 3D viewer with View → 3D Viewer. Pan by dragging with the middle mouse button, and orbit by dragging with the left mouse button. Orbit around the PCB to see the LED and resistor on the top, and the battery holder on the bottom.

A raytracing mode is available, which is slower but offers more accurate rendering. Switch to the raytracing mode with Preferences → Raytracing.

Many of the footprints in KiCad’s library come with 3D models, including all of the footprints used in this guide. Some footprints do not come with 3D models, but users can add their own.

With the board design finished, the final step is to generate fabrication outputs so the board can be manufactured.

Open the Plot dialog with File → Plot…​. This dialog can plot the design in several formats, but Gerber is usually the right format for ordering from a PCB fabricator.

Specify an output directory so that the plotted files will be collected in a folder. Otherwise, the default settings are fine, but make sure all the necessary layers are checked: include the copper layers (*.Cu), board outline (Edge.Cuts), soldermask (*.Mask), and silkscreen (*.Silkscreen). The paste layers (*.Paste) are useful for manufacturing solder paste stencils. The Adhesive layers (*.Adhesive) are needed only if any components will be glued to the board during assembly. Other layers may be useful to plot, but are not typically necessary for PCB fabrication.

Click Plot to generate the Gerber files. Also click Generate Drill Files…​ and then Generate Drill File to create files specifying the location of all holes that will be drilled in the board. Finally, close the Plot dialog. The design is finished.

Symbols and footprints are organized into libraries. A library can hold symbols or footprints, but not both.

KiCad keeps track of the user’s symbol libraries and footprint libraries in the symbol library table and footprint library table, respectively. Each library table is a list of library names and the location of where each library exists on disk.

In addition to global symbol and footprint library tables, there are also project library tables for symbols and footprints. Symbols and footprints that are added to the global tables are available in all projects, while symbols and footprints in the project-specific tables are available only for that specific project. Users can add their own libraries to the global library tables or to project-specific tables.

The symbol library tables can be viewed or edited with Preferences → Manage Symbol Libraries…​ in the Schematic Editor or Symbol Editor windows. The footprint library tables can be viewed or edited with Preferences → Manage Footprint Libraries…​ in the Board Editor or Footprint Editor. Both library tables can also be accessed from the Project Manager.

Often, paths to libraries are defined with path substitution variables. This enables a user to move all of their libraries to a new location without modifying the library tables. The only thing that needs to change is to redefine the variable to point to the new location. KiCad’s path substitution variables are edited with Preferences → Configure Paths…​ in the Project Manager or any of the Editor windows.

One useful path substitution variable is ${KIPRJMOD}. This variable always points at the current project directory, so it can be used for including project-specific libraries that are stored inside the project directory.

On first run, KiCad prompts the user to set up the symbol library table and footprint library table. To go through this setup again, delete or rename the symbol library table or footprint library table files. Make a backup of the tables before deleting them.

The location of the symbol and footprint library table files depends on operating system.

The first step in drawing a new symbol or footprint is to choose a library in which to store it. For this guide, the switch symbol and footprint will go into new project-specific libraries.

Open the Symbol Editor from the Project Manager. Click File → New Library, and select Project. Choose a name for the new library (e.g. getting-started.kicad_sym) and save it in the project directory. The empty new library is now selected in the Libraries pane at left, and has been automatically added to the project library table (check the Project Specific Libraries tab in Preferences → Manage Symbol Libraries…​).

Now create the switch symbol in the new library. With the getting-started library selected in the Libraries pane, click File → New Symbol…​. In the Symbol name field, enter the part number: M2011S3A1W03. Switch symbols should have reference designators that start with SW, so change the Default reference designator field to SW. All other fields can remain as the defaults.

In the Libraries pane, the M2011S3A1W03 symbol now appears under the getting-started library. In the canvas, a cross indicates the center of the footprint, and text has been added for the symbol name and reference designator. For now, move the text away from the center of the footprint to get it out of the way.

Open the Footprint Editor and create a new project-specific footprint library named getting-started.pretty (File → New Library…​). As with symbol libraries, the new footprint library is added to the project library table. With the new library selected in the Libraries pane, create a new footprint (File → New Footprint…​). Set the name to Switch_Toggle_SPST_NKK_M2011S3A1x03 and the type to Through hole.

For more information on how to use KiCad, see the manual.

Other resources include the official KiCad user forum, Discord or IRC, and additional learning resources from the KiCad community.

To see more of what’s possible with KiCad, browse the Made With KiCad section of the website, or open the demo projects included with KiCad (File → Open Demo Project…​).

To report a bug or request a feature, please use Help → Report a Bug or open an issue on Gitlab.

To contribute to KiCad’s development, please see the Developer Contribution page. Users can also help by contributing to the libraries or documentation and translation. Finally, consider financially supporting continued development of KiCad.