Pcbnew

Pcbnew is a powerful printed circuit board software tool available for the Linux, Microsoft Windows and Apple OS X operating systems. Pcbnew is used in association with the schematic capture program Eeschema to create printed circuit boards.

Pcbnew manages libraries of footprints. Each footprint is a drawing of the physical component including its land pattern (the layout of pads on the circuit board). The required footprints are automatically loaded during the reading of the Netlist. Any changes to footprint selection or annotation can be changed in the schematic and updated in pcbnew by regenerating the netlist and reading it in pcbnew again.

Pcbnew provides a design rules check (DRC) tool which prevents track and pad clearance issues as well as preventing nets from being connected that aren’t connected in the netlist/schematic. When using the interactive router it continuously runs the design rules check and will help automatically route individual traces.

Pcbnew provides a rats nest display, a hairline connecting the pads of footprints which are connected on the schematic. These connections move dynamically as track and footprint movements are made.

Pcbnew has a simple but effective autorouter to assist in the production of the circuit board. An Export/Import in SPECCTRA dsn format allows the use of more advanced auto-routers.

Pcbnew provides options specifically provided for the production of ultra high frequency microwave circuits (such as pads of trapezoidal and complex form, automatic layout of coils on the printed circuit, etc).

The smallest unit in pcbnew is 1 nanometer. All dimensions are stored as integer nanometers.

Pcbnew can generate up to 32 layers of copper, 14 technical layers (silk screen, solder mask, component adhesive, solder paste and edge cuts) plus 4 auxiliary layers (drawings and comments) and manages in real time the hairline indication (rats nest) of missing tracks.

The display of the PCB elements (tracks, pads, text, drawings…) is customizable:

For complex circuits, the display of layers, zones, and components can be hidden in a selective way for clarity on screen. Nets of traces can be highlighted to provide high contrast as well.

Footprints can be rotated to any angle, with a resolution of 0.1 degree.

Pcbnew includes a Footprint Editor that allows editing of individual footprints that have been on a pcb or editing a footprint in a library.

The Footprint Editor provides many time saving tools such as:

Footprint pads have a variety of properties that can be adjusted. The pads can be round, rectangular, oval or trapezoidal. For through-hole parts drills can be offset inside the pad and be round or a slot. Individual pads can also be rotated and have unique soldermask, net, or paste clearance. Pads can also have a solid connection or a thermal relief connection for easier manufacturing. Any combination of unique pads can be placed within a footprint.

Pcbnew easily generates all the documents necessary for production:

Due to the degree of control necessary it is highly suggested to use a 3-button mouse with pcbnew. Many features such as panning and zooming require a 3-button mouse.

In the new release of KiCad, pcbnew has seen wide sweeping changes from developers at CERN. This includes features such as a new renderer (OpenGL and Cairo view modes), an interative push and shove router, differential and meander trace routing and tuning, a reworked Footprint Editor, and many other features. Please note that most of these new features only exist in the new OpenGL and Cairo view modes.

The installation procedure is described in the KiCad documentation.

A default configuration file kicad.pro is provided in kicad/share/template. This file is used as the initial configuration for all new projects.

This configuration file can be modified to change the libraries to be loaded.

To do this:

You can have access to the library list initialization from the Preferences menu:

The image below shows the dialog which allows you to set the footprint library list:

You can use this to add all the libraries that contain the footprints required for your project. You should also remove unused libraries from new projects to prevent footprint name clashes. Please note, there is an issue with the footprint library list when duplicate footprint names exist in more than one library. When this occurs, the footprint will be loaded from the first library found in the list. If this is an issue (you cannot load the footprint you want), either change the library list order using the "Up" and "Down" buttons in the dialog above or give the footprint a unique name using the footprint editor.

As of release 4.0, Pcbnew uses the new footprint library table implementation to manage footprint libraries. The information in the previous section is no longer valid. The library table manager is accessible by:

The image below shows the footprint library table editing dialog which can be opened by invoking the "Footprint Libraries Manager" entry from the "Preferences" menu.

The footprint library table is used to map a footprint library of any supported library type to a library nickname. This nickname is used to look up footprints instead of the previous method which depended on library search path ordering. This allows Pcbnew to access footprints with the same name in different libraries by ensuring that the correct footprint is loaded from the appropriate library. It also allows Pcbnew to support loading libraries from different PCB editors such as Eagle and gEDA.

In Pcbnew it is possible to execute commands using various means:

The screenshot below illustrates some of the possible accesses to these operations:

During element layout the cursor moves on a grid. The grid can be turned on or off using the icon on the left toolbar.

Any of the pre-defined grid sizes, or a User Defined grid, can be chosen using the pop-up window, or the drop-down selector on the toolbar at the top of the screen. The size of the User Defined grid is set using the menu bar option Dimensions → User Grid Size.

The zoom level can be changed using any of the following methods:

The cursor coordinates are displayed in inches or millimetres as selected using the In or mm icons on the left hand side toolbar.

Whichever unit is selected Pcbnew always works to a precision of 1/10,000 of inch.

The status bar at the bottom of the screen gives:

In addition the relative position of the cursor can be displayed using its polar co-ordinates (ray + angle). This can be turned on and off using the icon in the left hand side toolbar.

Many commands are accessible directly with the keyboard. Selection can be either upper or lower case. Most hot keys are shown in menus. Some hot keys that do not appear are:

Operations to move, invert (mirror), copy, rotate and delete a block are all available from the pop-up menu. In addition, the view can zoom to that described by the block.

The framework of the block is traced by moving the mouse while holding down the left mouse button. The operation is executed when the button is released.

By holding down one of the keys Shift or Ctrl, both Shift and Ctrl together, or Alt, while the block is drawn the operation invert, rotate, delete or copy is automatically selected as shown in the table below:

When a block command is made, a dialog window is displayed, and items involved in this command can be chosen.

Any of the commands above can be cancelled via the same pop-up menu or by pressing the Escape key (Esc).

Units used to display dimensions values are inch and mm. The desired unit can be selected by pressing the icon located in left toolbar: However one can enter the unit used to define a value, when entering a new value.

Accepted units are:

The rules are:

The top menu bar provides access to the files (loading and saving), configuration options, printing, plotting and the help files.

This toolbar gives access to the principal functions of Pcbnew.

This toolbar gives access to the editing tool to change the PCB shown in Pcbnew.

The left hand-side toolbar provides display and control options that affect Pcbnew’s interface.

A right-click of the mouse opens a pop-up window. Its contents depends on the element pointed at by the cursor.

This gives immediate access to:

The screenshots below show what the pop-up windows looks like.

There are 3 modes when using pop-up menus. In the pop-up menus, these modes add or remove some specific commands.

Generally speaking, a schematic sheet is linked to its printed circuit board by means of the netlist file, which is normally generated by the schematic editor used to make the schematic. Pcbnew accepts netlist files made with Eeschema or Orcad PCB 2. The netlist file, generated from the schematic is usually missing the footprints that correspond to the various components. Consequently an intermediate stage is necessary. During this intermediate process the association of components with footprints is performed. In KiCad, CvPcb is used to create this association and a file named *.cmp is produced. CvPcb also updates the netlist file using this information.

CvPcb can also output a "stuff file" *.stf which can be back annotated into the schematic file as the F2 field for each component, saving the task of re-assigning footprints in each schematic edit pass. In Eeschema copying a component will also copy the footprint assignment and set the reference designator as unassigned for later auto-incremental annotation.

Pcbnew reads the modified netlist file .net and, if it exists, the .cmp file. In the event of a footprint being changed directly in Pcbnew the .cmp file is automatically updated avoiding the requirement to run CvPcb again.

Refer to the figure of "Getting Started in KiCad" manual in the section KiCad Workflow that illustrates the work-flow of KiCad and how intermediate files are obtained and used by the different software tools that comprise KiCad.

After having created your schematic in Eeschema:

Pcbnew will then load automatically all the necessary footprints. Footprints can now be placed manually or automatically on the board and tracks can be routed.

If the schematic is modified (after a printed circuit board has been generated), the following steps must be repeated:

Pcbnew will then load automatically any new footprints, add the new connections and remove redundant connections. This process is called forward annotation and is a very common procedure when a PCB is made and updated.

Some are associated in pairs, others not. When they appear as a pair this affects the behaviour of footprints. The elements making up a footprint (pads, drawing and text) appearing on a layer (solder or component), appear on the other complementary layer when the footprint is inverted (mirrored).

The technical layers are:

The selection of the active working layer can be done in several ways:

If the Add Tracks and Vias icon is selected on the right hand toolbar, the Pop-Up window provides the option to change the layer pair used for vias:

This selection opens a menu window which provides choice of the layers used for vias.

When a via is placed the working (active) layer is automatically switched to the alternate layer of the layer pair used for the vias.

One can also switch to an other active layer by hot keys, and if a track is in progress, a via will be inserted.

This mode is entered when the tool (in the left toolbar) is activated:

When using this mode, the active layer is displayed like in the normal mode, but all others layers are displayed in gray color.

There are two useful cases:

It is very often necessary to correct a board following a corresponding change in the schematic.

Changing a footprint ( or some identical footprints) to another footprint is very useful, and is very easy:

Options for Change Footprint(s):

One must choose a new footprint name and use:

Whilst moving footprints the footprint ratsnest (the net connections) can be displayed to assist the placement. To enable this the icon of the left toolbar must be activated.

Select the footprint with the right mouse button then choose the Move command from the menu. Move the footprint to the required position and place it with the left mouse button. If required the selected footprint can also be rotated, inverted or edited. Select Cancel from the menu (or press the Esc key) to abort.

Here you can see the display of the footprint ratsnest during a move:

The circuit once all the footprints are placed may be as shown:

Initially all footprints inherit the same orientation that they had in the library (normally 0).

If an alternative orientation is required for an individual footprint, or all footprints (for example all vertical) use the menu option AutoPlace/Orient All Footprints. This orientation can be selective (for example to relate only to the footprints whose reference starts with "IC".

Generally speaking, footprints can only be moved if they have not been "Fixed". This attribute can be turned on and off from the pop-up window (click right mouse button over footprint) whilst in Footprint Mode, or through the Edit Footprint Menu.

As stated in the last chapter, new footprints loaded during the reading of the netlist appear piled up at a single location on the board. Pcbnew allows an automatic distribution of the footprints to make manual selection and placement easier.

If there is a footprint under the cursor:

If there is nothing under the cursor:

In both cases the following commands are available:

The General options menu is available via the top toolbar link Preferences → General dialog.

The dialog looks like the following:

For the creation of tracks the necessary parameters are:

Pcbnew allows you to define different routing parameters for each net. Parameters are defined by a group of nets.

A netclass specifies:

Manual routing is often recommended, because it is the only method offering control over routing priorities. For example, it is preferable to start by routing power tracks, making them wide and short and keeping analog and digital supplies well separated. Later, sensitive signal tracks should be routed. Amongst other problems, automatic routing often requires many vias. However, automatic routing can offer a useful insight into the positioning of footprins. With experience, you will probably find that the automatic router is useful for quickly routing the obvious tracks, but the remaining tracks will best be routed by hand.

Pcbnew can display the full ratsnest, if the button is activated.

The button allows one to highlight a net (click to a pad or an existing track to highlight the corresponding net).

The DRC checks tracks in real time while creating them. One cannot create a track which does not match the DRC rules. It is possible to disable the DRC by clicking on the button. This is, however, not recommended, use it only in specific cases.

When clicking on a track or a pad, Pcbnew automatically selects the corresponding Netclass, and the track size and vias dimensions are derived from this netclass.

As previously seen, the Global Design Rules editor has a tool to insert extra tracks and vias sizes.

Before using the Interactive Router, please set up these two things:

To activate the router tool press the Interactive Router button or the X key. The cursor will turn into a cross and the tool name, will appear in the status bar.

To start a track, click on any item (a pad, track or a via) or press the X key again hovering the mouse over that item. The new track will use the net of the starting item. Clicking or pressing X on empty PCB space starts a track with no net assigned.

Move the mouse to define shape of the track. The router will try to follow the mouse trail, hugging unmovable obstacles (such as pads) and shoving colliding traces/vias, depending on the mode. Retreating the mouse cursor will cause the shoved items to spring back to their former locations.

Clicking on a pad/track/via in the same net finishes routing. Clicking in empty space fixes the segments routed so far and continues routing the trace.

In order to stop routing and undo all changes (shoved items, etc.), simply press Esc.

Pressing V or selecting Place Through Via from the context menu while routing a track attaches a via at the end of the trace being routed. Pressing V again disables via placement. Clicking in any spot establishes the via and continues routing.

Pressing / or selecting Switch Track Posture from the context menu toggles the direction of the initial track segment between straight or diagonal.

There are several ways to pre-select a track width/via size or to change it during routing:

The router can drag track segments, corners and vias. To drag an item, click on it with Ctrl key pressed, hover the mouse and press G or select Drag Track/Via from the context menu. Finish dragging by clicking again or abort by pressing Esc.

The router behavior be configured by pressing E or selecting Routing Options from the context menu while in the Track mode. It opens a window like the one below:

The options are:

Pad (and track) connections to filled copper areas are checked by the DRC engine. A zone must be filled (not just created) to connect pads. Pcbnew currently uses track segments or polygons to fill copper areas.

Each option has its advantages and its disadvantages, the main disadvantage being increased screen redraw time on slower machines. The final result is however the same.

For calculation time reasons, the zone filling is not recreated after each change, but only:

Copper zones must be filled or refilled after changes in tracks or pads are made. Copper zones (usually ground and power planes) are usually attached to a net.

In order to create a copper zone you should:

Pcbnew tries to fill all zones in one piece, and usually, there will be no unconnected copper blocks. It can happen that some areas remain unfilled. Zones having no net are not cleaned and can have insulated areas.

When you fill an area, you must choose:

A zone must already exist. To add a cutout area (a non-filled area inside the zone):

An outline can be modified by:

If polygons are overlapping they will be combined.

To do that, right-click on a corner or on an edge, then select the proper command.

Here is a corner (from a cutout) that has been moved:

Here is the final result:

Polygons are combined.

When right-clicking on an outline, and using Edit Zone Params the Zone params Dialog box will open. Initial parameters can be inputted . If the zone is already filled, refilling it will be necessary.

When the board is finished, one must fill or refill all zones. To do this:

After editing a schematic, you can change the name of any net. For instance VCC can be changed to +5V.

When a global DRC control is made Pcbnew checks if the zone net name exists, and displays an error if not.

Manually editing the zone parameters will be necessary to change the old name to the new one.

Select the tool

The active layer should be a copper layer.

After clicking on the starting point of a new keepout area, the dialog box is opened:

One can select disallowed items:

When a track or a via is inside a keepout which does not allow it, a DRC error will be raised.

For copper zones, the area inside a keepout with no copper pour will be not filled. A keep-out area is a like a zone, so editing its outline is analogous to copper zone editing.

The generation of the necessary files for the production of your printed circuit board includes the following preparatory steps.

Here is an example showing all of these elements, except ground planes, which have been omitted for better visibility:

A color key for the 4 copper layers has also been included:

Before generating the output files, a global DRC test is very strongly recommended.

Zones are filled or refilled when starting a DRC. Press the button to launch the following DRC dialog:

Adjust the parameters accordingly and then press the "Start DRC" button.

This final check will prevent any unpleasant surprises.

Set the coordinates origin for the photo plot and drill files, one must place the auxiliary axis on this origin. Activate the icon . Move the auxiliary axis by left-clicking on the chosen location.

This is done via the Files/Plot menu option and invokes the following dialog:

Usually, the files are in the GERBER format. Nevertheless, it is possible to produce output in both HPGL and POSTSCRIPT formats. When Postscript format is selected, this dialog will appear.

In these formats, a fine scale adjust can be used to compensate for the plotter accuracy and to have a true scale of 1 for the output:

Mask clearance values can be set globally for the solder mask layers and the solder paste layers. These clearances can be set at the following levels.

And Pcbnew uses by priority order.

The creation of a drill file xxxx.drl following the EXCELLON standard is always necessary.

One can also produce an optional drill report, and an optional drill map.

The generation of these files is controlled via:

The Drill tools dialog box will be the following:

For setting the coordinate origin, the following dialog box is used:

To produce wiring documentation files, the component and copper silkscreen layers can be traced. Usually, just the component-side silkscreen markings are sufficient for wiring a PCB. If the copper-side silkscreen is used, the text it contains should be mirrored in order to be readable.

This option is accessed via the Postprocess/Create Cmp file menu option. However, no file will be generated unless at least one footprint has the Normal+Insert attribute activated (see Editing Footprints). One or two files will be produced, depending upon whether insertable components are present on one or both sides of the PCB. A dialogue box will display the names of the file(s) created.

The options described below (part of the Files/Plot dialogue) allow for fine-grained control of the tracing process. They are particularly useful when printing the silkscreen markings for wiring documentation.

The available options are:

Pcbnew can simultaneously maintain several libraries. Thus, when a footprint is loaded, all libraries that appear in the library list are searched until the first instance of the footprint is found. In what follows, note that the active library is the library selected within the Footprint Editor, the program will now be described

Footprint Editor enables the creation and the editing of footprints:

Footprint Editor allows the maintenance of the active library as well by:

It is also possible to create new libraries.

The library extension is .mod.

The Footprint Editor can be accessed in two different ways:

In this case, the active footprint of the board will be loaded automatically in Footprint Editor, enabling immediate editing or archiving.

By calling Footprint Editor the following window will appear:

From this toolbar, the following functions are available:

The creation of a new library is done via the button , in this case the file is created by default in the library directory or via the button , in which case the file is created by default in your working directory.

A file-choosing dialog allows the name of the library to be specified and its directory to be changed. In both cases, the library will contain the footprint being edited.

The action of saving a footprint (thereby modifying the file of the active library) is performed using this button . If a footprint of the same name already exists, it will be replaced. Since you will depend upon the accuracy of the library footprints, it is worth double-checking the footprint before saving.

It is recommended to edit either the reference or value field text to the name of the footprint as identified in the library.

You may also wish to delete the source footprint.

It is possible to copy all of the footprints of a given board design to the active library. These footprints will keep their current library names. This command has two uses:

It is strongly recommended to document the footprints you create, in order to enable rapid and error-free searching.

For example, who is able to remember all of the multiple pin-out variants of a TO92 package? The Footprint Properties dialog offers a simple solution to this problem.

This dialog accepts:

The description is displayed with the component list in Cvpcb and, in Pcbnew, it is used in the footprint selection dialogs.

The keywords enable searches to be restricted to those footprints corresponding to particular keywords.

When directly loading a footprint (the icon of the right-hand Pcbnew toolbar), keywords may be entered in the dialog box. Thus, entering the text =CONN will cause the display of the list of footprints whose keyword lists contain the word CONN.

It is recommended to create libraries indirectly, by creating one or more auxiliary circuit boards that constitute the source of (part of) the library, as follows: Create a circuit board in A4 format, in order to be able to print easily to scale (scale = 1).

Create the footprints that the library will contain on this circuit board. The library itself will be created with the File/Archive footprints/Create footprint archive command.

The "true source" of the library will thus be the auxiliary circuit board, and it is on this circuit that any subsequent alterations of footprints will be made. Naturally, several circuit boards can be saved in the same library.

It is generally a good idea to make different libraries for different kinds of components (connectors, discretes,…), since Pcbnew is able to search many libraries when loading footprints.

Here is an example of such a library source:

This technique has several advantages:

The list of footprint libraries in Pcbnew can be edited using the Footprint Libraries Manager. This allows you to add and remove footprint libraries by hand, and also allows you to invoke the Footprint Libraries Wizard by pressing the "Append With Wizard" button.

The Footprint Libraries Wizard can also be invoked through the Preferences menu, and can automatically add a library (detecting its type) from a file or from a Github URL. The URL for the official libraries is: https://github.com/KiCad

More details about footprint library tables and the Manager and Wizard can be found in the CvPcb Reference Manual in the section Footprint Library Tables.

The 3D shape libraries can be downloaded by 3D Shape Libraries Wizard. It can be invoked from the menu Preferences → 3D Shapes Libraries Downloader.

Footprint Editor is used for editing and creating PCB footprints. This includes:

A footprint is the physical representation (footprint) of the part to be inserted in the PCB and it must be linked to the relative component in your schematic. Each footprint includes three different elements:

In addition, a number of other parameters must be correctly defined if the auto-placement function will be used. The same holds for the generation of auto-insertion files.

Footprint Editor can be started in two ways:

Calling Footprint Editor will launch a new window that looks like this:

The right mouse button calls up menus that depend upon the element beneath the cursor.

The context menu for editing footprint parameters:

The context menu for editing pads:

The context menu for editing graphic elements:

This dialog can be launched when the cursor is over a footprint by clicking on the right mouse button and then selecting Edit Footprint.

The dialog can be used to define the main footprint parameters.

A new footprint can be created via the button . The name of the new footprint will be requested. This will be the name by which the footprint will be identified in the library.

This text also serves as the footprint value, which is ultimately replaced by the real value (100uF_16V, 100_0.5W, …).

The new footprint will require:

Alternative method:

When a new footprint is similar to an existing footprint in a library or a circuit board, an alternative and quicker method of creating the new footprint is as follows:

Once a footprint has been created, pads can be added, deleted or modified. Modification of pads can be local, affecting only the pad under the cursor, or global, affecting all pads of the footprint.

There are at least two fields: reference and value.

Their parameters (attribute, size, width) must be updated. You can access the dialog box from the pop-up menu, by double clicking on the field, or by the footprint properties dialog box:

If the user wishes to exploit the the full capabilities of the auto-placement functions, it is necessary to define the allowed orientations of the footprint (Footprint Properties dialog).

Usually, rotation of 180 degrees is permitted for resistors, non-polarized capacitors and other symmetrical elements.

Some footprints (small transistors, for example) are often permitted to rotate by +/- 90 or 180 degrees. By default, a new footprint will have its rotation permissions set to zero. This can be adjusted according to the following rule:

A value of 0 makes rotation impossible, 10 allows it completely, and any intermediate value represents a limited rotation. For example, a resistor might have a permission of 10 to rotate 180 degrees (unrestrained) and a permission of 5 for a +/- 90 degree rotation (allowed, but discouraged).

The attributes window is the following:

It is strongly recommended to document newly created footprints, in order to facilitate their rapid and accurate retrieval. Who is able to recall the multiple pin-out variants of a TO92 footprint?

The Footprint Properties dialog offers a simple and yet powerful means for documentation generation.

This menu allows:

The comment line is displayed with the component list in CvPcb and in the footprint selection menus in Pcbnew. The keywords can be used to restrict searches to those parts possessing the given keywords.

Thus, while using the load footprint command (icon in the right-hand toolbar in Pcbnew), it is possible to type the text =TO220 into the dialog box to have Pcbnew display a list of the footprints possessing the keyword TO220

A footprint may have been associated with a file containing a three-dimensional representation of itself. In order to associate such a file with a footprint, select the 3D Settings tab. The options panel is the following:

The data information should be provided:

Setting scale allows:

If such a file has been specified, it is possible to view the component in 3D.

The 3D model will automatically appear in the 3D representation of the printed circuit board.

The save command (modification of the file of the active library) is activated by the button.

If a footprint of the same name exists (an older version), it will be overwritten. Because it is important to be able to have confidence in the library footprints, it is worth double-checking the footprint for errors before saving.

Before saving, it is also recommended to change the reference or value of the footprint to be equal to the library name of the footprint.

If the edited footprint comes from the current board, the button will update this footprint on the board.

Duplication is a method to clone an item and pick it up in the same action. It is broadly similar to copy-and-pasting, but it allows you to "sprinkle" components over the PCB and it allows you to manually lay out components using the "Move Exact" tool (see below) more easily.

Duplication is done by using the hotkey (which defaults to Ctrl-D) or the duplicate item option in the context menu. In the legacy renderer, these appear as below, depending on the item type:

The "Move Exact" tool allows you to move an item (or group of items) by a certain amount, which can be entered in Cartesian or polar formats and which can be entered in any supported units. This is useful when it would otherwise be cumbersome to switch to a different grid, or when a feature is not spaced according to any existing grids.

To use this tools, select the items you wish to move and then use either the hotkey (defaults to Ctrl-M) or the context menu items to invoke the dialog. You can also invoke the dialog with the hotkey when moving or duplicating items, which can make it easy to repeatedly apply an offset to multiple components.

Move exact with Cartesian move vector entry

Move exact with polar move vector entry

The checkbox allows you to switch between Cartesian and polar co-ordinate systems. Whatever is currently in the form will be converted automatically to the other system.

Then you enter the desired move vector. You can use the units indicated by the labels ("mm" in the images above) or you can specify the units yourself (e.g. "1 in" for an inch, or "2 rad" for 2 radians).

Pressing OK will apply the translation to the selection, and cancel will close the dialog and the items will not be moved. If OK is pressed, the move vector will be saved and pre-filled next time the dialog is opened, which allows repeated application of the same vector to multiple objects.

Pcbnew and the Footprint Editor both have assistants for creating arrays of features and components, which can be used to easily and accurately lay out repetitive elements on PCBs and in footprints.

The scripting API reflects the internal object structure inside KiCad/pcbnew. BOARD is the main object, that has a set of properties and a set of MODULEs, and TRACKs/SEGVIAs, TEXTE_PCB, DIMENSION, DRAWSEGMENT. Then MODULEs have D_PADs, EDGEs, etc.

All the pcbnew API is provided from the "pcbnew" module in Python. GetBoard() method will return the current pcb open at editor, useful for commands written from the integrated scripting shell inside pcbnew or action plugins.

Board is the basic object in KiCad pcbnew, it’s the document.

BOARD contains a set of object lists that can be accessed using the following methods, they will return iterable lists that can be iterated using "for obj in list:"

The footprint wizards are a collection of python scripts that can be access via from the Footprint Editor. If you invoke the footprint dialog you select a given wizard that allows you to see the footprint rendered, and you have some parameters you can edit.

If the plugins are not properly distributed to your system package, you can find the latest versions in the KiCad source tree at launchpad.

They should be located in for example C:\Program Files\KiCad\bin\scripting\plugins.

On linux you can also keep your user plugins in $HOME/.kicad_plugins.