我的书签
添加书签
移除书签Creating a PCB
Basic PCB concepts
A printed circuit board in KiCad is generally made up of footprints representing electronic components and their pads, nets defining how those pads connect to each other, tracks, vias, and filled zones that form the copper connections between pads in each net, and various graphic shapes defining the board edge, silkscreen markings, and any other desired information.
KiCad normally keeps the information about nets on a PCB synchronized with an associated schematic, but nets can also be created and edited directly within the PCB editor.
Capabilities
KiCad is capable of creating printed circuit boards with up to 32 copper layers, 14 technical layers (silkscreen, solder mask, component adhesive, solder paste, etc), and 13 general-purpose drawing layers.
The internal measurement resolution of all objects in KiCad is 1 nanometer, and measurements are stored as 32-bit integers. This means it is possible to create boards up to appproximately 4 meters by 4 meters.
KiCad currently supports one board file per project / schematic.
Starting from a schematic
Creating a board from a schematic is the recommended workflow for KiCad. When you create a new project, KiCad will generate an empty board file with the same name as the project. To start designing the board after you have created a schematic, simply open the board file. You can do this either from the KiCad project manager, or by clicking the “Open PCB in board editor” button in the schematic editor.
Starting from scratch
It is also possible to create a board with no matching schematic, although this workflow has some limitations and is not recommended for most users. To do this, you must start the PCB editor standalone (not from the KiCad project manager). Before beginning your design, it is a good idea to save the board file, which will also create a project file to store board settings. Use “Save As…” from the File menu to choose where to save your board file. A project file with the same name will be created in the same location you choose to save the board file in.
Board setup
Before beginning your board design, use the Board Setup dialog to configure the basic parameters of the board. To open Board Setup, click the 
icon in the top toolbar or choose “Board Setup…” from the File menu.
Configuring board stackup and physical parameters
There are two sections of Board Setup used to configure the stackup and layers of the board. The Board Editor Layers section is used to enable or disable technical (non-copper) layers, and give custom names to layers if desired. The Physical Stackup section is used to configure the number of copper layers, as well as the physical parameters of the copper and dielectric layers such as thickness and material type.
To configure the board stackup, start on the Physical Stackup section:
Set the number of copper layers in the upper left corner and then enter the physical parameters of the stackup if desired. These parameters may be left at their default values, but note that the board thickness value will be used when exporting a 3D model of the board. If you plan to use this feature, it is a good idea to ensure that the stackup thickness is correct.
| KiCad currently only supports stackups with an even number of copper layers. To create designs with an odd number of layers (for example, flexible printed circuits or metal-core printed circuits), simply choose the next highest even number and ignore the extra layer. |
Next, if desired, use the Board Editor Layers section to rename layers or hide non-copper layers that you will not be using in the design. For example, if you will not use a back silkscreen on the design, uncheck the box next to the B.Silkscreen layer.
| Copper layers can be designated as signal, power plane, mixed, or jumper in the Board Editor Layers section. This designation is intended as a guide for the user only. Tracks and zones can be routed on any copper layer, no matter what the type is configured to in this dialog. |
Some additional board stackup settings are found on the Board Finish and Solder Mask/Paste sections of the Board Setup dialog. The Board Finish section has settings for defining the copper finish and special features such as castellations or edge plating. Note that these settings only impact the board attributes output as part of Gerber job files at this time.
The Solder Mask/Paste section allow global adjustment of the clearance (positive or negative) between the copper shapes and solder mask / solder paste shapes of pads on the board. These values will be added to any clearance overrides set on individual footprints or pads. Positive clearance values will result in the shape of the solder mask or paste opening being larger than the copper shape. Negative clearance values will result in the opening being smaller than the copper shape.
| Most commercial PCB fabricators expect these values to be zero and make their own adjustments to solder mask and paste openings as part of their CAM process. It is usually best to leave these values at their default of zero unless you are making the PCB yourself or have specific advice from your fabricator to use different values. |
Configuring default text and graphic settings
The Text & Graphics Defaults section of the Board Setup dialog can be used to configure the properties that will be used for new text and graphic shapes that are placed on the board.
Line thickness, text size, and text appearance can be configured for the six different categories of layers shown in the dialog. Additionally, the properties for dimension objects can be configured for all layers. For more details about dimension properties, see the Dimensions section below.
Text replacement variables can be created in the Text Variables section. These variables allow you to substitute the variable name for any text string. This substitution happens anywhere the variable name is used inside the variable replacement syntax of ${VARIABLENAME}.
For example, you could create a variable named VERSION and set the text substitution to 1.0. Now, in any text object on the PCB, you can enter ${VERSION} and KiCad will substitute 1.0. If you change the substitution to 2.0, every text object that includes ${VERSION} will be updated automatically. You can also mix regular text and variables. For example, you can create a text object with the text Version: ${VERSION} which will be substituted as Version: 1.0.
Configuring design rules
Design rules control the behavior of the interactive router, the filling of copper zones, and the design rule checker. Design rules can be modified at any time, but we recommend that you establish all known design rules at the beginning of the board design process.
Constraints
Basic design rules are configured in the Constraints section of the Board Setup dialog. Constraints in this section apply to the entire board and should be set to the values recommended by your board manufacturer. Any minimum value set here is an absolute minimum and cannot be overridden with a more specific design rule. For example, if you need the copper clearance on part of a board to be 0.2mm and in the rest 0.3mm, you must enter 0.2mm for the minimum copper clearance in the Constraints section and use a netclass or custom rule to set the larger 0.3mm clearance.
In addition to setting minimum clearances, a number of features can be configured here:
| Setting | Description |
|---|---|
Allow blind/buried vias | This setting must be enabled before you can place blind or buried vias using the router. Blind vias are mechanically-drilled vias that start at one of the outer copper layers but end at one of the inner layers. Buried vias are mechanically-drilled vias that start and end at inner copper layers. |
Allow micro vias | This setting must be enabled before you can place microvias using the router. Microvias are typically laser-drilled vias that connect an outer copper layer to the adjacent inner layer. KiCad supports a separate size constraint for microvias as they typically can be smaller than mechanically-drilled vias. |
Arc/circle approximated by segments | In some situations, KiCad must use a series of straight line segments to approximate round shapes such as those of arcs and circles. This setting controls the maximum error allowed by this approximation: in other words, the maximum distance between a point on one of these line segments and the true shape of the arc or circle. Setting this to a lower number than the default value of 0.005mm will result in smoother shapes, but can be very slow on larger boards. The default value typically results in arc approximation error that is not detectable in the manufactured board due to manufacturing tolerances. |
Zone fill strategy | KiCad’s zone filling algorithm has been improved to give better results and faster performance. The new algorithm produces slightly different results from the old algorithm, so this setting allows the old behavior to be preserved to prevent producing different Gerber outputs when opening an old design in the latest version of KiCad. We recommend using the Smoothed Polygons mode for all new designs. |
Allow fillets outside zone outline | Zones can have fillets (rounded corners) added in the Zone Properties dialog. By default, no zone copper, including fillets, is allowed outside the zone outline. This effectively means that inside corners of the zone outline will not be filleted even when a fillet is configured. By enabling this setting, inside corners of the zone outline will be filleted even though this results in copper from the zone extending outside the zone outline. |
Include stackup height in track length calculations | By default, the height of the stackup is used to calculate the additional length of a track that travels through vias from one layer to another. This calculation relies on the board stackup height being correctly configured. In some situations, it is preferable to ignore the height of vias and just calculate the track length assuming that vias add no length. Disabling this setting will exclude via length from track length calculations. |
Pre-defined Sizes
The pre-defined sizes section allows you to define the track and via dimensions you want to have available while routing tracks. Net classes can be used to define the default dimensions for tracks and vias in different nets (see below) but defining a list of sizes in this section will allow you to step through these sizes while routing. For example, you may want the default track width on a board to be 0.2 mm, but use 0.3 mm for some sections that carry more current, and 0.15 mm for some sections where space is limited. You can define each of these track widths in the Board Setup dialog and then switch between them when routing traces.
Net Classes
The Net Classes section allows you to configure routing and clearance rules for different classes of nets. In KiCad, each net is part of exactly one net class. If you do not add a net to a specific class, it will be part of the Default class, which always exists. Nets may be added to net classes from either the schematic or PCB editor, via the Schematic Setup and Board Setup dialogs.
The upper portion of the Net Classes section contains a table showing the design rules that apply to each net class. Every class has values for copper clearance, track width, via sizes, and differential pair sizes. These values will be used when creating tracks and vias unless a more specific rule overrides them (see Custom Rules below).
No rule may override the minimum values set in the Constraints section of Board Setup. For example, if you set a net class clearance to 0.1 mm, but the Minimum Clearance in the Constraints section is set to 0.2 mm, nets in that class will have a clearance of 0.2 mm. |
The track widths and via sizes defined for each net class are used when the track width and via size controls are set to “use netclass values” in the PCB editor. These widths and sizes are considered the default, or optimal, sizes for that netclass. They are not minimum or maximum values. Manually changing the track width or via size to a different value from that defined in the Net Classes section will not result in a DRC violation. To restrict track width or via size to specific values, use Custom Rules.
Custom Rules
The Custom Rules section contains a text editor for creating design rules using the custom rules language. Custom rules are used to create specific design rule checks that are not covered by the basic constraints or net class settings.
Custom rules will only be applied if there are no errors in the custom rules definitions. Use the Check Rule Syntax button to test the definitions and fix any problems before closing Board Setup.
See Custom Design Rules in the Advanced Topics chapter for more information on the custom rules language as well as example rules.
Violation Severity
The Violation Severity section allows you to configure the severity of each type of design rule check. Each rule may be set to create an error marker, a warning marker, or no marker (ignored).
| Individual rule violations may be ignored in the Design Rule Checker. Setting a rule to Ignore in the Violation Severity section will completely disable the corresponding design rule check. Use this setting with caution. |
Importing settings
You can import part or all of the board setup from an existing board. This technique can be used to create a “template” board that has the settings you want to use on multiple designs, and then importing these settings from the template board into each new board rather than entering them manually.
To import settings, click the Import Settings from Another Board… button at the bottom of the Board Setup dialog and then choose the kicad_pcb file you want to import from. Select which settings you want to import and the current settings will be overwritten with the values from the chosen board.
