KiCad Library Convention

The KiCad Library Convention (KLC) is a set of requirements for contributing to the official KiCad libraries. Users wishing to submit or update library files should be familiar with these guidelines.

The KLC are a set of guidelines, rather than rules. Electronic component libraries are diverse and complex, and exceptions can be made at the discretion of the library team.

Where the KLC deviates from a particular datasheet or manufacturer recommendation, the datasheet should take preference unless there is a good reason not to do so (which should be clarified by a librarian).

Where the KLC is unclear, users should attempt to match the convention of existing library components, or seek further clarification.

Refer to the contribution guidelines for introductory information on contributing to the KiCad libraries.

KLC Helper Scripts

The KiCad library team has developed a set of Python scripts which can be used to help test if library components conform to the KLC requirements.

When a pull request is made to the libraries, the contributed files are automatically checked using these scripts. It can be helpful to run these scripts on your local machine before submitting a PR, as it will help speed up the process of merging your contribution(s) into the library.

To run the footprint checker script, for instance, cd into the "kicad-library-utils/pcb" directory, then run the Python script ./ path_to_fp1.kicad_mod path_to_fp2.kicad_mod -vv. This will carefully check your footprint according to the KLC requirements laid out below, notifying you of any discrepancies, errors, or violations. See more usage examples in the readme at the link above.

Note: While many of the KLC guidelines are checked by these scripts, there are some which are not covered. Additionally, any PR requires manual checking by a member of the library team.

General Library Guidelines

The general library guidelines apply to all library elements (symbols / footprints / models). However, these guidelines may be overridden in some cases by specific exceptions described in further sections.

G1 - General Guidelines

G1.1 - Only standard characters are used for naming libraries and components

Filenames, symbol names, footprint names and model names must contain only valid characters, as determined below:

  1. Alphanumeric characters (A-Z, a-z, 0-9)

  2. Underscore _

  3. Hyphen / dash -

  4. Period / dot .

  5. Comma ,

  6. Plus symbol +

This character set ensures that symbols will be compatible with all filesystems, and will not cause any issues due to character rendering.

Further, filenames and symbol names must not use the space character. This can cause issues with string escaping and is best avoided.

G1.2 - Each library is limited to 250 items

Libraries with more than 250 items can result in long library loading times. Additionally, such broad categorization of components means that it can be hard to locate a particular component in the libraries.

A library size limit of 250 items ensures that libraries are quick to load and components are easy to locate. If a given library exceeds 250 components, it should be split and further subcategorized according to component functionality.

G1.3 - Libraries are organized by functionality

Rather than grouping components (e.g. symbols, footprints) by their manufacturer, KiCad libraries are organized by component functionality. This grouping strategy has a number of key benefits:

  • Similar components are grouped together, allowing alternative parts to be easily substituted

  • Symbol aliases for pin-identical symbols can be used to reduce library size

  • Generic parts which are produced by multiple manufacturers are supported

Library organization should follow the general form as described below, with each element separated by the underscore (_) character:

  1. Library function

  2. Library sub-function

  3. Tertiary qualifier

  4. Manufacturer name

  5. Component series name

  6. Extra library descriptors

Note: Some of the elements listed above may be omitted if not required.

For specific examples, refer to the guidelines for organizing symbol libraries and footprint libraries.

G1.4 - English language should be used throughout libraries

KiCad software is used by people who speak many different languages. The KiCad software provides translations for these languages, but the library files do not provide translations.

Library files should be written using English, excepting where specific component names are non-English (for non-English manufacturers).

Where potential differences in spelling and grammar exist, American English should be given preference.

  • Color instead of Colour

G1.5 - Plural naming is to be avoided

In general, plural naming (e.g. for libraries) should be avoided, as pluralisation of some words is inconsistent. Non pluralized names should be used in preference:

  • Sensor_Temperature instead of Sensors_Temperature

  • Memory_Flash instead of Memories_Flash

  • TerminalBlock instead of TerminalBlocks

G1.6 - Capitalization conventions

  1. Acronyms should be capitalized

    • MCU (microcontroller)

    • FPGA (field programmable gate array)

  2. Manufacturer names should be capitalized according to the manufacturer

    • Microchip

    • ROHM

    • Texas

    • NEC

  3. Unless separated by delimiters such as _, -, ., words should be separated using CamelCase convention, with the first letter of each word capitalised

    • TestPoint

    • BatteryHolder

G1.7 - Library files use Unix style line endings

Library files must always be commited to GitHub using Unix-style line endings. This means that lines are terminated using the LF (line feed) character, rather than the DOS style CR+LF line endings.

KiCad library files must be compatible across multiple operating systems, and users should be able to contribute without generating unnecessary noise in the files by constantly changing line endings.

When using the KiCad libraries on a Windows PC, the line endings in the library files may be automatically converted to CR+LF. This is fine, as long as any contributions made to the libraries observe the LF line ending requirements.

This issue is addressed by insisting that all KiCad libraries include a .gitattributes file. This file ensures that the line endings are automatically converted by Git.

An example of a simple .gitattributes file which ensures footprint files have correct line endings is as follows:

*.kicad_mod text=auto

Note: The KiCad library repositories should already have the correct .gitattributes file in place to achieve this

G1.8 - Components can only contain features supported in latest stable release

KiCad library components (symbols, footprints) may only contain features that are supported by the latest stable KiCad software release.

Features introduced in nightly builds are not allowed in official KiCad library files.

G1.9 - Dimensional units

  1. When specifying a dimension (e.g. in a footprint name) the units must always be provided:

    • 3mm - millimeters

    • 1in - inches

  2. When specifying multidimensional units (e.g. length x width x height) then the units only need to be appended once

    • 3x4x7mm - 3mm x 4mm x 7mm

  3. Metric units are preferred, where appropriate

  4. Linear dimensions should be specified in millimeters

  5. Angular dimensions should be specified in degrees

  6. Temperature should be specified in degrees Celsius

G2 - Atomic and Generic Parts

G2.1 - Defining generic and atomic parts

In general terms, the symbols in the KiCad library can be categorized into two groups:

Generic symbols

Generic symbols can be used with multiple footprints, and do not have a default footprint assigned. Generic symbols allow flexibility in the design workflow. Symbols are first added to the schematic, and the footprint is selected before PCB layout. Using generic symbols allows a small number of library symbol elements to represent a very large number of possible component combinations.

An example of the use of generic symbols is the Resistor and Capacitor symbols available in the KiCad library. These symbols do not have an assigned default footprint, as there are many possible compatible footprints.

Atomic Parts

Atomic parts fully define a component, specifying a matching footprint, and are named based on the MPN (manufacturer part number). Atomic parts are ready to be placed onto the PCB as they are already associated with a footprint.

Symbol Guidelines

The following guidelines apply to schematic symbols and symbol library files.

S1 - Symbol Libraries

S1.1 - Symbol libraries should be categorized by function

Symbol libraries are individual .lib files, which have a corresponding .dcm file. Both files are required to fully describe the symbols contained in the library. Apart from the file extension, both files must have the same name (case sensitive).

Symbol library names must be defined based on the priority list below, with each element separated by the underscore (_) character:

  1. Function (e.g. Sensor, Amplifier, MCU)

  2. Sub-function (e.g. Temperature, CurrentSense)

  3. Tertiary qualifier (e.g. CMOS)

  4. Manufacturer name (e.g. Atmel, Infineon)

  5. Symbol series name (e.g. PIC24, STM32)

  6. Extra library descriptors (e.g. Deprecated )

Note: Some of the elements listed above may be omitted if not required.

Example symbol library names:

  • Power_Monitor - Power monitoring components

  • Sensor_Temperature - Temperature sensors

  • Driver_Motor - Motor drivers

  • MCU_Microchip_PIC32 - PIC32 microcontrollers from Microchip

S2 - Symbol Naming

S2.1 - General symbol naming guidelines

  1. Library naming should not be duplicated in footprint name

  2. If symbol with same name exists for multiple manufacturers, the manufacturer name is written first

  3. Specific manufacturer name (for atomic parts)

  4. Type of symbol (for generic parts)

    1. May be shortened for common components (e.g. Conn for Connector)

    2. Reference designator may be substituted for common components (e.g. D, C, LED)

  5. Part name should include extension for specific footprint if required (e.g. SOIC)

  6. Any modification of the original symbol, indicated by appending the reason (e.g. different pin ordering - Q_NPN_CBE, Q_NPN_BCE)

  7. Indicate quantity of elements for symbol arrays (e.g. resistor array with 8 elements - Resistor_x8)

  8. Add suffixes for symbol variations

    1. For multi unit variants of typically single unit symbols add the suffix _Split

S2.2 - Non-functional variations in part number should be replaced with wildcard

Manufacturer Part Numbers (MPN) often include variations that are non-functional.


  • Temperature rating of the component

  • Packaging information (e.g. reel, tray, tape)

  • RoHS / PbFree information

To capture every possible combination of part variation requires a large number of symbol aliases - this is to be avoided.

Where an MPN has options for such non-functional variations, these portions of the MPN should be replaced with a wildcard character (x).

Rule of thumb

A single symbol should be drawn for each footprint variation of an atomic part. Other variations (as listed above) do not require their own symbol alias.

S2.3 - Where atomic parts are available in multiple footprint options, a separate symbol must be drawn for each footprint

Many electronic components are provided in multiple footprint (package) options. These may or may not be pin compatible.

e.g. LTC4357

Here there is a requirement for two separate symbols, one corresponding to each available footprint.

The naming of the symbols must match the manufacturer naming convention for the footprint variants. In the image above (taken from the datasheet) the footprints are defined as follows:

  • DCB - 6-lead DFN

  • MS8 - 8-lead MSOP

Thus, two symbols must be drawn:

Where possible, the symbols should be drawn such that they can be swapped in the schematic with minimal disruption to wire connections.

As a further example we shall consider the comparator MCP6566 which is available in three SOT-23-5 versions, each with a different pinout.

In this case, a separate symbol must again be drawn for each version, and named according to the convention called out in the datasheet.

S3 - General Symbol Requirements

S3.1 - Origin is centered on the middle of the symbol

For symmetrical symbols, the symbol must be centered around the origin (0, 0) in the symbol editor.


For non-symmetrical symbols, or symbols where this requirement would move pins off the 100mil grid, then the symbol should be placed as close to the origin as possible while observing the pin grid alignment requirements.

S3.2 - Text fields should use a common text size of 50mils

  1. All text fields (pin name, pin number, value, reference, footprint, datasheet) should use a text size of 50mil.

  2. Pin names and pin numbers can use a text size as small as 20mil if the symbol is small or has special geometry.

S3.3 - Symbol outline and fill requirements

  1. Symbol body must have a line width of 10mil (0.254mm)

  2. Black-box symbols (e.g. ICs with hidden functionality) should be filled with background color

  3. Simple components (e.g. discrete components or those with a distinctive shape) should not be filled with background color

Fill background

Do not fill

S3.4 - Symbols with complex functionality may incorporate simple functional diagrams

For black box symbols with complex functionality (e.g. special function ICs), a simplified diagram of the symbol functionality may be drawn on the symbol. This may be used to provide functional clarity in a schematic.

  1. Functional drawing must remain simple

  2. Do not add functional drawings for multi-function components (e.g. microcontrollers)

S3.5 - Pin connection points must be placed outside of the symbol

Connection points for symbol pins must be placed outside the symbol body and must not require a connecting wire to cross the symbol.

Example of incorrect symbol:

Example of correct symbols:

S3.6 - Pin name position offset

  1. Pin name position offset must not exceed 50mil (1.27mm)

  2. Pin name position offset should not be set less than 20mil (0.508mm)

  3. Preferred value is 20mil

  4. Larger offset allowed to accomodate particular symbol geometry


S3.7 - Pin numbering for specialized pads

For IC components with exposed pads, the number of the exposed pad should start one greater than the pin-count of the footprint.

For a SOIC-8 package with a single exposed pad, the exposed pad will be assigned the number 9

Shielded components use "SH" as the pin number for connecting the shield. For a pin to qualify as the shield pin it must be connected to a metal enclosure. For connectors it must connect to the shield of the cable.

Parts that include mechanical mounting pads without electrical use, get the pin number "MP". Non plated through holes do not get any pad number assigned. (They do not get a pin in the symbol.) An example for such a pure mechanical mounting pad would be the pads for the two metal leads on the side of Molex picoblade smd connectors.

S3.8 - Multi unit symbols

  1. For symbols with multiple units that are drawn separately, where the units share common power pins, a separate unit should be drawn which contains these power pins.

This approach should not be taken for single-unit symbols. Power pins in this case must be drawn on the same symbol as the logic pins.

S4 - Pin Requirements

S4.1 - General pin requirements

  1. Using a 100mil (2.54mm) grid, pin origin must lie on grid node (IEC-60617)

  2. Pins should have a length of at least 100mil (2.54mm)

    • Shorter pins may be allowed to accommodate simple symbols for discrete devices such as resistors, capacitors, etc.

  3. Pin length must not exceed 300mil (7.62mm)

  4. Pin length can be incremented in steps of 50mil (1.27mm) as required, whilst meeting the absolute length limits as specified above

  5. Pin numbers must be unique (no two pins may have the same number)

S4.2 - Pins should be grouped by function

Where possible, pins should be grouped by similar function, rather than by their physical location on the associated footprint. This provides cleaner schematic routing and symbols are easier to understand in the schematic.

  1. Pins with similar functions should be grouped together:



  2. Ports should be ordered from top to bottom

  3. Positive power pins should be placed at the top of a symbol

    • Vcc, Vdd, Vin, V+, etc.

  4. Negative power and ground pins should be placed at the bottom of a symbol

    • GND, Vss, V-, etc.

  5. Input/Control/Logic pins should be placed on the left of a symbol

    • UART Tx/Rx

  6. Output/Controlled/Driver pins should be placed on the right of a symbol

    • RS232 Tx/Rx

S4.3 - Rules for pin stacking

Many symbols have corresponding footprints where multiple physical pins are connected to a single logical net. It is desirable that in such cases the user only has to connect a single pin in the schematic, and it will automatically route to all the physical pins on the PCB. (This is not only done to reduce clutter in the schematic drawing. The main reason is to move some responsibility for correct connections from the circuit designer over to the library.)

KiCad currently has no native method for designating that a particular symbol pin maps to multiple footprint pins. The following guide serves as a workaround for designing such symbols.

In the schematic view, pins that share the same position are considered to be connected by the KiCad routing algorithm. Thus, pins can only be placed in the same location under a very specific set of circumstances:

  1. Pins must not be of type No Connect (these pins should never be connected together)

  2. Power supply pins must be stacked unless the datasheet specifies the need for decoupling capacitors on every pin.

  3. Pins are logically connected in the symbol

  4. Pins must have the same name

  5. Pins must have the same electrical type

  6. One pin in the stack must be visible (all other pins set to invisible)

Special Case: Pins of electrical type [Output, Power Output, Power Input] are special cases. . Connecting Output or Power Output pins would result in an ERC error. Output pins that always need to be connected together must therefore be stacked. The invisible pins get the pin type passive in this case. . Invisible Power Input pins are global labels. This is to be avoided. For this reason the electrical type pasive is to be used for the invisible pins in such stacks.

S4.4 - Pin electrical type

Pin Electrical type should be set to match the appropriate pin function

  1. Power and ground pins should be set to either Power Input or Power Output

  2. Logic pins should be set according to datasheet requirements

  3. Pins with programmable functionality (e.g. MCU I/O ports) should be set to Bidirectional

  4. Pins must not be 'double inverted' by assigning the inverting graphical symbol and also having a bar above the name of the pin

S4.5 - Pins not connected on the footprint may be omitted from the symbol

Often a component has pins that are not physically connected, and in such cases, unconnected pins may be omitted from the schematic symbol.

  1. Pins may only be omitted if they are never to be connected under any circumstances

  2. If pins are designated NC but the datasheet specifies that these must be pulled to ground or otherwise connected to a specific net, then these must be shown on the schematic symbol

  3. If the pin-count in the schematic does not match the pad-count on the footprint, the footprint filter must include the pad-count of the footprint (see also requirements for footprint filters)

    • SOT?23?5

    • SOIC?8

S4.6 - Hidden pins

Hidden connection pins are generally not allowed for schematic symbols. Any connection point must be visible, otherwise unexpected net connections can occur.

Hidden power pins are also not allowed.


  1. Unused NC pins can be set to invisible. In this case the electrical type must be Not Connected. The end of the pin should lie on the symbols outline box to prevent unwanted connections to the invisible pin (see screenshot below).

  2. Invisible pins may be used in a pin stack to allow one-to-many connections. Refer to the requirements for pin stacking

S4.7 - Active low pins should be designated using a bar above the symbol name

Rather than selecting the active low graphical pin style, active low pins should be designated using a bar above the pin name.

This provides a cleaner look for the schematic.

To place a line above the pin text, prefix the name with the tilde (~) character. In case of a pin name where only part of it is active low, and hence, not all of it needs a bar above, two tilde characters must be used as delimitation, e.g. ~SPD_LED~/GPIO2.

If the pin name given by the manufacturer includes an active low prefix or suffix, it should be removed when adding the bar above it to avoid negating it twice. For example for nRESET, use ~RESET.

S5 - Footprint Association

S5.1 - Symbols with a default footprint link to a valid footprint file

  1. For atomic symbols (those with an associated default footprint), the Footprint field must be filled with a valid entry of the format <footprint_library>:<footprint_name>.

  2. For generic symbols (those which map to multiple possible footprints), the Footprint field must be left blank

S5.2 - Footprint filters must match all appropriate footprints. They should be designed to result in no false suggestions.

Footprint filters are used to help match appropriate footprints to a given symbol. This is important even for fully specified symbols (symbols with only one matching footprint), as there still may be multiple compatible footprints with different variants or options (e.g. _HandSoldering, _Heatsink, _ThermalVias).

Footprint filters use wildcard pattern matching, and allow the following wildcards:

  • * - Match zero or many characters

  • ? - Match zero or one characters

The library name can be used as a filter criterium. The delimiter between library and footprint filtering is :

Filter conventions:

  1. Filters must end with a * wildcard to allow matching of modified footprint suffixes

  2. Filters must match the dimensional information (where required) to be as specific as necessary:

    • DIP*W7.62mm* to match DIP-22_W7.62mm but not DIP-22_W9.3mm

    • Neighter the size of the exposed pad nor the size of the mask cutout are included.

  3. Filters must not contain the pin count if the pin-count in the symbol matches the pin count in the footprint. In those cases the footprint is matched by KiCad’s pin count filter. If not all pins are present in the symbol (e.g. NC-pins) the pin-count has to be part of the footprint filter (see requirements for NC pins). Then e.g. SOT?23?5 might be used instead of simply SOT?23* to match SOT-23-5.

    • Special pin specifiers are always included. Meaning the specifier for Exposed pads EP, Mounting pad MP and Shield SH including their count must be included if the symbol uses these pins. (Filter for QFN-16-1EP_3x3mm_P0.5mm_EP1.8x1.8mm would be QFN*1EP*3x3mm*P0.5mm*)

  4. By default, the footprint search does not include the name of the footprint library. To force the library name to be included, add the : (colon) character to the filter. Text appearing before the : will match the library name. Text appearing after the : will match the footprint name.

    • Connector*:*Pitch?1.25mm* will match any footprint with '1.25mm' pitch, only in libraries that begin with the text 'Connector'

Footprint filters can be set in the Footprint Filter tab in the Symbol Properties window.

S6 - Symbol Metadata

S6.1 - Component Reference Designator (RefDes)

The symbol Reference Designator must be filled out appropriately for the particular type of symbol.

The table below provides a list of appropriate RefDes values. If you do not find an appropriate component entry, consult with the KiCad library team.

Designator Component Type
ASub-assembly or plug-in module
FBFerrite bead
HHardware (mounting screws, etc)
JJack, fixed part of a connector pair
JPJumper / link
LInductor, coil, ferrite bead
LSLoudspeaker or buzzer
PPlug, movable part of a connector pair
RNResistor network
TPTest point
UIntegrated circuit (IC)
YCrystal / oscillator
ZZener diode

S6.2 - Component fields must be filled appropriately

  1. Reference field is selected appropriately for the symbol and is visible

  2. Value field contains the name of the symbol and is visible

  3. Footprint field contains footprint link for atomic parts, and is empty for generic parts. It must be invisible

  4. Datasheet field is left empty, and is invisible

  5. The symbol contains no other custom fields

S6.3 - Component metadata is added to symbol (and all aliases)

Component metadata is contained in the <libname>.dcm file, and must be filled in for each unique symbol (and each alias for the symbol).

  1. Description field contains comma-separated device information

    1. For symbols with a default footprint, the simplified footprint name should be appended to the description e.g. SOIC-8

    2. Part name should not be duplicated in the description field

  2. Keywords field contains space-separated keyword values. These values are used to assist in part searching and should not include filler words

  3. Documentation File Name field contains URL to part documentation if applicable, or is otherwise left blank

S7 - Special Symbols

S7.1 - Power flag symbols

Power flag symbols are special symbols in KiCad, used to designate global nets. These symbols use a special RefDes value to indicate that they must be considered as global power flags

  1. Reference Designator must be set to #PWR

  2. Power flag symbols must contain exactly one pin, which is set to invisible

  3. Electrical pin type must be set to Power Input

  4. Pin name must match the symbol name

The example image below demonstrates the requirements as listed above:

S7.2 - Graphical symbols

Graphical symbols are used only to annotate schematics and do not correspond to a footprint on the PCB.

  1. Reference Designator must be set to #SYM and must be invisible

  2. Symbol name must be set to invisible

  3. Graphical symbols must not contain any pins

  4. No pins or footprint association

  5. No footprint filters


Footprint Guidelines

The following guidelines apply to PCB footprints and footprint libraries.

F1 - Footprint Libraries

F1.1 - Footprint libraries are categorized by function

Footprints are grouped into libraries (directories with .pretty extension) based on their primary function. As an extension of this, footprint libraries should be named based on this same functionality.

Library names must be defined based on the priority list below, with each element separated by the underscore (_) character:

  1. Function (e.g. Conn, Capacitor)

  2. Sub-function (e.g. HDMI, USB)

  3. Tertiary qualifier (e.g. RightAngle, SMD)

  4. Manufacturer name (e.g. Texas, Microchip)

  5. Footprint series name (e.g. MicroFit)

  6. Extra library descriptors as required

Note: Some of the elements listed above may be omitted if not required.

Example footprint library names:

  • Conn_USB_SMD - Surface mount USB connectors

  • Conn_Molex_MicroFit - Molex MicroFit series rectangular connectors

  • Capacitor_Tantalum_SMD - Surface mount Tantalum capacitors

F1.2 - Connector footprint libraries

Categorizing connectors by function can prove difficult as many connectors can be used in a wide variety of applications.

Therefore, categorization of connector footprints is given special consideration as detailed below:

  1. Connectors are grouped firstly by their primary function (where such a function exists). Examples of primary function include:

    • Conn_USB

    • Conn_HDMI

    • Conn_Ethernet

  1. When primary function libraries become too large, they can be split by sub-function or by manufacturer

    • Conn_USB_Molex

    • Conn_DSUB_HighDensity

  2. For connectors without a specific function, then connectors are grouped by their mechanical type:

    • Conn_Barrel

    • Conn_DIN

    • Conn_DSUB

    • Conn_PinHeader

    • Conn_PinSocket

    • Conn_Rectangular

  3. Connector libraries can be further split by another qualifier:

    • Conn_PinHeader_2.54mm

    • Conn_PinHeader_1.27mm

  4. Connector libraries can also be split by manufacturer and series, for multi-purpose connectors

    • TerminalBlock_Phoenix_MKDS

    • TerminalBlock_Phoenix_PT

    • TerminalBlock_Wago

    • Conn_JST

    • Conn_Hirose_DF13

F2 - General Footprint Naming Guidelines

F2.1 - General footprint naming conventions

Each footprint is a .kicad_mod file (stored within a .pretty directory). The naming convention for a given footprint depends largely on the type of footprint, however a general guide is presented below:

  1. Specific package type is written first, e.g.

    • QFN - Quad Flat No-Lead package

    • C - Capacitor

  2. Package name and number of pins are separated by a hyphen

    • TO-90

    • QFN-48

    • DIP-20

  3. Packages with special pads add an identifier to the pin count field separated by a hyphen

    • The field includes the count of uniquely numbered pads of this type.

      • For exposed pads (large copper pad below the part) [count]EP

      • For shield pads [count]SH (Unless such a pin is already expected for the part. An example would be a HDMI connector.)

      • For pads connecting pure mechanical mounting leads [count]MP

    • Examples from the library.

      • DFN-6-1EP_2x2mm_P0.5mm_EP0.61x1.42mm

      • Samtec_LSHM-110-xx.x-x-DV-S_2x10-1SH_P0.50mm_Vertical

      • Molex_PicoBlade_53261-0271_1x02-1MP_P1.25mm_Horizontal

  4. Unique fields (parameters) in the footprint name are separated by _ character.

  5. Package dimensions are specified as length x width (and optionally height)

    • 3.5x3.5x0.2mm

    • 1x1in

    • If necessary for clarity, footprint body dimensions may be prefixed with a leading B

  6. Pin layout

    • 1x10

    • 2x15

  7. Pitch is specified with a leading P:

    • P1.27mm - 1.27mm pitch

    • P5.0mm - 5.0mm pitch

  8. Modifiers to standard footprint values

    • Drill1.25mm

    • Pad2.4x5.2mm

  9. Orientation e.g. Horizontal, Vertical

  10. Any modification to the original footprint, indicated by appending the reason

    • _HandSoldering

    • _ThermalVias

    • _CircularHoles

Not all of the fields defined above are strictly required for a particular footprint. Additional fields may also be added as needed.

F2.2 - Footprint naming field prefixes

A footprint name has to convey a lot of information to clearly specify the purpose and parameters of the footprint. Some fields in footprint names are common to many footprints and can be shortened using special abbreviations.

Not all footprints will require the use of these abbreviations - they are provided as a method of standardising the manner in which footprint parameters are called out when encountered.

In many cases, the major dimensions (x/y/z) of a footprint may be specified without a prefix, as the body dimensions are assumed to have the greatest priority in the footprint name. Therefore, the "3.2x5.7mm" part of the example name below requires no 'B' prefix, and is not required to be written as "B3.2x5.7mm".

e.g. SOIC-8_3.2x5.7mm_P1.27mm

In cases where potential conflicts exist, however, the body dimensions must be explicitly named with the prefix B.

Refer to the table below for accepted prefix abbreviations.

Prefix Field Description Notes
BBody dimensions
  • Body size (XxYxZ)
  • Height parameter Z may be omitted
  • Prefix B may be omitted if the body size is the major dimension used to define the footprint
  • Diameter of major axis for cylindrical component
  • e.g. D10mm - 10mm diameter
  • Height of component measured from PCB
  • Body size B should be used in preference, where possible
  • e.g. H1.1 - component measures 1.1mm above PCB
  • Length along major axis of component
  • Body size B should be used in preference, where possible
  • e.g. L15.3mm - 15mm length
  • Width along minor axis of component
  • Body size B should be used in preference, where possible
  • e.g. W4.75mm - 4.75mm width
EPExposed pad dimensions
  • Packages that include a single exposed pad include the size of this pad. e.g. EP2.4x3.6 - for a single 2.4mm x 3.6mm pad.
PPad pitch
  • Pitch (distance) between pins, pads or leads
  • e.g. P0.63mm - 0.63mm pitch between pads
TThicknessComponent thickness, where appropriate


  • LQFP-32_4x4x1.1mm_P1.65mm - LQFP package, 32 pins, 4x4mm body, 1.1mm height, 1.65mm pitch

  • CP_Radial_D4.5mm_P2.5mm_H10mm - Radial polarized capacitor, 4.5mm diameter, 2.5mm pitch, 10mm height

If the parameter is not found in the table above, the name of the parameter should be entered in full.

Following is a list of examples of (non-abbreviated) parameter names used in footprint naming

Prefix Field Description
BallBGA Ball diameter
ClearanceClearance between pin rows
DrillDrill diameter
LayoutSpecific footprint layout
e.g. Layout3x7 for a BGA with 21 balls arranged in 3 columns and 7 rows
LeadLead dimensions
MaskCustom soldermask dimensions
PadCustom pad dimensions
TabTab dimensions

F2.3 - Manufacturer specific version of generic footprints

If a manufacturer footprint deviates from the "standard" footprints available, then this should be added to the library and designated as manufacturer-specific.

  1. If a footprint is specific to a single manufacturer, this must be indicated by prepending the manufacturer name and MPN to the footprint name.

    • Texas_S-PVQFN-N48_

  1. Sometimes the component datasheet will have specific requirements which do not conform to KLC requirements. A common example is specific requirements for the shape of stencil (solder paste layer).

In such cases, the KLC requirements can be superseded by the datasheet requirements, at the discretion of the KiCad library team.

F2.4 - Footprint naming for non-standard pin numbering

Generally, a footprint should include a field of the format <pkg>-<pincount>, e.g.

  • SOIC-8

  • QFN-24

In the majority of cases, the pin quantity is self explanatory and is sufficient to describe the number of pins on the symbol.

However there may be cases where this numbering is insufficient. Where the number of footprint pins does not match the number of package pins, exceptions must be made.

Exception: Omitted pins, missing pin numbers are skipped

Example: LTC3638

The LTC3638 comes in an MSOP-16 package which has four missing pins, for increased voltage isolation.

In this case, the numbers for the missing pins are skipped and the normal pin numbers are assigned to the remaining pins.

To indicate this, the footprint should be named as follows:

PKG-<xx>-<yy> where:

  • xx = number of remaining pins

  • yy = number of remaining pins + number of removed pins

In the LTC3638 example above, this would result in:


The footprint pads should be numbered like so:

F2.5 - Footprint naming conventions for specific components

Footprint naming is sufficiently complex that a general rule is not enough to fully define a naming scheme that fits the wide range of footprints.

In addition to the general footprint naming guidelines defined in KLC 2.1, a set of footprint naming guidelines for specific footprint types is provided in KLC F3.x.

F3 - Specific Footprint Naming Guidelines

F3.1 - SMD chip package naming conventions

The following footprint naming conventions should be used as examples for naming SMD chip package footprints.

If you do not find an appropriate convention that matches a particular footprint type, either contact the KiCad library team or try to match a convention set by existing library components.

In the entries below, variable fields are denoted as follows:

- Fixed fields
- Mandatory fields
- Optional fields

[Prefix]_[Imperial size]_[Metric size]Metric_[Modifiers]_[Options]

  • Prefix - Device type
  • Imperial size - Imperial case size (Optional)
  • Metric size - Metric case size (Optional)
  • Modifiers - Modifiers to footprint if non standard (Optional)
  • Options - Extra footprint options (Optional)




The prefix is determined by the default reference designator of the device, e.g.

  • Capacitor = C

  • Capacitor (polarised) = CP

  • Resistor = R

  • Diode = D

Case size codes:

Imperial Code Metric Code Size Imperial Size Metric



0.0157 in × 0.0079 in

0.4 mm × 0.2 mm



0.024 in × 0.012 in

0.6 mm × 0.3 mm



0.039 in × 0.020 in

1.0 mm × 0.5 mm



0.063 in × 0.031 in

1.6 mm × 0.8 mm



0.079 in × 0.049 in

2.0 mm × 1.25 mm



0.098 in × 0.079 in

2.5 mm × 2.0 mm



0.126 in × 0.063 in

3.2 mm × 1.6 mm



0.126 in × 0.098 in

3.2 mm × 2.5 mm



0.177 in × 0.063 in

4.5 mm × 1.6 mm



0.18 in × 0.13 in

4.5 mm × 3.2 mm



0.18 in × 0.25 in

4.5 mm × 6.4 mm



0.197 in × 0.098 in

5.0 mm × 2.5 mm



0.25 in × 0.13 in

6.3 mm × 3.2 mm



0.29 in × 0.20 in

7.4 mm × 5.1 mm

F3.2 - Resistor naming conventions

The following footprint naming conventions should be used as examples for naming resistor footprints.

If you do not find an appropriate convention that matches a particular footprint type, either contact the KiCad library team or try to match a convention set by existing library components.

In the entries below, variable fields are denoted as follows:

- Fixed fields
- Mandatory fields
- Optional fields

Axial Resistors


  • Length - Resistor body length
  • Diameter - Body diameter
  • Pitch - Lead spacing
  • Modifiers - Modifiers to footprint specifications (Optional)
  • Orientation - Resistor orientation (Vertical / Horizontal) (Optional)
  • Options - Extra footprint options (Optional)



F3.3 - Capacitor naming conventions

The following footprint naming conventions should be used as examples for naming capacitor footprints.

If you do not find an appropriate convention that matches a particular footprint type, either contact the KiCad library team or try to match a convention set by existing library components.

In the entries below, variable fields are denoted as follows:

- Fixed fields
- Mandatory fields
- Optional fields

SMD Chip Capacitor

[C/CP]_[Imperial size]_[Metric size]Metric_[Modifiers]_[Options]

  • C/CP - Capacitor style (polarised or non-polarised)
  • Imperial size - Imperial case size (Optional)
  • Metric size - Metric case size (Optional)
  • Modifiers - Footprint modifiers if non standard (Optional)
  • Options - Footprint options (Optional)




  1. At least one case size (either imperial or metric) must be specified

  2. Metric case size must have the suffix Metric

SMD Tantalum Capacitor

CP_Tantalum_EIA-[Metric size]_[Size code]_[Modifiers]_[Options]

  • Metric size - EIA metric size code
  • Size code - Letter size code including naming standard ([Standard]-[Letter])
  • Modifiers - Footprint modifiers if non standard (Optional)
  • Options - Footprint options (Optional)


EIA Metric size Body size (XxYxZ) Kemet Code AVX Code


1,6 x 0,8 x 0,8 mm



1,6 x 0,85 x 1,05 mm



2,05 x 1,35 x 1,2 mm




2,05 x 1,35 x 1,5 mm



3,2 x 1,6 x 1,0 mm




3,2 x 1,6 x 1,2 mm




3,2 x 1,6 x 1,8 mm




3,5 x 2,8 x 1,2 mm




3,5 x 2,8 x 1,5 mm



3,5 x 2,8 x 2,1 mm




6,0 x 3,2 x 1,5 mm




6,0 x 3,2 x 2,0 mm



6,0 x 3,2 x 2,8 mm




7,3 x 4,3 x 1,5 mm




7,3 x 4,3 x 2,0 mm




7,3 x 4,3 x 3,0 mm



7,3 x 4,3 x 3,1 mm




7,3 x 4,3 x 4,0 mm



7,3 x 4,3 x 4,3 mm




7,3 x 6,0 x 3,8 mm



7,3 x 6,1 x 3,8 mm



7,3 x 6,1 x 4,3 mm


SMD Electrolytic Capacitor


  • Manufacturer - Manufacturer name (Optional)
  • X - Case size in x dimension
  • true - Case size in y dimension
  • [Height] - Case height (Optional)
  • [Pitch] - Lead spacing (Optional)
  • [Modifiers] - Footprint modifiers if non-standard (Optional)
  • [Options] - Footprint options (Optional)



THT Capacitor

[C/CP]_[Style]_L[Case size]_D[Diameter]_W[Width]_P[Pitch]_[Modifiers]_[Options]

  • C/CP - Capacitor polarisation
  • Style - Capacitor case style (see notes below)
  • Case size - Body length (Optional)
  • Diameter - Case diameter (Optional)
  • Width - Body width (Optional)
  • Pitch - Lead spacing
  • Modifiers - Footprint modifiers if non-standard
  • Options - Footprint options (Optional)




  1. There are different capacitor styles available:

    • Axial: Cylindrical body with axial lead attachment.

    • Radial: Cylindrical body, both leads enter at same end.

    • Disc: Disc shaped body (sometimes enclosed), leads enter tangent to the inner disc

    • Rect: Box shaped body (Bottom face in contact with the board)

  2. Body size:

    • For Axial body styles: L[length]_D[diameter]

    • For Radial body style: D[diameter]{_H[height]}

    • For Disc body style: D[diameter]_W[width]{_H[overall height]}

    • For box shaped body styles: [X]x[Y]{x[Z]}

F3.4 - SMD IC package naming conventions

The following footprint naming conventions should be used as examples for naming SMD IC package footprints.

If you do not find an appropriate convention that matches a particular footprint type, either contact the KiCad library team or try to match a convention set by existing library components.

In the entries below, variable fields are denoted as follows:

- Fixed fields
- Mandatory fields
- Optional fields

Gullwing Packages

The format below provides a guide for naming Gullwing IC packages.


  • SOIC

  • SOP

  • QFP

  • J-Lead

[PKG]-[Pin count]-[EP Qty]EP_[X]x[Y]x[Z]_P[Pitch]_[Modifiers]_[Options]

  • PKG - Package name
  • Pin count - Number of (unique) pins
  • EP Qty - Number of exposed pads under the device (if greater than zero) (Optional)
  • X - Major dimension of part on x axis
  • Y - Major dimension of part on y axis
  • Z - Major dimension of part on z axis (Optional)
  • Pitch - Lead pitch
  • Modifiers - Footprint modifiers (Optional)
  • Options - Extra footprint options (Optional)




  1. [PKG] - refers to the name most commonly used in the industry. Generally this implies JEDEC naming but some other standard may be used as required.

  2. [Pin count] - the number of uniquely numbered pads (excluding any exposed pads under the device)

  3. [Modifiers] - may vary for individual IC footprint types. Includes:

    • Clearance

    • Lead size

    • Pad size

    • Exposed pad size

    • Soldermask expansion

No-Lead Packages


  • DFN

  • QFN

  • LCC

[PKG]-[Pincount]-[EP Qty]EP_[X]x[Y]x[Z]_P[Pitch]_[Modifiers]_[Options]

  • PKG - Package name
  • Pincount - Number of (unique) pins
  • EP Qty - Number of exposed pads under the device (if greater than zero) (Optional)
  • X - Major dimension of part on x axis
  • Y - Major dimension of part on y axis
  • Z - Major dimension of part on z axis (Optional)
  • Pitch - Lead pitch
  • Modifiers - Footprint modifiers (Optional)
  • Options - Extra footprint options (Optional)




  1. The lead length is the nominal lead length for which the footprint is designed

  2. Optionally the nominal lead width can also be provided

Ball Grid Array Packages

[PKG]-[Pincount]_[X]x[Y]x[Z]_Layout[Columns]x[Rows]_P[Pitch X]x[Pitch Y]_Ball[Ball]_Pad[Pad]_[NSMD/SMD]_[Modifiers]_[Options]

  • PKG - Package name
  • Pincount - Number of (unique) pins
  • X - Major dimension of part on x axis
  • Y - Major dimension of part on y axis
  • Z - Major dimension of part on z axis (Optional)
  • Columns - Number of ball columns
  • Rows - Number of ball rows
  • Pitch X - Ball pitch in x direction
  • Pitch Y - Ball pitch in y direction (if different from x direction (Optional)
  • Ball - Ball diameter
  • Pad - Pad diameter
  • NSMD/SMD - Solder Mask Defined or Non Solder Mask Defined
  • Modifiers - Footprint modifiers (Optional)
  • Options - Extra footprint options (Optional)




  1. For BGA simply providing the pin count is not sufficient. It is also necessary to provide the number of [Columns] (x direction) and [Rows] (y direction).

  2. Some BGA packages have different pitch in x and y directions. If this is the case then both [Pitch] dimensions need to be provided

  3. The [Ball] diameter for which the footprint is designed needs to be provided

  4. [NSMD/SMD]

    • NSMD means the footprint is designed for non solder mask defined (mask cutout is larger than copper pad)

    • SMD means the footprint is designed for solder mask defined (mask cutout is smaller than copper pad)

F3.5 - THT IC package naming conventions

The following footprint naming conventions should be used as examples for naming THT IC package footprints.

If you do not find an appropriate convention that matches a particular footprint type, either contact the KiCad library team or try to match a convention set by existing library components.

In the entries below, variable fields are denoted as follows:

- Fixed fields
- Mandatory fields
- Optional fields

Through Hole Packages (DIP)

[PKG]-[Pincount]_[X]x[Y]x[Z]_W[Lead span]_P[Pitch]_[Modifiers]_[Options]

  • PKG - Package name
  • Pincount - Number of (unique) pins
  • X - Major dimension of part on x axis
  • Y - Major dimension of part on y axis
  • Z - Major dimension of part on z axis (Optional)
  • Lead span - Distance between leads
  • Pitch - Lead pitch
  • Modifiers - Modifiers to footprint specifications
  • Options - Extra footprint options (Optional)




  1. Drill size (if specified) must be given in mm

Through Hole Packages (TO)

[PKG]-[Pincount]_[X]x[Y]x[Z]_W[Lead span]_P[Pitch x]x[Pitch y]_[Stagger]_[Modifiers]_[Orientation]_[Options]

  • PKG - Package name
  • Pincount - Number of (unique) pins
  • X - Major dimension of part on x axis (Optional)
  • Y - Major dimension of part on y axis (Optional)
  • Z - Major dimension of part on z axis (Optional)
  • Lead span - Distance between leads (Optional)
  • Pitch x - Lead pitch in x dimension (Optional)
  • Pitch y - Lead pitch in y dimension (if different from x dimension) (Optional)
  • Stagger - Pin staggering options (Optional)
  • Modifiers - Modifiers to footprint specifications (Optional)
  • Orientation - Component orientation (see notes below)
  • Options - Extra footprint options (Optional)




  1. Drill size (if specified) must be given in mm

  2. Orientation can be chosen from:

    • Vertical

    • TabDown

    • TabUp

  3. Stagger can be chosen from:

    • StaggerOdd (odd pins are further from component body)

    • StaggerEven (even pins are further from component body)

Size Parameter:


F3.6 - Connector naming conventions

The following footprint naming conventions should be used as examples for naming connector footprints.

If you do not find an appropriate convention that matches a particular footprint type, either contact the KiCad library team or try to match a convention set by existing library components.

In the entries below, variable fields are denoted as follows:

- Fixed fields
- Mandatory fields
- Optional fields

Conventions for Connectors

Connector footprints are extremely diverse and the naming conventions for connectors can be complicated. This section details some examples of naming schemes for various connector types. While there are variations between connectors, the general format for naming connectors is as follows:

[Series]_[Subseries]-[Pins]_[MPN]_[Pin layout]_P[Pitch]_[Modifiers]_[Orientation]_[Options]

  • Series - Generic series name (Optional)
  • Subseries - Series secondary identifier (Optional)
  • Pins - Pin count (Optional)
  • MPN - Manufacturer specific identifier (Optional)
  • Pin layout - Pin configuration, specific to connector type (Optional)
  • Pitch - Pin pitch, if not implied by connector standard (Optional)
  • Modifiers - Modifiers to connector specifications (pad size, etc) (Optional)
  • Orientation - Orientation of connector relative to board (Optional)
  • Options - Extra footprint options (Optional)


  1. [Series] - a versatile field which could contain:

    • Functional description (e.g. USB)

    • Connector type (e.g. PinHeader or TerminalBlock)

    • Industry standard (e.g. DSUB-15)

    • Manufacturer specific series (e.g. Hirose_DF13)

  2. [MPN] (manufacturer part number) - uniquely identifies a connector according to that manufacturer’s internal naming conventions

  3. [Pin layout] - dependent on the connector type

    • Single row connectors: 1x[number of pins]

    • Multi row connectors with equal number of pins in each row: [number of rows]x[number of pins per row]

    • Other connectors: [number of rows]Rows_[number of pins overall]Pins

    • Connectors for standardized interfaces do not need to include the pin configuration information (e.g. USB)

  4. Number format:

    • [number of rows] number of rows no leading zero.

    • [number of pins per row] and [number of pins] two digit number with leading zero. (can have more digits for connectors with > 99 pins)

  5. [Pitch] - if the connector standard does not imply the pin pitch, then this field is required

  6. [Modifiers] - multiple fields may be added here, detailing modifications or devations from the standard footprint design. Examples include:

    • Pad size variation

    • Drill size variation

  7. [Orientation] - The orientation of the connector with reference to the board plane

  1. [Options] - Extra footprint options

In addition to these conventions, additional schemes are employed for specific connector types - these are detailed below.

Connectors for Specific Functions

Many connectors are designed for specific functions (e.g. USB, HDMI, SD-Card, etc). In these cases, specific naming conventions should be followed:


  • Function - Functional purpose of the connector
  • Standard - Standard to which the connector complies, if applicable (Optional)
  • Size - Connector size (e.g. Micro/Mini) (Optional)
  • Type - Connector sub-type (e.g. A/B/C) (Optional)
  • MAN - Manufacturer name (Optional)
  • MPN - Manufacturer part number (Optional)
  • Modifiers - Footprint modifiers (Optional)
  • Orientation - Connector orientation (Optional)
  • Options - Extra footprint options (Optional)




  1. Some examples of functional connector naming are provided below:

    • USB_Micro-B_Wuerth_614105150721_Vertical_CircularHoles

    • HDMI_Micro-D_Molex_46765-2x0x

    • MicroSD_Wuerth_WR-CRD_693072010801

  2. In most cases, pin layout does not need to be explicitly specified

Connectors with Standardised Shape

Many connectors are provided by multiple manufacturers in an industry standard package or physical layout. These connectors should use the accepted industry naming at the beginning of the footprint name:

[Standard]-[Pins]_[Series modifier]_[MAN]_[Series]_[MPN]_[Pin layout]_P[Pitch]_[Modifiers]_[Orientation]_[Options]

  • Standard - Generic connector standard (see notes below)
  • Pins - Number of pins
  • Series modifier - Series Modifier (see notes below)
  • MAN - Manufacturer name (Optional)
  • Series - Manufacturer series name (Optional)
  • MPN - Manufacturer part number (Optional)
  • Pin layout - Pin configuration, if not fully defined by applicable standard (Optional)
  • Pitch - Pin pitch, if not fully defined by applicable standard (Optional)
  • Modifiers - Footprint modifier field(s) (Optional)
  • Orientation - Connector orientation (if multiple options exist) (Optional)
  • Options - Extra footprint options (Optional)




  1. The generic connector type [Standard] defines the shape of the connector

    • e.g. DSUB Tab Circular

Generic Connector Types

Examples of generic arrayed connectors:

  • PinHeader

  • PinSocket

  • TerminalBlock

[Connector type]_[MPN]_[Pin layout]_P[Pitch]_[Modifiers]_[Orientation]_[Options]

  • Connector type - Generic connector style (see notes below)
  • MPN - Manufacturer specific identifier (Optional)
  • Pin layout - Pin configuration layout (see notes below)
  • Pitch - Pin pitch
  • Modifiers - Modifiers to connector specifications (pad size, etc) (Optional)
  • Orientation - Orientation of connector relative to board
  • Options - Extra footprint options (Optional)



Manufacturer Specific Connectors

Manufacturer series connectors are those which are particular to a particular manufacturer standard.

[MAN]_[Series]_[MPN]_[Pin layout]_P[Pitch]_[Modifiers]_[Orientation]_[Options]

  • MAN - Manufacturer name (Optional)
  • Series - Manufacturer series name
  • MPN - Manufacturer part number
  • Pin layout - Pin layout information (see notes below)
  • Pitch - Pad pitch
  • Modifiers - Modifiers to connector specifications (pad size, etc)
  • Orientation - Direction of connector insertion relative to board plane
  • Options - Extra footprint options (Optional)




  1. If the footprint is located in a library dedicated to a single manufacturer, then the MAN prefix is not required

F3.7 - Fuse naming conventions

The following footprint naming conventions should be used as examples for naming fuse and fuse holder footprints.

If you do not find an appropriate convention that matches a particular footprint type, either contact the KiCad library team or try to match a convention set by existing library components.

In the entries below, variable fields are denoted as follows:

- Fixed fields
- Mandatory fields
- Optional fields

Fuse Holders

FuseHolder_[Fuse Type]_[MAN]_[Series]_[MPN]_[Modifiers]_[Orientation]_[Options]

  • Fuse Type - Type of fuse (Optional)
  • MAN - Manufacturer name (Optional)
  • Series - Manufacturer series name (Optional)
  • MPN - Manufacturer part number (Optional)
  • Modifiers - Footprint modifiers if non-standard (Optional)
  • Orientation - Orientation of fuse, if multiple orientations are available (Optional)
  • Options - Extra footprint options (Optional)



Examples of Fuse Type field:

  • Automotive fuses:

    • Automotive-Micro2

    • Automotive-Micro3

    • Automotive-LowProfile

    • Automotive-Mini

    • Automotive-ATO

    • Automotive-Maxi

    • Automotive-Bosch

    • Automotive-SFE-[SizeCode]

  • Industrial fuses

    • Cylinder-[diameter]x[length]mm


Cylindrical Fuse

Fuse_[MAN]_[Series]_[MPN]_[Body size]_[Modifiers]_[Orientation]_[Options]

  • MAN - Manufacturer name (Optional)
  • Series - Manufacturer series name (Optional)
  • MPN - Manufacturer part number (Optional)
  • Body size - Major fuse dimensions
  • Modifiers - Footprint modifiers if non standard (Optional)
  • Orientation - Orientation of fuse, if multiple orientations are available (Optional)
  • Options - Extra footprint options (Optional)



Rectangular SMD Fuses

Fuse_[Imperial size]_[Metric size]Metric_[Modifiers]_[Orientation]_[Options]

  • Imperial size - Imperial case size (Optional)
  • Metric size - Metric case size (Optional)
  • Modifiers - Footprint modifiers if non standard (Optional)
  • Orientation - Orientation with respect to board plane (Optional)
  • Options - Footprint options (Optional)



F4 - General Footprint Requirements

F4.1 - Datasheet recommendations take priority

Where conflict exists between datasheet recommendations and KLC requirements, then (in the general case) the datasheet should take priority.

It is important when designing footprints that they adhere to requirements for soldering and assembly - often these requirements have very small tolerance for variation.

If the KLC is at odds with the datasheet, follow the datasheet, and note this difference to the KiCad library team when submitting your contribution.

F4.2 - Pin 1 should be located at the top left

Footprints should be oriented such that Pin 1 is located in the upper left corner (IPC-7351).


Where footprints cannot be oriented with pin 1 in the top-left quadrant, pin 1 should be aligned to the top

Two terminal footprints should be aligned with pin 1 on the left side

F4.3 - Connected copper elements have the same pad number

Footprints that contain multiple pads or conductive elements that are physically connected require special attention:

  1. Multiple pads that are physically connected must share the same number

  2. Thermal vias (if present) must share the same number as the thermal pad to which they are connected

F4.4 - Thermal pads

Manufacturer datasheets may specify that thermal vias should be added to the thermal pad under a device package, to assist in moving heat away from the device.

In such cases the datasheet will usually specify the quantity, size and position of these vias.

In addition to manufacturer requirements, a number of extra conventions should be followed when creating thermal vias.

  1. Thermal vias must share the same pad number as the pad on which they are placed

  2. Where thermal vias are connected to a pad on the F.Cu layer, a copper pad on the B.Cu layer should be added, to provide thermal relief for the via. This pad must be large enough to fully surround the via(s) with a margin of >= 0.5mm. Note: If the datasheet gives conflicting advice to the placement of this pad on the B.Cu layer, then the datasheet instruction should be given preference.

  1. Unless instructed by the datasheet, solder paste must not be placed over the thermal via(s). This can cause solder to wick into the via during reflow, and cause solder joint issues.

  2. When submitting a footprint with thermal vias, the suffix _ThermalVias should be added to the footprint name

  3. If it does not already exist, a second version of the footprint without the thermal vias should be added. Note: This second version should not have the _ThermalVias suffix in the footprint name.

F4.5 - Specifying footprint keepout areas

KiCad does not yet have a method for drawing keepout areas inside footprint files. Until this feature is implemented, footprint keepout must should be indicated using the following procedure:

  1. Keepout area shape should be drawn on the Dwgs.User layer

  2. Area should be hatched diagonally

  3. Descriptive text may be included on the Cmts.User layer. This text is used to provide further information about keepout requirements to the user.


F4.6 - Local clearance and settings should be set to zero

Pad clearance values are determined using a priority system, which checks the following locations for clearance values, in descending order of priority. If a particular setting reads as zero (0) then it is ignored, and the next location is checked.

  1. Local pad settings - If an individual pad specifies clearance values, these are used

  2. Footprint settings - If clearance values are specified in the Footprint Properties window, these are used

  3. Global settings - If no values are specified as above, then the global values (as specified in PCB settings dialog) are used.

Unless there is a specific reason for setting explicit values for local clearance values for pads or pins, they should be left at zero (0).


If the component datasheet calls for specific clearance values for a particular pad (or the entire footprint) then these values should be used as appropriate.

F5 - Layer Requirements

F5.1 - Silkscreen layer requirements

The silkscreen is printed to the external surface of a PCB to aid in component identification and orientation. Typically this layer contains the component RefDes to locate components on the board after assembly.

KiCad refers to the silkscreen layers as:

  • F.SilkS - Front silkscreen layer

  • B.SilkS - Back silkscreen layer

The following elements must be provided on the silkscreen.

  1. Reference Designator must be drawn on F.SilkS layer

    1. Text size = 1.00mm

    2. Text thickness = 0.15mm

  2. Silkscreen must not be placed over pads or areas of exposed copper

    • Clearance between silkscreen and exposed copper elements must be at least 0.2mm or more than the pad mask expansion (whichever is greater).

  3. For SMD footprints, silkscreen must be fully visible after boards assembly (no silkscreen allowed under component)

  4. For THT components, silkscreen may be placed under component to aid in assembly process

  5. Silkscreen line width is between {0.10mm and 0.15mm} as per IPC-7351C:

    • Silkscreen line width should nominally be 0.12mm

    • 0.1mm is allowed for high density designs

    • 0.15mm is allowed for low density designs

  6. Pin-1 designator is provided on the F.SilkS layer

  7. Pin-1 designator must be visible after board assembly

F5.2 - Fabrication layer requirements

The fabrication layers are used to display the simplified mechanical outline of components on the PCB.

KiCad refers to the fabrication layers as:

  • F.Fab - Front fabrication layer

  • B.Fab - Back fabrication layer

The following elements must be provided on the fabrication layer(s)

  1. Simplified component outline must be provided on F.Fab layer

    1. Outline uses line width between {0.10mm and 0.15mm} (recommended 0.10mm)

    2. Outline should be simplified and not display complex features

  2. Footprint polarisation / location of pin-1 is drawn

    1. For IC packages, bevel is drawn at corner next to pin-1

    2. Bevel should be 1mm or 25% of package size (whichever is smaller)

    3. For connectors, a small arrow indicator drawn next to pin-1 should be used

  3. Component value (footprint name) must be displayed on the F.Fab layer

    1. Recommended text size = 1.0mm

    2. Allowable text size = {0.5mm to 1.0mm}

    3. Text thickness should be approximately 15% of text size ( with allowances for variation for aesthetic reasons)

    4. Placed below (positive y direction) the part outline.

  4. A second copy of the reference designator (RefDes) must be provided on the F.Fab layer. To add a second RefDes item, add a text object with the value %R

    1. RefDes must be centered on component body (inside component outline)

    2. Orientation of RefDes should match major component axis

    3. Size of text should be scaled to match component size

      1. It is recommended to scale it such that 4 characters fit without overlapping other features of the same layer.

      2. If it is not possible to fit at least 3 characters with the text size restrictions, then the reference should be moved outside (but scaled to smallest allowable text size)

    4. Recommended text size = 1.00mm

    5. Allowable text size = {0.5mm to 1.0mm}

    6. Text thickness should be approximately 15% of text size (with allowances for variation for aesthetic reasons)

F5.3 - Courtyard layer requirements

The component courtyard is defined as the smallest rectangular area that provides a minimum electrical and mechanical clearance around the combined component body and land pattern boundaries. It is allowed to create a contoured courtyard area using a polygon instead of a simple rectangle. (IPC-7351C)

The courtyard should include any extra required clearance for mating connectors (for example).

KiCad refers to the courtyard layers as:

  • F.CrtYd - Front courtyard layer

  • B.CrtYd - Back courtyard layer

A fully enclosed Component courtyard must be drawn on the F.CrtYd layer, with the following parameters:

  1. Courtyard uses 0.05mm line width

  2. All courtyard line elements are placed on a 0.01mm grid

  3. If the component requires a courtyard on the back of the PCB, a corresponding courtyard must be provided on the B.CrtYd layer.

Courtyard clearance should adhere to the following requirements:

  1. Unless otherwise specified, clearance is 0.25mm

  2. Components smaller than 0603 should have a clearance of 0.15mm

  3. Connectors should have a clearance of 0.5mm, in addition to the clearance required for mating of connector

  4. Canned capacitors should have a clearance of 0.5mm

  5. Crystals should have a clearance of 0.5mm

  6. BGA devices should have a clearance of 1.0mm

Example for courtyard clearance when applied to the contoured courtyard outline of a QFP-64 package. (Shown are courtyard, fab-outline and copper pads.)

F6 - Surface Mount Components

F6.1 - Footprint placement type must be set to surface mount

The Footprint placement type must be set to Surface mount for SMD footprints. This is to ensure that these footprints are included in the Footprint position (.pos) file output.

To set the footprint placement type, open the Footprint properties window and select Surface Mount as indicated.

In KiCad 4.x, Placement type is called Attributes and Surface mount is called Normal+Insert.

F6.2 - Footprint anchor should be placed in the middle of the component body

The footprint anchor (also called component origin) is used by automated Pick and Place (PNP) machines for locating and placing SMD components on a PCB.

For most standard components, the anchor should generally be located on the centroid of the component body.

In the KiCad footprint editor, the footprint anchor is always located at the origin (0, 0). To move the footprint relative to the anchor (origin), press the Place footprint reference anchor button (refer to image below).


Some footprints (especially those which are non-symmetrical) require special consideration and the anchor may not necessarily be placed on the component centroid.

Generally speaking, the correct location of the footprint anchor can be found in the component datasheet. The image below shows an example for a Molex Pico-Lock connector.

F6.3 - Pad requirements for SMD footprints

Surface mount pads have specific requirements for PCB design.

  1. By default, pads for SMD footprints should use only the following layers

    1. F.Cu - Front copper

    2. F.Mask - Front soldermask

    3. F.Paste - Front solderpaste (stencil openings)

  2. If SMD pads are placed on the back of the PCB, then the following layers should be used:

    1. B.Cu - Back copper

    2. B.Mask - Back soldermask

    3. B.Paste - Back solderpaste (stencil openings)

  3. Pads with specific stencil aperture design requirements require special attention (see details below)

Requirements for solderpaste

Many components (IC packages in particular) have specific design requirements for solderpaste (stencil) design. These requirements are often found in the footprint datasheet or an associated technical document.

Most often, custom stencil openings are required for the exposed pads on large IC packages to reduce the amount of solderpaste that is applied during stencil application.

The image below shows an example stencil design found in a footprint datasheet. The superimposed blue square represents the shape of the exposed copper pad. The green squares are the required openings in the stencil.

Custom stencil openings are accommodated as follows:

  1. Construct copper shape with pad(s) with only copper layers (F.Cu and/or B.Cu) as appropriate. These copper pads should not have the F.Paste or B.Paste layers checked.

  2. Add stencil opening(s) with pad(s) which only use solderpaste layers (F.Paste and/or B.Paste) as required. These pads do not have a pad number.

  3. The solderpaste should cover between 50% and 80% of the soldermask free pad area. (recommendation: 65%)

Result: (note: this footprint does not correspond to the example shown above)

Size of exposed pads

The following rules apply for finding the correct pad size for parts including an exposed pad.

  1. By default the nominal size of the package pad is used.

  2. Variation within the tolerance ranges of said package pad are allowed if the manufacturers suggested footprint suggest it that way.

    1. It is not allowed to use a footprint pad smaller than the minimum size of the package pad.

    2. Soldermask defined pas are to be used if the suggested footprint uses a pad larger than the maximum size of the package pad. (Meaning: copper can cover a larger area, but the exposed copper is still within the package pads tolerance range.)

Clearance requirement between exposed pads and normal pads

  1. There should be clearance of at least 0.2mm between the exposed pad and the normal pads.

  2. This clearance applies only to the area free of soldermask. (The clearance for soldermask defined pads is the spacing between the normal pads and the soldermask cutout of the exposed pad.)

  3. The heel fillet of the normal pads is to be decreased if necessary to achieve this clearance.

F7 - Through Hole Components

F7.1 - Footprint placement type must be set to Through Hole

The footprint placement type must be set to Through Hole for THT footprints. This ensures that these footprints are not included in the Pick and Place (PNP) location files.

This can be selected in the Footprint Properties window

In KiCad 4.x, Placement type is called Attributes and Through hole is called Normal.

F7.2 - Footprint anchor should placed at the location of Pin-1

For through hole components the footprint anchor should be placed at the location of pin 1.

F7.3 - Pin 1 should be rectangular or a rounded rectangle. Other pads circular or oval

Through hole components should set the shape of Pin 1 to Rectangular or Rounded Rectangle, and all other pads to either Circular or Oval. This aids in orienting the component during placement and also for locating Pin 1 for circuit troubleshooting. For rounded rectangle pads the corner size should be 25% with a maximum radius of 0.25mm.

Pad shape can be adjusted in the Pad Properties dialog:


Non polarized parts (such as THT resistors) should not set the shape of Pin 1 to Rectangular. For these (non polarized) footprints, all pad shapes should be consistent.

F7.4 - Pad requirements for THT footprints

Through hole pads must have soldermask pulled back to allow soldering. However they must not have solderpaste openings as they do not receive solder paste during stencil screening.

  1. Pads for THT footprints must have the following layers set:

    1. All copper layers

    2. F.Mask (front mask)

    3. B.Mask (back mask)

  2. Pads must not have the silkscreen layers active

F7.5 - Minimum annular ring width

For drilled through-holes, the minimum annular ring width must be at least 0.15mm (IPC-2221).

The annular ring is the copper pad which remains after the hole has been drilled.

F7.6 - Minimum hole diameter

For drilled through-holes, minimum drilled hole diameter is the maximum lead diameter plus 0.2mm (IPC-2222 class 2)

Maximum lead diameter is obtained from the device datasheet.

F7.7 - Oval holes (Plated Milled Slots)

The sizes for oval holes must be chosen such that there is 0.2mm clearance between the maximum lead size and the hole in all directions. Oval holes are only allowed if the lead length to width ratio is greater than 2. (Lead cross section is at least twice as long as wide)

Maximum lead dimensions are obtained from the device datasheet.

Some PCB manufacturers are not able to produce milled slots. It is allowed to add an alternative footprint using only circular holes. These need to follow the same drill size increase as all other holes. The equivalent lead diameter should be rounded up to the next 0.01mm increment.

The footprint name of such an alternative is marked with the suffix _CircularHoles.

F8 - Virtual Components

F8.1 - Virtual components

Virtual components are those which have a footprint on the PCB (and may additionally have a schematic symbol) but do not have an associated physical component which needs to be loaded onto the board during assembly.

Examples of virtual components include:

  • Mounting holes

  • Solder bridges

  • Net ties

  • Test points

  • Fiducial markings

Virtual components must be indicated by setting the Placement type to Virtual in the Footprint Properties dialog.

F9 - Footprint Properties

F9.1 - Footprint meta-data is filled in as appropriate

  1. Documentation field contains comma-separated device information. Where appropriate, a URL to the footprint datasheet should be included.

  2. Keywords field contains space-separated keyword values

  3. Ref field must be set to REF**

  4. Value field must match footprint filename (ignoring the .kicad_mod extension)

F9.2 - Footprint properties are as default values unless otherwise required in datasheet

Footprint properties should be left as default, unless there is a reason to do so as specified by the footprint datasheet (for example).

  1. Move and Place must be set to Free

  2. Auto Place should be set to 0, 0

  3. Local Clearance Values should all be set to 0


The Local Clearance Values parameters are generally set to 0, indicating that the global clearance values will be used to determine pad clearances.

If all the pads on the particular footprint require a specific clearance value (for e.g. as described by the datasheet) then these values can be used here to override pad-specific settings for the entire footprint.

F9.3 - Footprint 3D model requirements

  1. All non-virtual footprints must have 3D model references, even if the 3D model is missing (does not yet exist). This allows the 3D model to be added later without requiring the footprint to be edited again. (It is not required to supply a 3d model file.)

  2. 3D model files must be placed in a library (directory) which has the same name as the footprint library, with the extension .3dshapes

    • Capacitor_SMD.prettyCapacitor_SMD.3dshapes

    • Connector_USB.prettyConnector_USB.3dshapes

  3. 3D model files should be named the same as the footprint (ignoring file extension)

    • SOIC-8.kicad_modSOIC-8.wrl

    • R0805.kicad_modR0805.wrl

  4. If a footprint is a simple variation that does not change the 3D representation, the common 3D model should be used (do not duplicate models unnecessarily)

    • R0805_HandSoldering.kicad_modR0805.wrl

    • QFN-48_ThermalVias.kicad_modQFN-48.wrl

  5. Model scaling must be 1:1:1 (model file should not require any scaling to correctly fit the footprint)

  6. Rotation and offset must be 0 (The model must be aligned correctly to the footprint within the 3d modeling software.)

  7. Path to 3D model must have ${KISYS3DMOD}/ prefix

  8. Filetype must be .wrl (KiCad replaces it with .step automatically for the step export.)

3D Model Guidelines

The following guidelines apply to contribution of 3D model data.

M1 - Contributing Models

M1.1 - Models should be created by contributor

Users should only submit models they have created themselves, either manually designed or via parametric scripting tools.

Contributing model data designed by a third party complicates licensing issues and should be avoided.

M1.2 - Manufacturer models should not be duplicated

If a manufacturer provides 3D model data for download from its website, these models should not be duplicated in the KiCad library.

A link to the manufacturer model files may be added to the file within the 3D model directory.


If 3D model data provided by a manufacturer is of low quality or not available for public download, then these data may be added if the following criteria are met:

  • The contributor is the creator of the model data

  • The contributed files provide some advantage over the data supplied by the manufacturer

M1.3 - Source files for 3D models should be supplied

The KiCad library maintains a repository for 3D source files at

The source files used to generate 3D model data should be submitted to this repository when a user contributes 3D model data.

Source files include file generator scripts, or native model files from source software (e.g. FreeCAD).

The source repository directory structure mirrors that of the kicad-packages-3d repository.

M2 - 3D File Requirements

M2.1 - Permitted 3D model file types

The KiCad 3D model library supports two file formats:


  • WRL files contain material properties and are used for realistic rendering. However they cannot be exported to MCAD packages.

  • KiCad v4.x and lower can only render WRL files


  • STEP files are used for integration with MCAD software packages. These files do not contain material properties and cannot be used for realistic rendering.

  • KiCad v5.x and above can render STEP files directly in the 3D viewer

Only models provided in these file formats will be accepted.

It is suggested that a .WRL and .STEP version of the model are provided simultaneously. This provides options for both high quality rendering and MCAD integration.

M2.2 - Model alignment and scaling

The 3D models must be aligned and scaled appropriately to match the associated footprint.


The 3D model must be aligned such that it does not require an additional alignment offset in the footprint options. When associating a 3D model with a footprint, the offset parameter must read (0, 0, 0)


  1. STEP files include absolute dimensional information, and should never have a secondary scaling factor applied. The model scaling parameter in KiCad must read (1, 1, 1)

  2. WRL files do not specify absolute dimensions. KiCad normalizes model parameters to units of inches and the internal units (dimensionless) of the WRL model must be scaled accordingly.


The model should be rotated such that no additional rotation is required within KiCad to align the 3D model with the footprint.

KLC Revision History

Revision information for the KLC can be found here.