-
Notifications
You must be signed in to change notification settings - Fork 26
Conventions
Where possible footprints in the Freetronics Kicad library follow the following conventions:
Freetronics does not print designator labels or values on our PCB silkscreens, we produce a separate image showing what components are located where. Therefore these footprints are not set up for printing labels on silkscreen. However each footprint can be easily modified for this use.
Reference text (usually the name of the footprint in the PCB editor, that becomes a name designator label on the board - ie C22) should be visible on the Eco1.User layer. The reference may overlap pads or other features if necessary. Text thickness must be at least 0.1mm, recommended text size 0.6mm x 0.6mm or larger.
The exception is footprints where a name is likely to be printed on the board for the user to see (for example solder jumpers like SJ2). In these instances the Reference text goes on the Front.Silks layer.
Value text (usually the placeholder val** in the PCB editor, that becomes the component value on the board) should be Invisible on the Eco1.User layer. The value should be placed in such a way that it could be switched to the SilkScreen layer and made visible, without needing to be moved. Text thickness should be at least 0.1mm, minimum text size 0.5mm x 0.5mm.
Value text may be left visible on Eco1.User in cases where the footprint area is very large, and the text can fit wholly under the component.
Footprint outlines are not well handled at the moment. Currently outlines are sometimes on Cmts.User, sometimes on Dwgs.User and sometimes on the silkscreen. Sometimes the outline is the component and sometimes it is the "Courtyard" (area to be left clear around the component for assembly).
Eventually this should be cleaned up as follows:
- Use KiCad's new ".Crtyrd" layers for "courtyard" clearance around the component (ie space that needs to be left free for assembly).
- Markings on silkscreen should indicate outlines or corners of component where necessary.
Use a small dot on the silkscreen to indicate pin 1. The dot should be visible even after the component is placed, for easier troubleshooting/testing.
Diodes have pins numbered "A" for Anode and "K" for Cathode instead of 1 & 2. This convention is used in any schematic symbols whose names start with DIODE or LED and in any footprints with DIODE or LED in the name. In some cases there may be a standard footprint numbered 1 & 2 and a DIODE version with the A & K numbering.
FETs have pins numbered "G","D","S" for Gate, Drain & Source. Footprints for FETs have the suffix _FET to indicate they use this convention. In some cases there may be a standard numbered footprint and a FET version.
Like FETs, BJT transistors (NPN/PNP) have pins numbered "B","C","E" for Base, Collector & Emitter.
Package names should indicate at least one key body dimension as well as pin count, ie
SO16_4mm indicates a SOIC 16 pin package with 4mm wide body.
For packages where it is possible for there to be multiple pin pitches, the pin pitch should also be appended to the name - ie QFP32_5mm_0.5mm indicates a 32 pin QFN, 5mm x 5mm body size, with 0.5mm pin pitch.
The suffix _EP indicates an exposed pad in addition to the numbered pins (this pad is named PAD by convention, and not counted towards the pin count provided in the name).