Origin/anchor on part centre
Pad 1 on the left and then at the top
Ensure rotational symmetry for symmetric parts
Text has size 1mm x 1mm and thickness 0.15mm (checked automatically)
Aim to conform to IPC-7351B footprint design
Reference and Value fields:
- On the F.Fab layer (checked automatically)
- May only be hidden for non-functional parts such as mounting holes
- Place just outside the part courtyard, without overlapping the part
- If the part is usually arrayed vertically, place on left and right, with text running vertically
- If the part is usually arrayed horizontally, place on top and bottom, with text horizontal
- Otherwise, prefer top and bottom
- Reference on top or left, value on bottom or right
Fabrication Layer:
- Include reasonably accurate part drawing
Courtyard:
- Lines 0.01mm thick on 0.05mm grid (checked automatically)
- Clearance:
  - 0.25mm normally
  - Other clearances as applicable per-package
Silkscreen:
- May be omitted only for very small footprints where inclusion would impede close packing or soldering, or for non-functional parts such as mounting holes
- All lines 0.15mm thick (checked automatically)
- Provide pin 1 indicator where applicable
- No silk over exposed copper
- Internal drawings where possible
  - Not for ICs with exposed pads
  - Be careful of situations where the height of the silk could cause soldering issues
  - Placement alignment indications for no-lead packages will need to be external
  - In general prefer less silk visible post-assembly

Associated Documentation

Has the footprint been validated in practice? With what symbol? Where?
Link to any specific layout recommendations or requirements
Any other notes / gotchas

Footprints in unchecked/ have not been standardised or documented yet.

Footprints

0201, 0201-L, 0402, 0402-L, 0603, 0603-L, 0805, 1206

Imperial sized chip device.

Footprints are IPC-7351B compliant
Default NOMINAL environment, -L parts in LEAST environment
Clearance and courtyards are all 0.25mm from the pad edges
Fabrication layer shows typical device and terminal size
Generally all tested in production but are by no means process-optimised

0603-LED

0603 (aka 1.6mm x 0.8mm) sized LED.

Standard 0603 footprint pads
LED polarity arrow with pin 1 as cathode
Farnell codes:
- Red 2290329
- Green 2290328
- Amber 2290330 ("yellow")
- Blue 1686062

0805-LED

0805 (aka 2.0mm x 1.25mm) sized LED.

Standard 0805 footprint pads
LED polarity arrow with pin 1 as cathode
Farnell codes:
- Red 5790840
- Green 5790852
- Yellow 5790876
- Orange 5790864
- Blue 8554749

SOIC, MSOP, LQFP, QFN, DFN, LGA, LPCC, others

Standard footprints, either from IPC-7351B in nominal environments or otherwise modified for a specific package or device.

Generated automatically by scripts/icmod.py. Please see the notes by each footprint in that script for further details.

MICROUSB_MOLEX_47589-0001

MicroUSB connector.

Farnell 1568023
Not tested yet
Bottom mount (so USB cables will be upside down if footprint is on top)
Footprint uses round drill hits for oblong slots
Probably wants hand soldering the through connections

MICROSD_MOLEX_503398-1892

MicroSD card holder.

Farnell 2358234
Used successfully

M3_HOLE, M3_MOUNT

M3 sized mounting holes.

The M3_MOUNT variant includes a no-mask region with extra drill hits for a locking washer.
The M3_HOLE courtyard does not include space for a bolt head or washer (as it may not always be required) so be sure to check this or use the M3_MOUNT variant.