pcb-rules

Track width/spacing:
===================

Track thickness/clearance
Fab Min: 
	2-layer no BGAs: 5mil (0.127mm). 
	2-layer w/BGA: 4mil/4mil (0.102mm) e.g. STM32F722IEK
	4-layer: 3.5mil (0.09mm) e.g. STM32MP153DAD
	4-layer BGA fan-outs: Can do 3mil (Posin charges extra)
Pref: 
    6mil minimum (.15mm), 8mil if possible (0.2mm)
High current: 
    12mil if possible (0.3mm)

Posin:
 - 0.09mm/0.09mm is OK (example: MetaModule p11)
 - Don't know the minumum they will do but 0.073mm will cost extra (see email May 6, 2022)

JLCPCB: 
 From their Capabilities page:
 - 2layer: 0.1mm/0.1mm min
 - 4layer: 0.09mm/0.09mm min (verifed with mp153-devboard)
 - 4layer: in BGA fan-outs 3mil (0.0762mm) is acceptable


BGA Pad diameter:
================

**Summary:** Unknown... use 0.250 if possible?

Note: P0.5mm with 0.09mm track/space leaves 0.230mm pad

Posin:
 - Don't know minimum, but 0.230mm has been done with MM board (P0.5mm)
 - 0.28mm pad done with DLDs

JLCPCB:
 - BGA pad diameter ≥ 0.25 mm (according to website)
   - But 0.230mm has been done with mp153-devboard (P0.5mm) with no failures so far
 - Same clearance of 0.1mm for 2layer, 0.09mm for 4layer

Vias
====

**Summary:** Prefer 0.3mm hole, 0.6mm diameter. Drop to 0.3mm hole/0.5mm dia if needed. Min 0.15mm hole, 0.25mm diameter.
Need to use laser vias for 0.1mm.

Posin:
 - Min. hole: 0.15mm through all layers
 - Min. laser via 0.1mm hole between L1 and L2 (or L3 and L4)

JLCPCB:
 - website recommends 0.3mm hole, 0.45m diameter
 - charges more for 0.25mm hole, 0.4m diameter
 - charges more for 0.2mm hole, 0.35m diameter
 - charges more for 0.15mm hole, 0.3mm diameter, will go down to 0.25mm diameter

Vias-in-Pads:
============

Posin:
- Can do laser holes on pad. We had lots of failures with a run of these DLDs.(0.28mm pad for P0.5mm, 0.1mm laser via to L2)

JLCPCB:
- from website: "Vias can be placed within BGA pads using filled and plated-over vias" 0.15mm-0.5mm


Silk legends:
============
(Height/Width/Thickness)
Fab Min: 40mil(1mm) min height. 6mil (0.15mm) min line thickness
Pref: 0.040/0.040/0.006 = 1mm/1mm/.15mm
Min legible: 0.024/0.024/0.006 = 0.6mm/0.6mm/.15mm
Bigger and thicker is easier to read, if there’s room.

Distance from Edge Cut to pad or trace:
======================================
Pref: 10mil

Distance between jack and LED w/light pipe
==========================================
(Center to Center):
345mil (8.76mm)

Height and Width of Eurorack PCB:
Height ideal: 4.3" (109.22mm)
Heigh max (if necessary): 4.365" (110.871mm)
Width ideal < width of faceplate (EnsOsc = 2.9mm shorter than faceplate)
Width max = width of faceplate
Minimum distance from edge of PCB to edge of faceplate: 0.347" (8.81mm)