Add BGA rule for BGA Pad to Trace Clearance

[SolvedSphinx126]

Adds a new rule to support JLCPCB's BGA spacing as per:
https://jlcpcb.com/help/article/BGA-Design-Guidelines---PCB-Layout-Recommendations-for-BGA-packages

[Cimos]

Hi @SolvedSphinx126,

Thanks for adding. This rule will match for a lot more than the intended BGA pads.

[Cimos]

The 0.1mm clearance is fine for BGA fan-outs, but A.Pad_Type == 'SMD' matches every SMD pad on the board. As written this relaxes pad-to-track clearance to 0.1mm everywhere, not just under the BGA.

Cleanest fix is to scope by net class:

(rule "JLCPCB: BGA to Trace"
    (condition "A.NetClass == 'BGA' && B.Type == 'Track' && A.Net != B.Net")
    (constraint clearance (min 0.1mm))
)

Users then assign the relevant nets to a BGA net class in Board Setup. Only those nets get the relaxed clearance, nothing else changes.

Also worth pinning the 0.1mm value to a specific line in JLCPCB's capabilities/BGA page in a comment above the rule, so it's checkable against future updates.