Differential pair ground plane clearance

[kilobytech]

I’m trying to implement a distance between my differential pairs and the ground plane in my PCB layout. Setting a bigger clearance is basically doing what I want. But this has the side effect of throwing DRC errors.

Is there something like a keep out distance which respects the DRC clearance? Or is the only solution for this to manually draw keep out areas around the differential pairs?

[der.ule]

I believe that custom design rules are what you are looking for, unfortunately, I haven’t use them to give a meaningful example.

PCB Editor | master | English | Documentation | KiCad

[fjullien]

This should work:

(rule "dp clearance top"
    (constraint clearance (min 1mm))
    (condition "A.inDiffPair('*') && B.Type == 'Zone' && B.Layer == 'F.Cu'"))

(rule "dp clearance bot"
    (constraint clearance (min 1mm))
    (condition "A.inDiffPair('*') && B.Type == 'Zone' && B.Layer == 'B.Cu'"))

You need to add this rule in your custom rules:

[kilobytech]

Thanks! This does exactly the desired purpose.

Just out of curiosity, what is the difference between setting the clearance with a Custom Rule and via Net Class? Or in other words, why does the Custom Rule not throw a DRC error but the Net class does?

[fjullien]

Net Class clearance is applied between your net and everything else: pads, other nets, vias.
What you want here is a clearance between your nets and only another item.