Regarding Clearances

Layout
1

Hello guys.
We are working on design of power board. in PCB layout I have described different net classes like power and signal. with power netclass has copper to copper clearance of 100mil and signal netclass has clearance of 20mils. now when I am refilling my zones. my power copper plane is taking 100mils clearance from every copper.

  1. i just want 100mil clearance between my power planes. and a different clearance for power to signal copper
  2. second thing i have a 4 pin connector whose two pins are unconnected. although pads have no connection my power plane is still taking a clearance
    Capture
    Capture599×540 46.1 KB

    of 100mil
2

You have to add custom design rules to define the additional clearance between your power nets. It could look something like this:

(version 1)

(rule "Clearance 3.3V 5V"
  (constraint clearance (min 1.5mm))
  (condition "A.NetClass == '3.3V' && B.NetClass == '5V'")
)

Add this for all cases where you want a specific clearance.

Regarding 2: if your power net has a clearance of 100mil then it is also between this net and N/C, because it is also a net (although with no further connections).

3

Thank you ekoeck

for your answer

4

Something like this should work

(rule HV_HV
   # wider clearance between HV tracks
   (constraint clearance (min "3mm + 2.0mm"))
   (condition "A.NetClass == 'HV' && B.NetClass == 'HV'"))

(rule HV_*
   # wider clearance between HV tracks to non-HV
   (constraint clearance (min "3mm + 2.0mm"))
   (condition "A.NetClass == 'HV' && !B.NetClass == 'HV'"))

just change the min distance. I have 3mm + 2mm just as a reminder it takes basic maths, I am happy with 5mm to anything

1 Like