3

In Altium 14.3 how can one define via to via clearance in differential pair routing to produce a different spacing between via to via and track to track?

I defined a design Rule: Electrical->Clearance->ClearenceViaToVia[IsVia,IsVia] to 0.2mm

Because my differential pair routing rule is set to MaxGap 0.15mm Altium violates it in interactive routing mode, which is pretty annoying enter image description here enter image description here

Tom
  • 115
  • 2
  • 9
  • 3
    Do you truly need the 0.2 mm clearance for vias in differential pairs? My solution would be to make a rule for `IsVia And InAnyDifferentialPair` with 0.15 mm clearance. – The Photon Nov 20 '15 at 18:25

1 Answers1

3

I would use the "InDifferentialPairClass" and "IsVia" clauses in Altium:

enter image description here

I haven't tested this, but theoretically if the object is a via and is in a differential pair, then it won't complain unless the clearance is less than 0.15mm.

Just make sure this rule has a higher priority than the original clearance rule (which is currently being broken).

Rev
  • 10,017
  • 7
  • 40
  • 77
DerStrom8
  • 21,042
  • 8
  • 61
  • 95
  • Sorry @ThePhoton , Just read your comment. Didn't mean to steal it – DerStrom8 Nov 20 '15 at 19:02
  • No worries. But it's not clear to me if OP wants a rule that will make the 0.15 mm clearance not be a violation, or if he wants a way to make the interactive router produce 0.2 mm spacing. – The Photon Nov 20 '15 at 19:30
  • I read it as the OP wanting to prevent it from showing as a violation, considering this statement: "Altium violates it in interactive routing mode, which is pretty annoying" – DerStrom8 Nov 20 '15 at 20:13
  • Yes, but that could also mean "the Altium auto-router violates the design rule". – The Photon Nov 20 '15 at 21:22
  • He did not mention autorouting, he mentioned interactive routing so I made the assumption he was running the differential traces and changed layers mid-route to place the vias. It made the most sense to me, but I certainly can't argue. You could very well be right. I'd like to hear a bit more from the OP. – DerStrom8 Nov 20 '15 at 21:33
  • Okay, "the Altium interactive router violates the design rule, and that is annoying." – The Photon Nov 20 '15 at 22:09
  • I need Altium to produce a clearance of 0.2mm from via to via but keep the 0.15mm from track to track. – Tom Nov 21 '15 at 16:34
  • 1
    Ah. In that case, I would just up the "max gap" in the differential pair rules to 0.2mm. I believe then the 0.2mm via-via clearance rule will take over, but as long as the preferred gap is set to 0.15mm then the traces will still be that far apart. Now, just a quick comment on Vias, generally it's good practice for the hole diameter to match the width of the trace and the outer ring to have a diameter 2x the hole diameter (i.e. 0.2mm traces would have 0.2mm diameter holes with 0.4mm outer rings). Otherwise your impedance will increase, and your current-carrying capabilities will decrease. – DerStrom8 Nov 21 '15 at 17:54