1
\$\begingroup\$

Background

I'm fanning out and routing controlled impedance tracks underneath a BGA. The stack-up predetermines that a 50 Ohm track must be 121 um (~5 mil) wide on a given internal layer. This, however will not fit between two vias, where my minimum clearance design constraint dictates 100 um (~4 mil) track widths.

The solution to this is to reduce the track width to 100 um (~4 mils) between the vias. The image below illustrates the problem: the middle track is 100 um (~4 mils) wide throughout, the tracks on either side of it neck down only where necessary.

Alternating track widths between vias

Corresponding design rules

Problem

Creating this alternating track width pattern only seems to be possible if done manually.

Question

Is it possible to make Altium dynamically switch between minimum and preferred track widths depending on the available space around the track? In other words can I make Altium use the preferred width where possible and resort to using the minimum width where necessary?

\$\endgroup\$

1 Answer 1

3
\$\begingroup\$

The stack-up predetermines that a 50 Ohm track must be 121 um (~5 mil) wide on a given internal layer.

The vias in your image can be made to have a smaller diameter copper on inner layers thus, the 5 mil track will easily fit through. Not all PCB software supports this type of pad-stack arrangement (for through-hole pads) but, Altium does I believe. So does PADs and OrCAD. I don't believe KiCAD does though.

So, my suggestion is, forget your question for now and make life easier for yourself by having the via copper a smaller diameter on inner layers.

\$\endgroup\$
10
  • 1
    \$\begingroup\$ There are 2 ways of doing this in Altium, 1st is removing the inner layer pad: Tools > Remove unused pad shapes > Vias/Remove unused. Alternatively, its possible to edit the via stack "Top-Mid-Bottom" or Full-Stack (edit each layer). \$\endgroup\$
    – Wesley Lee
    May 2, 2022 at 14:17
  • 2
    \$\begingroup\$ There are discussions whether removing the pads is better or worse for PCB reliability but I could never find a conclusive answer. (i.e. can be better in some aspects and worse in others) \$\endgroup\$
    – Wesley Lee
    May 2, 2022 at 14:18
  • 1
    \$\begingroup\$ KiCad sort of supports that as of version 6, actually--you can set a via to only have a pad on layers where things connect to it, and no pad on layers where they don't. The feature still has a couple bugs last I checked. I think they plan to have full custom pad stacks in version 7. \$\endgroup\$
    – Hearth
    May 2, 2022 at 14:51
  • 1
    \$\begingroup\$ @Andyaka Yes, it's a new feature in version 6. \$\endgroup\$
    – Hearth
    May 2, 2022 at 15:00
  • 1
    \$\begingroup\$ @pfabri - Minimum annular ring is for layers where there is a connection to copper and the drill has to "match" the ring. If there is no connection in that layer, there is no need for copper, so the via can be plated as a regular through hole (i.e. no annular ring at all). I suggest you ask your fab house if it is acceptable to remove unused via connections. I've done that with a few different manufacturers with no issues. \$\endgroup\$
    – Wesley Lee
    May 2, 2022 at 15:23

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.