0
\$\begingroup\$

I imported PCB design files into Altium from Allegro.

I noticed that some of the vias look like the following, where blue is the GND polygon, and the GND net via does not connect to it at all.

The same is seen for thr +3v3 net (seen in yellow) where the via once again does not seem to connect to the polygon at all.

In both these instances there seem to be 4 tracks from these vias, it's almost as if the relief connects from Allegro have been imported incorrectly into Altium. Does anybody have any good idea on how to resolve this issue?

enter image description here

enter image description here

\$\endgroup\$
5
  • \$\begingroup\$ These are AGND net vias. Is the blue pour GND or AGND? \$\endgroup\$
    – user253751
    Aug 15, 2022 at 19:54
  • \$\begingroup\$ @user253751 the naming is AGND on both. \$\endgroup\$
    – user1084113
    Aug 15, 2022 at 20:05
  • 2
    \$\begingroup\$ Is "pour over same net polygons only" or "pour over all same net objects" selected? \$\endgroup\$
    – vir
    Aug 15, 2022 at 20:13
  • 1
    \$\begingroup\$ Yup, @vir I've been playing around with repouring over the same net objects, and that seems to connect the plane to the vias, however the tracks that were created from the import seem to remain and the copper looks very odd. In addition, I'm not sure if I have inadvertently changed any of the traces using this method, certainly a work around but doesn't seem to be ideal. Thank you. \$\endgroup\$
    – user1084113
    Aug 15, 2022 at 20:27
  • 1
    \$\begingroup\$ You'll probably have to manually delete all the little bits of track.... A perfect "import" is something that's likely never going to happen with any software. It'll get you 98% of the way there, you have to be alert and fix whatever doesn't import right. \$\endgroup\$
    – Kyle B
    Aug 15, 2022 at 20:58

1 Answer 1

Reset to default
0
\$\begingroup\$

I use Altium on a daily basis, but haven't used Allegro since college. That said, I am fairly certain that the way the two softwares manage polygons is fundamentally different. After having to convert multiple allegro designs into Altium, I have yet to discover a way to connect traces and polygons of the same net unless you give up thermal relief by selecting "Pour over all same net objects" -no matter what settings you use. I could be missing something, but if I am it is not apparent (perhaps some scripting in the design rules would do, I haven't tried). Polygon manipulation is rather basic compared to Allegro, where everything is rather intuitive. Allegro has no qualms about letting you connect traces to polygons. In practice this means that you have different design philosophies, both of which make the same board, but converting from one to the other a pain, especially with hundreds of thermal reliefs (or if you don't have a copy of Allegro on your Altium machine, then you can't convert at all)

Practically, your best bet is to delete all the traces and then use Altium's rules to make auto generated 45° thermal reliefs. As stupid as that sounds.

Please somebody prove me wrong.

\$\endgroup\$
3
  • 1
    \$\begingroup\$ Altium has no problems connecting traces and polygons, it's simply whether you have "pour over all same net objects" selected in the polygon properties. And if the objects match (which it looks like they would here). Evidently they didn't import that way, for whatever reason. The extra trace stubs could be filtered say by matching TraceLength and then deleted to use pour rules instead. \$\endgroup\$
    – Tim Williams
    May 26 at 21:29
  • 1
    \$\begingroup\$ As I recall from the one Allegro import I've handled, the bigger problem is the polygons import as-poured, clearance and all. So you either have to delete vast swaths of vertices to get it to pour by rule again, or start over and draw new ones. Which, isn't always a pain, but depending on the design, it can be. \$\endgroup\$
    – Tim Williams
    May 26 at 21:31
  • 1
    \$\begingroup\$ I've been spending some time on this problem again, and one thing I just rediscovered is if you go into the clearance design rules under constraints select "Different Nets Only" and then selecting poor over all same net objects works... somewhat. If you have overlapping polygons with different nets, they don't seem to care about each other for instance \$\endgroup\$
    – Songbird
    May 26 at 21:50

Your Answer

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

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