1
\$\begingroup\$

In Altium PCB designer I have setup the following default clearance design rules:

enter image description here

At the beginning I had this rule to be applied only to different nets but I later realized I need to have some rules for objects of the same net. Mainly to have a minimum distance between vias and pads of the same net.

So I then changed this rule to be applied for any net. Although this achieved what I wanted, it also created thousands of new violations that are mainly related to not having enough distance between a via and a track of the same net. See for example the images below. The first one shows all new violations that came after I changed the rule and the second shows one example of "false" violation:

enter image description here

enter image description here

However this is totally wrong, since in this case the track in intentionally connected to the via. However Altium thinks this violates the design rules.

Which of course makes somehow sense. I mean by following blindly the rules set, the tool should indeed raise these violations.

But then the question is how to achieve what I want without having all these "false" violations that appear where there is basically short-circuit / correct connection between track segments or track and pad or track and via.

\$\endgroup\$
7
  • \$\begingroup\$ When it comes to Altium rules, less is more. Trim down your rules as much as possible and simplify \$\endgroup\$
    – DerStrom8
    Commented Dec 1, 2017 at 15:24
  • \$\begingroup\$ OK, I would agree with you. But what do you mean specifically in this case? The only rule that applies is the default rule. The other with higher priority are not applicable, if that's what you meant. \$\endgroup\$
    – nickagian
    Commented Dec 1, 2017 at 15:27
  • 1
    \$\begingroup\$ Your screenshot doesn't show a special rule for vias and pads. It shows a rule for any copper to any other copper. If you want a special rule for vias and pads, make a rule restricted to vias and pads, and make that rule apply to same nets. \$\endgroup\$
    – The Photon
    Commented Dec 1, 2017 at 16:58
  • \$\begingroup\$ @ThePhoton Yeah, that is exactly what I need. But I don't know how to do it? Is that intuitive? Except you mean restrict the first object in the rule to, let's say via, and the second object, let's say pad. Well, now that I think of it that should work... \$\endgroup\$
    – nickagian
    Commented Dec 1, 2017 at 17:03
  • 1
    \$\begingroup\$ 1. Create new rule. 2. Change where the first object matches to "IsVia" 3. Change where the second object matches to "IsPad" 4. Adjust the clearance value as required. 5. Put the new rule priority just above the default rule. \$\endgroup\$
    – The Photon
    Commented Dec 1, 2017 at 17:05

1 Answer 1

Reset to default
2
\$\begingroup\$

As "The Photon" suggested, the situation can be solved by creating a special rule targeting specific only vias and pads or vias and vias of the same net. For example something like the rule shown below enter image description here

\$\endgroup\$

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.