9
\$\begingroup\$

In Altium, when I draw a polygon, it automatically leaves a gap around copper of a different net. However, my Vin net is high voltage, and needs to have a 1mm clearance. Therefore, If I draw a Vin polygon, it needs to leave a 1mm clearance between itself and other nets. And if I draw a polygon of another net over a Vin via, then, again, it needs to leave a 1mm clearance.

I have tried setting the design rules, but to no avail.

How do I get polygon to automatically leave 1mm clearance when one of the two nets is Vin?

Polygon Clearance Design Rules

\$\endgroup\$
  • 2
    \$\begingroup\$ Have you tried Altium support? \$\endgroup\$ – Leon Heller Oct 24 '11 at 16:08
  • \$\begingroup\$ In the 'Where The First Object Matches' try and select 'Net' and then choose the 'VIN' net from the drop-down menu. Afterwards, try repouring the polygon. Also, The priority of 'PlaneClearence_1' rule must be higher than the priority of 'PlaneClearence' \$\endgroup\$ – m.Alin Oct 24 '11 at 16:46
  • 1
    \$\begingroup\$ @LeonHeller Maybe he doesn't have a license :) \$\endgroup\$ – m.Alin Oct 24 '11 at 16:52
  • 1
    \$\begingroup\$ Yes Leon, we do have a License. But Altium have recently messed about with their (already irritating) forum, and I can't seem to log on any more. \$\endgroup\$ – Rocketmagnet Oct 24 '11 at 16:57
8
\$\begingroup\$

Polygons in Altium are tricky.

The solution to your problem is to use the rule InPolygon instead of IsPolygon.

As I understand it, Altium treats polygons as kind of a "meta" descriptor, internally. A "Polygon" object contains the polygon outline. The outline itself is matched with the InPolygon rule (which is what you want).

This is of course made far more obnoxious by the fact that IsPolygon is a valid rule token, so your rule will seem to be correct, and even pass the rule-checker, but silently fail when you try to actually repour the polygon, since the IsPolygon rule matches against something else.


Also, from your included image, you are trying to make a Power Plane Clearance rule affect a polygon. I think you may need to change that to a Clearance rule (Under the Electrical grouping in the rules window, since Altium's polygons are not planes.

This is off the top of my head, ATM. It's been a while since I needed varying plane clearances in Altium


Don't ask how long it took me to figure this out myself....

Oh, as an aside, placing polygons over polygons can have interesting effects, since which polygon is held-back due to the rules is dictated by the pour order. Subsequently, if you modify your layout, and run a command like Repour Violating, your can wind up with your polygons in a odd state, where a subsequent full Repour will change the overall polygon outline, even though the polygons already were passing the design rules.

\$\endgroup\$
  • 1
    \$\begingroup\$ I can confirm that your vauge memories are correct. It needs to be a regular clearance rule (not power plane clearance) and it needs to be InPolygon \$\endgroup\$ – Peter Green Sep 12 '16 at 12:13
  • \$\begingroup\$ And you should also remember to make your specific clearance rules (e.g. this polygon one) higher priority than your generic clearance rule. \$\endgroup\$ – Peter Green Sep 12 '16 at 12:16
4
\$\begingroup\$

If the gap between your Vin net and anything else needs to be 1mm, just put InNet('VIN')
Make sure the rule is higher in priority than any default rule. The polygon should go green (as it flags it being too close), then repour and the clearance should now be 1mm.

\$\endgroup\$
1
\$\begingroup\$

Maybe you it helps to set the clearance attribute instead of power plane clearance (however I doubt this will offer the solution)

Otherwise create a seperate room over the wanted area and use validations for your (top? bottom?) layer and that room (InRoom I believe), and the clearance higher.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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