I have a polygon reaching to the outside of the board. There I want to place mousebites for the panel, but when they are placed, there is a clearance generated around the holes that I don't want:

Hole Clearance

Where do I need to set up a custom rule in the design rules?

I tried this, but without luck:

Design Rules



  • \$\begingroup\$ You’ve set a rule for polygon to pad clearance but your question is about polygon to hole clearance. That’s another constraint. \$\endgroup\$ Apr 10, 2023 at 22:47
  • \$\begingroup\$ Yes, because in Altium there is no "hole" just by itself. You generate one as a "pad" but without any copper. I updated the post with a picture. \$\endgroup\$
    – Creatronik
    Apr 11, 2023 at 12:01
  • \$\begingroup\$ What is the rule's precedence? \$\endgroup\$ Apr 11, 2023 at 12:08
  • \$\begingroup\$ @TimWilliams Do you mean the priority? I set this to highest. \$\endgroup\$
    – Creatronik
    Apr 11, 2023 at 12:18

1 Answer 1


I was able to make this work with the following rule setup:

enter image description here

The first condition 'InPoly' is, I think, the correct way to match polygons in the design rules. I'm not an expert in Altium's query language, but I was able to get the 'InPoly' condition to work and not the 'ObjectKind=' from your screenshots. I believe it may be because the ObjectKind queries return the objects and not the child primitives.

Likewise, the second condition required the condition 'HasFootprint' and then the name of my mousebite footprint. In my library, they're called 'MOUSE BITES', but that would need to be updated to match whatever your footprint name is. It's also likely that the singular query string "Name='Free-Mousebites'" or "Designator='Mousebite'" would result in a successful match for the second condition.

  • \$\begingroup\$ Great! Thank you. And as I had other holes in the layout, I changed the Query to match with pads with 0mm pad expansion. \$\endgroup\$
    – Creatronik
    Apr 12, 2023 at 11:25

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.