The PCB Design Professionals

Rules – 05

Design -> Rules (D R)

The design rules in Altium are very powerful and it would take us an age to type an in depth blog on the rules. So here are a few of the one’s we use.

Polygon Rules

You have to keep an eye on polygon rules  if you use the query helper and select polygon from the object types checks, then the syntax would be ‘ispoly’ we have found that this doesn’t work, instead you can use the syntax ‘inpoly’ to set up rules for clearance checks or direct connects to polygons.

Unused BGA pins Rule

If you have a BGA with unused pins that you still want to fanout to a via. You will get short circuit error between the ‘no net’ pad and ‘no net’ via and track. There is away around that though, you can add another short circuit rule to be as pictured. This should fix those ‘no net’ errors and stop any other short circuits.

Tenting Via’s

Tenting via’s is a neat  little rule and pretty simple too. The rule is under the Mask heading, then Solder Mask Expansion. The syntax for a via is ‘isvia’, the rule is structured as pictured. Just make sure the expansion value is set to at least the minus of your via pad size. (eg. if your via has a 24thou pad then your expansion rule should be -12thou).

Clearance area’s

If you want to set up a specific area on a board to have a smaller clearances than the rest of the board (say for a fine pitch BGA) but you don’t want to extend this clearance over the whole board.  You can use a room  that has been pulled in from the schematic or create a new one from scratch. You can then create a rule similar to the one pictured.

If you would like us to list a rule that’s giving you trouble let us know – blog@blackstick.co.uk