Polygon<>polygon clearance vs. pad <> polygon clearance

[tomex]

Hi everyone,
I have encountered an interesting feature (or a bug) in AD19.0.15 and have no good solution to it.

Pictures are worth a thousand words so I'll try to explain with the help of a few. A rectangular SMD pad is surrounded by polygon like this:

The gap is defined in design rules. However this rule is obviously not obeyed in corners of the pad - the polygon gets rectangular as well as the surrounded pad instead of keeping specified distance and creating radius.

On the other hand, when you place a polygon inside a polygon the rule is obeyed with no exceptions. The corners get rounded as in the picture below.


This creates an ugly design when the SMD pad is a part of a polygon.


This can be solved by defining a rule for polygon <> polygon clearance to be exactly sqrt(2) times the pad <> polygon distance. This, however, solves the aesthetics but creates larger gaps which may be unacceptable.

Any idea how to keep all clearances the same and still produce nice-looking design?

[T3sl4co1l]

Know what's worse?  Check the soldermask layer... in extreme cases you can end up with soldermask openings overlapping the adjacent copper, exposing it!

Easy solution: don't use stupid square pads, they're ugly, their corners don't work right, and probably something about stress or solderability or something, I don't know.  I prefer them for aesthetics if nothing else, but Altium's functionality on square corners is obviously an issue...

If you don't want to go through your libraries, this can be done on the PCB: open PCB Filter, query
IsPad AND (PadShape_AllLayers = 'Rectangular')
go to Properties (older AD: PCB Inspector), change pad shape to Rounded Rectangle, set Pad Corner Radius to say 5-30% (depending on if you want it to look basically square still, but be handled as rounded to get the right corners, or to round it off visibly).

May have to insert additional steps if you have pad stacks in the design, obviously.

BTW, you can do this in the libraries as well, just query and edit the whole library; do set aside some time to inspect everything and make sure it didn't bone anything up, though.  The warning that you "can't undo" the operation is worth heeding.

Tim

[cgroen]

.
BTW, you can do this in the libraries as well, just query and edit the whole library; do set aside some time to inspect everything and make sure it didn't bone anything up, though.  The warning that you "can't undo" the operation is worth heeding.

Tim

Thanks for that one Tim!
I had not noticed the "Filter the whole library" option before!

Regards,
Carsten

[tomex]

Thanks Tim for your reply. I'm using vault-managed libraries so I'm a bit limited in editing those.

Know what's worse?  Check the soldermask layer... in extreme cases you can end up with soldermask openings overlapping the adjacent copper, exposing it!

The soldermask looks alright in my design.

If you don't want to go through your libraries, this can be done on the PCB: open PCB Filter, query
IsPad AND (PadShape_AllLayers = 'Rectangular')
go to Properties (older AD: PCB Inspector), change pad shape to Rounded Rectangle, set Pad Corner Radius to say 5-30% (depending on if you want it to look basically square still, but be handled as rounded to get the right corners, or to round it off visibly).

This is very good tip, thanks. Rounded rectangle with Pad Corner Radius set even to 1% makes the polygon round in corners!

Tomas